[title] Supported operations on expressions [path] G-code/Macro programming/ # Unary operations | **Operation** | **Description** | | ------------- | --------------------------------------------------------- | | abs | Absolute Value | | acos | Arc cosine | | asin | Arc sine | | atan\[y]\[x] | Arc tangent | | cos | Cosine | | exp | e raised to | | fix | Round down | | fup | Round up | | int | Integer part | | ln | Natural log of | | round | Round | | sin | Sine | | sqrt | Square root | | tan | tangent | | not | Logical not | | ResetModulo | \[A\|B\|C] reset a rotation axis to its modulo position | # Binary Operations | **Operation** | **Description** | | ------------- | ------------------------ | | / | Divided by | | mod | Modulo | | \*\* | Power | | \* | Times | | and | Logic AND | | xor | Logic exclusive OR | | - | Minus | | or | logic nonexclusive OR | | + | Plus | | > | Greater then | | >= | Greater than or equeal | | \< | Less then | | \<= | Less than or equal | | == | Is equel | | \<> | Not equeal | | band | Bitwise AND | | bxor | Bitwise exclusive OR | | bor | Bitwise nonexeclusive OR | | \<\< | Shift left | | >> | Shift right | # Example This example drills holes at a circle with a radius of 10, each 30 degrees. The code that performs this is put in a subroutine, which can be called as many times as needed in the main program. :::BlockQuote sub do\_circle\_holes \#100=0 g0 z1 x0 y0 while \[#100 \<> 360] \#102 = \[10 \* sin\[#100]] \#103 = \[10 \* cos\[#100]] g0 x\[#103] y\[#102] g1 z-1 g1 z1 \#100 = \[#100 + 30] if \[#100 == 360] msg "Done" else msg "processing at angle "#100 endif endwhile endsub gosub do\_circle\_holes M30 ::: [title] M0, M1, M2, M30, M60 (Program Stopping and Ending) [path] G-code/Supported M-codes/ To temporarily halt a running program, program `M0`. If a program is stopped by an `M0`, pressing the cycle start button will restart the program at the following line, so the program will continue. To optionally halt a program when the stopM1 feature is enabled in the user interface, please use the `M1` command. Command `M30` results in: - The selected plane is set to CANON\_PLANE\_XY (like `G17`). - Distance mode is set to MODE\_ABSOLUTE (like `G90`). - The feed rate mode is set to UNITS\_PER\_MINUTE (like `G94`). - Feed and speed overrides are set to ON (like `M48`). - Cutter compensation is turned off (like `G40`). - The spindle is stopped (like `M5`). - The current motion mode is set to G\_1 (like `G1`). - Coolants are turned off (like `M9`). - The program is rewinded to the first line, ready for the next start. - All 3D printer heating OFF. Note that the coordinate systems are not reset when M30 is issued. Program `M60` instead of `M30` if the spindle and coolants should remain on, which is useful with nesting. ### **** [title] System parameters/Variables [path] G-code/Language standard/ In the RS274/NGC language view, a machining center maintains 5999 numerical parameters. They can be accessed by #1 .. #5999. The specific parameters with a dedicated function are listed in the table below. Other parameters in the range of 1..5999 are free to use in your G-Code program. Some of them have a special function and are read-only; see the table below: \**parameters in italics are read-only* | Parameter Number | Purpose | | ---------------------------------------------- | ----------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- | | *1 - 26\** | Used for **parameters **when overriding m-functions.
In the g-code there is e.g. `M999 X100 S1000`
And you have in your macro.cnc:
:::BlockQuote Sub m999 msg “this is my m999 X=”#24” S=”#19 Endsub :::
Inside the subroutine, the given X and S parameters are at #24 and #19
#1-#26 = A – Z parameter value.
Values are negative -1e10 if not provided with `m999` in this example. | | 27 - 4999 | **Free to use**, note that 4995 – 4999 are used by the tool length measurement function under user button 2.
`Z#4996` safe height for tool measurement above the fixed tool setter. `x#4997` `y#4998` fixed tool setter position. `z#4999` chuck height, or zero length tool height, chuck just touches the fixed tool setter at this height. `Z#4995` is used for the tool setter height for zeroing Z under user button 1. | | 4000 - 4999 | Free to use, **persistent**, see above some of these are used by tool length measurement and zeroing. | | *5001 - 5006\** | Position of X – C, interpreter position = work position | | *5008\** | Current tool number | | *5009\** | Current tool radius | | *5010\** | Current tool Z offset (length + zDelta) | | *5011\** | New tool number during tool change (M6) | | *5012\** | Current tool X offset (X offset + xDelta) | | *5013\** | Current G43 Z offset (Z offset + zDelta) | | *5014\** | Current G43 X offset (X offset + xDelta) | | 5015 - 5050 | Used in tool change sub routine | | *5051 - 5056\** | Probe position X - C in machine coordinates | | *5061 - 5066\** | Probe position X - C in work coordinates | | *5067\** | 1 if the probe is triggered after `G38.2`, 0 otherwise | | *5068\** | Current probe value | | *5069\** | Handwheel counter | | *5070\** | Spindle rate in rev/second | | *5071 - 5076\** | Position of X - C, interpreter position without offsets = machine position | | *5081 - 5086\** | Probe position X - C in joint coordinates | | *5101 - 5106\** | MCA negative limit X - C | | *5111 - 5116\** | MCA positive limit X - C | | *5121 - 5126\** | Home position X - C | | *5131 - 5133\** | TCA negative limit X - Z | | *5141 - 5143\** | TCA positive limit X - Z | | *5150\** | Active kinematics type:
1: Trivial 2: 4\_AX\_ACYLINDER (Y -> A mapping) 3: Virtual C 4 - 17: System reserved 18 - 30: Custom 1 – Custom 12 | | *5151\** | ZHC is active | | *5152\** | 1 if the spindle is on, 0 if the spindle is off. | | *5161 - 5166\** | G28 home X - C | | *5181 - 5186\** | G30 home X - C | | *5190\** | G68 rotation method (0 = off, 1 = on) | | *5191 - 5193\** | G68/G51 rotation point X - C | | *5194\** | G68 rotation angle XY | | *5195\** | G68 rotation angle YZ | | *5196\** | G68 rotation angle XZ | | *5200\** | 0 if G51 scaling is off, 1 if G51 scaling is on | | *5204\** | G51 scaling factor X | | *5205\** | G51 scaling factor Y | | *5206\** | G51 scaling factor Z (always 1.0) | | 5211 - 5216 | G92 offset X - C | | 5220 | Coordinate system number | | 5221 - 5226 | Coordinate system 1 X - C | | 5241 - 5246 | Coordinate system 2 X - C | | 5261 - 5266 | Coordinate system 3 X - C | | 5281 - 5286 | Coordinate system 4 X - C | | 5301 - 5306 | Coordinate system 5 X - C | | 5321 - 5326 | Coordinate system 6 X - C | | 5341 - 5346 | Coordinate system 7 X - C | | 5361 - 5366 | Coordinate system 8 X - C | | 5381 - 5386 | Coordinate system 9 X - C | | *5390\** | Spindle selection 0 = M90, 1 = M91, 2 = M92 | | *5391 - 5393\** | Alternative spindle offset X- Z | | *5394 - 5397\** | Spindle speed max M90 - M93 | | 5230, 5250, 5270, 5290, 5310, 5330, 5350, 5370 | Reserved for rotation coordinate system | | *5380\** | Simulation mode, 0: controller connected, 1: simulation mode | | *5397\** | Running mode, 0: running, 1: rendering
Use e.g. if you have `G38.2` movements in your macro file because during rendering `G38.2` always runs until the given end point which may give incorrect tool measurement results. Always take care that the tool table contains (approx.) correct tool data | | *5398\** | Return value of `dlgmsg` (1 = OK, -1 = Cancel) | | *5399\** | Return value for `M55`, `M56` | | 5401 - 5499 | Tool Z offset (length) for tools 1 - 99 | | 5501 - 5599 | Tool diameter for tools 1 - 99 | | 5601 - 5699 | Tool X offset (for lathe) for tools 1 - 99 | | 5701 - 5799 | Tool orientation (for turning) for tools 1 - 99 | | 5801 - 5899 | Tool X delta due to wear | | 5901 - 5999 | Tool Z delta due to wear | ** [title] G40, G41, G41.1, G42, G42.1 (Cutter Radius Compensation) [path] G-code/Supported G-code/ To turn cutter radius compensation off, program `G40`. It is OK to turn compensation off when it is already off. Cutter radius compensation may be performed only if the XY plane is active. To turn cutter radius compensation on the **left** (i.e., the cutter stays to the left of the programmed path when the tool radius is positive), program `G41 D...`. To turn cutter radius compensation on the **right** (i.e., the cutter stays to the right of the programmed path when the tool radius is positive), program `G42 D...`. The D-word is optional; if there is no D-word, the radius of the tool currently in the spindle will be used. If used, the D number should normally be the slot number of the tool in the spindle, although this is not required. It is OK for the D number to be zero; a radius value of zero will be used. It is an error if: - The D number is not an integer, is negative or is larger than the number of car­ousel slots - The XY-plane is not active or for turning the ZX plane is not active - Cutter radius compensation is commanded to turn on when it is already on. The behavior of the machining center, when cutter radius compensation is on, is described in Appendix A. With `G41.1 D...` is the same as `G41 D...` except now the D number is not a tool number but a tool diameter. With `G42.1 D...` is the same as `G42 D...` except now the D number is not a tool number but a tool diameter. ### Example code for milling This example mills out a rectangular object from the outside and inside. On the outside, we use G42, tool radius compensation right and for the inside G41, tool radius compensation left is used. For both contours, a tool-radius-compensation entry move is programmed consisting of a line that must be longer than the tool-radius used and a circle, of which also the radius is bigger than the tool. As a side note, all arc radii should be bigger than the tool radius. If you have inside corners, there should always be an arc, so that the tool fits. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/kW9Z8PLEhilnZ_fNIfgRy_image.png" size="54" width="373" height="339" caption="Milling Example 1" position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/kW9Z8PLEhilnZ_fNIfgRy_image.png"} The G42, G41, and G40 codes are programmed with a / (block delete sign) in front. This makes it easy to debug tool comp programs. The program is loaded with the block delete, this is the blue curve. Then the program is run with block delete off resulting in the yellow curve. It is clear to see what the entry move does. :::BlockQuote g0 z3 g0 x-15 y15 f500 /g42.1 D6 g1 x-5 (cutter comp entry move 1) g2 x0 y10 r5 (cutter comp entry move 2) g1 z-3 (plunge down) g3 x10 y0 r10 g1 x70 g3 x80 y10 r10 g1 y90 g3 x70 y100 r10 g1 x10 g3 x0 y90 r10 g1 x0 y10 /g40 g0 z3 g0 x30 y30 /g41.1 d6 g1 x20 g3 x10 y20 r10 g1 z-3 g3 x20 y10 r10 g1 x60 g3 x70 y20 r10 g1 y80 g3 x60 y90 r10 g1 x20 g3 x10 y80 r10 g1 y20 /g40 g0 z3 m30 ::: ## Example Code for Turning The movement starts at the right upper corner. The blue line is the programmed contour. The yellow is the contour with tool-radius compensation G41. The first G1 line is the tool comp entry move. You can get this figure by putting a / character in front of the G41/G40 codes. The load the program with block delete on and execute it with block delete off. With block delete on the tool comp is skipped. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/ISNFknuk7W3z_gLvrD3dl_image.png" size="54" width="513" height="437" caption="Turning Example 1" position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/ISNFknuk7W3z_gLvrD3dl_image.png"} The G42, G41, and G40 codes are programmed with a / (block delete sign) in front. This makes it easy to debug tool comp programs. The program is loaded with the block delete, this is the blue curve. Then the program is run with block delete off resulting in the yellow curve. It is clear to see what the entry move does. :::::Tabs ::::Tab{title="Diameter / R arcs"} :::BlockQuote (Radius programming) (Use I,K programming for arc’s) g0 x-10 z20 /g41.1 d5 g1 x-10 z10 g3 x0 z0 i10 k0 g1 x10 g2 x20 z-10 i0 k-10 g1 z-20 g3 x30 z-30 i10 k0 /g40 m30 ::: :::: ::::Tab{title="Diameter / I,K arcs"} :::BlockQuote (Diameter programming) (Use I,K programming for arc’s) g0 x-20 z20 /g41.1 d5 g1 x-20 z10 g3 x0 z0 i10 k0 g1 x20 g2 x40 z-10 i0 k-10 g1 z-20 g3 x60 z-30 i10 k0 /g40 m30 ::: :::: ::::Tab{title="Radius / R arcs"} :::BlockQuote (Radius programming) (Use R word for arc’s) g0 x-10 z20 /g41.1 d5 g1 x-10 z10 g3 x0 z0 r10 g1 x10 g2 x20 z-10 r10 g1 z-20 g3 x30 z-30 r10 /g40 m30 ::: :::: ::::Tab{title="Radius / I, K arcs"} :::BlockQuote (Radius programming) (Use I,K programming for arc’s) g0 x-10 z20 /g41.1 d5 g1 x-10 z10 g3 x0 z0 i10 k0 g1 x10 g2 x20 z-10 i0 k-10 g1 z-20 g3 x30 z-30 i10 k0 /g40 m30 ::: :::: ::::: [title] G2, G3 (Arc at Linear Feed) [path] G-code/Supported G-code/ A circular or helical arc is specified using either G2 (clockwise arc) or G3 (counterclockwise arc). The axis of the circle or helix must be parallel to the X, Y, or Z-axis of the machine coordinate system. The axis (or, equivalently, the plane perpendicular to the axis) is selected with [**G17, G18, G19 (Plane Selection)**](docId\:Uo-PghD6GWTJ4p9XJ2NzP) (Z-axis, XY-plane), [**G17, G18, G19 (Plane Selection)**](docId\:Uo-PghD6GWTJ4p9XJ2NzP) (Y-axis, XZ-plane), or [**G17, G18, G19 (Plane Selection)**](docId\:Uo-PghD6GWTJ4p9XJ2NzP) (X-axis, YZ-plane). If the arc is circular, it lies in a plane parallel to the selected plane. If a line of RS274/NGC code makes an arc and includes rotational axis motion, the rotational axes turn at a constant rate so that the rotational motion starts and finishes when the XYZ motion starts and finishes. Lines of this sort are hardly ever programmed. If cutter radius compensation is active, the motion will differ from what is described here. See Appendix A. Two formats are allowed to specify an arc. We will call these the center format and the radius format. In both formats, the G2 or G3 is optional if it is the current motion mode. ## Radius Format Arc In the radius format, the coordinates of the endpoint of the arc in the selected plane are specified, along with the radius of the arc. Program `G2 X... Y... Z... A... R...` (or use G3 instead of G2) where R is the radius. The axis words are all optional except that at least one of the two words for the axes in the selected plane must be used. The R number is the radius. A positive radius indicates that the arc turns through 180 degrees or less, while a negative radius indicates a turn of 180 degrees to 359.999 degrees. If the arc is helical, the value of the endpoint of the arc on the coordinate axis parallel to the axis of the helix is also specified. It is not good practice to program radius format arcs that are nearly full circles or are semicircles (or nearly semicircles) because a small change in the location of the endpoint will produce a much larger change in the location of the center of the circle (and, hence, the middle of the arc). The magnification effect is large enough that rounding errors in a number can produce out-of-tolerance cuts. Nearly full circles are outrageously bad, semicircles (and nearly so) are only very bad. Other size arcs (in the range of tiny to 165 degrees or 195 to 345 degrees) are OK. Here is an example of a radius format command to mill an arc: `G17 G2 x10 y15 r20 z5`. That means to make a clockwise (as viewed from the positive Z-axis) circular or helical arc whose axis is parallel to the Z-axis, ending where X=10, Y=15, and Z=5, with a radius of 20. If the starting value of Z is 5, this is an arc of a circle parallel to the XY plane; otherwise, it is a helical arc. ## Center Format Arc In the center format, the coordinates of the endpoint of the arc in the selected plane are specified along with the offsets of the center of the arc from the current location. In this format, it is OK if the end point of the arc is the same as the current point. It is an error if: - When the arc is projected on the selected plane, the distance from the current point to the center differs from the distance from the endpoint to the center by more than 0.0002 inches (if inches are being used) or 0.002 millimeters (if millimeters are being used). When the XY-plane is selected, program `G2 X... Y... Z... A... I... J...` (or use G3 instead of G2). The axis words are all optional except that at least one of X and Y must be used. I and J are the offsets from the current location (in the X and Y directions, respectively) of the center of the circle. I and J are optional except that at least one of the two must be used. It is an error if: - I and J are both omitted. When the XZ-plane is selected, program `G2 X... Y... Z... A... I... K...` (or use G3 instead of G2). The axis words are all optional except that at least one of X and Z must be used. I and K are the offsets from the current location (in the X and Z directions, respectively) of the center of the circle. I and K are optional except that at least one of the two must be used. It is an error if: - I and K are both omitted. When the YZ-plane is selected, program `G2 X... Y... Z... A... B... C... J... K...` (or use G3 instead of G2). The axis words are all optional except that at least one of Y and Z must be used. J and K are the offsets from the current location (in the Y and Z directions, respectively) of the center of the circle. J and K are optional except that at least one of the two must be used. It is an error if: - J and K are both omitted. Here is an example of a center format command to mill an arc: `G17 G2 x10 y16 i3 j4 z9` That means to make a clockwise (as viewed from the positive z-axis) circular or helical arc whose axis is parallel to the Z-axis, ending where X=10, Y=16, and Z=9, with its center offset in the X direction by 3 units from the current X location and offset in the Y direction by 4 units from the current Y location. If the current location has X=7, Y=7 at the outset, the center will be at X=10, Y=11. If the starting value of Z is 9, this is a circular arc; otherwise, it is a helical arc. The radius of this arc would be 5. In the center format, the radius of the arc is not specified, but it may be found easily as the distance from the center of the circle to either the current point or the endpoint of the arc. [title] Mapping X/Y G-code to cylinder on A-Axis [path] How to use/ ### Mapping X/Y G-code to cylinder on A-Axis This is useful if you have a 4th axis and want to mill on the outside of a cylinder as if it were the X-Y plane. You must have set up the A axis as “4THMILL”. This is possible with a normal XY G-Code file. EdingCNC will perform the mapping for you. Some calibration needs to be done to make this work. It is done on the coordinates page. The location of the A-axis rotation point needs to be set and also the radius of the workpiece needs to be set first. ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/rsc9LeI7XE-A9Ixcek6vo_screenshot-coordinate-tab-with-5th-axis-milling.jpg) **First, we set the location of the A rotation point:** We move by jogging or MDI to the center point of rotation of the A axis, only Z and Y are important here. Press button "**1. Set to current position**". Done, center is set. **Next, we set the outside radius of the workpiece:** There are *two *possibilities to do this: 1\. Just type the radius if you know it and press "**Set Radius**" 2\. We move the Z up touch the outside of the material with the tool bit and press "**Calibrate Radius**". Calibration is done. First, we need to be sure that our Y axis is at the correct position before we switch on the Y->A mapping. We need to do this now because when the mapping is ON, Y can no longer be moved, as Y is now mapped to A. You can press "**Move Y to rotation point**” to do the movement. The mapping can be switched ON now. Then, we can load a standard G-Code file with XYZ coordinates. Below, we see how it looks in the graphic. Position the X and the Z at the zero point of the drawing, so where the milling should start. Now Zero all axes in the **Operate **screen :::hint{type="info"} Important: Zero the Z at the top surface of the cylindric material, in this case, the material has a radius of 20 mm, so the Z zero is 20 mm higher than the CenterPoint. ::: **Y to A mapping OFF** //IMAGE of flat picture.... **Y to A mapping ON** [title] M6 (Tool Change) [path] G-code/Supported M-codes/ To change a tool in the spindle from the tool currently in the spindle to the tool most recently selected (using a T word - see Section 3.7.3), program `M6`. When the tool change is complete: - The spindle will be stopped. - The tool that was selected (by a T word on the same line or on any line after the previous tool change) will be in the spindle. The T number is an integer giving the changer slot of the tool (not its id). - If the selected tool was not in the spindle before the tool change, the tool that was in the spindle (if there was one) will be in its changer slot. - The coordinate axes will be stopped in the same absolute position they were in before the tool change (but the spindle may be re-oriented). - No other changes will be made. For example, coolant will continue to flow during the tool change unless it has been turned off by an M9. The tool change may include axis motion while it is in progress. It is OK (but not useful) to program a change to the tool already in the spindle. It is OK if there is no tool in the selected slot; in that case, the spindle will be empty after the tool change. If slot zero was last selected, there will definitely be no tool in the spindle after a tool change. The tool change command will call the `change_tool` subroutine inside *macro.cnc*. You can adapt the behavior for your own needs in this function e.g: - Perform automatic tool-length measurement - Perform tool change with an automatic tool changer. For a (non-functional) example of how to implement automatic tool change for a 16-tool changer. see the contents of the *default\_macro.cnc *file at the end of this document. It checks whether the current tool is already in the spindle. It checks that the tool number is in the range of 1-4. Then it first drops the current tool and picks the new tool: [title] M54, M55, M56, M57 (General purpose IO) [path] G-code/Supported M-codes/ :::hint{type="warning"} Please note that mentioned commands may fail during loading and/or simulation. To make your macro code avoid these errors please take a look at the manual section [**Run behavior during loading of job file and simulation**](docId\:p2Jh9fFRvp0WCb5jCD9px) ::: ## Digital outputs ### Set output - M54 P*... * The P word must be between `1` and `10` where `1` is *AUX1* and `10` is *AUX10*. :::BlockQuote M54 P1 (set AUX1 out to 1) ::: If the connected controller only has one AUX output, `2` is mapped to *FLOOD *and `3` to *MIST*. :::BlockQuote M54 P2 (set AUX2 out to 1 or FLOOD to 1 if the controller has 1 AUX) ::: *** ### Clear output - M55 P*...* Clear output. The P word must be between `1` and `10` where `1` is *AUX1* and `10` is *AUX10*. :::BlockQuote M55 P1 (set AUX1 out to 0) ::: If the connected controller only has one AUX output, `2` is mapped to *FLOOD* and `3` to *MIST*. :::BlockQuote M55 P2 (set AUX2 out to 0 or FLOAD to 0 if the controller has 1 AUX) ::: *** ### Read outputs - M57 P Read output *x*, store the result in variable `#5399` :::BlockQuote M57 P... ::: | Output | P value | | ---------------- | -------- | | AUX1-AUX*n* | 1 to *n* | | Machine On | 51 | | Drive Enable | 52 | | Coolant1 (Flood) | 61 | | Coolant2 (Mist) | 62 | | Tool | 63 | | Tool direction | 64 | *** ## Digital inputs ### Read input - M56 P*...* | P value | Input | | -------- | --------------- | | 51 - 56 | Home Inputs X-C | | 61 | Probe Input | | 62 | Sync Input | | 63 | HWA Input | | 64 | HWB Input | | 65 | ESTOP1 | | 66 | ESTOP2 | | 67 | EXTERR | | 68 | PAUSE | The result is stored in [**System-Parameters/Variables**](docId\:oqHjs3LLCfQkSac_cemc2) `#5399` Example: erad AUX input 3: :::BlockQuote M56 P3 (Read AUX in 3) If \[#5399 == 1] Msg "AUX3=ON" Else Msg "AUX3=OFF" endif ::: Example: read home-input of X axis: :::BlockQuote M56 P51 If \[#5399 == 1] Msg "HOME X=ON" Else Msg "HOME X=OFF" endif ::: *** ### Read input + wait - M56 P* ... *L... Q... Read digital input *P* and specify wait mode, the result is stored in variable `#5399` - **P**...: the input number - **L*****0*****:** do not wait - **L*****1*****:** Wait for High - **L*****2***: Wait for Low - **Q**...: timeout (seconds) :::BlockQuote M56 P3 L2 Q30 (Read AUX in 3) If \[#5399 == -1] Errmsg "Timeout while waiting for AUX3 becoming low" Else Msg "AUX3 is off" Endif ::: Note that we use wait (L2) here, in the event of a timeout, the value of `#5399` is -1. In order to make this **code simulation and rendering proof **we need to extend it like this: :::BlockQuote If \[\[#5380 == 0] and \[#5397 == 0]] ;;Check only if running job M56 P3 L2 Q30 (Read AUX in 3) If \[#5399 == -1] Errmsg “Timeout while waiting for AUX3 becoming low” Else Msg “AUX3 is off” Endif Endif ::: *** ## Analog inputs ### Read analog input - M56 E*…* Read analog input E, result stored in `#5399` :::BlockQuote M56 E3 Msg "analog value is " #5399 ::: *** ## PWM ### Set PWM - M54 E... Q*...* Set PWM output E to permille value Q (0 \<= *y* \<= 1000) :::BlockQuote M54 E2 Q500 (Set PWM2 to 50% PWM) ::: *** ### Read PWM output - M57 E... Read PWM output, result stored in `#5399` :::BlockQuote M57 E3 If \[#5399 == 0] Msg "PWM IS OFF" Else Msg "PWM IS ON, VALUE="#5399 endif ::: *** ## Optional IOCARD If a relay board is used such as [**RLY8**](https://edingcnc.com/product/rly8-io/), the IO number *P* or *E* is specified like in the following examples: - value of `103` means card 1 port 3 - value of `208` means card 2 port 8 [title] G38.2 (Straight Probe) [path] G-code/Supported G-code/ ### The Straight Probe Command Program `G38.2 X... Y... Z... A...` to perform a straight probe operation. The rotational axis words are allowed, but it is better to omit them. If rotational axis words are used, the numbers must be the same as the current position numbers so that the rotational axes do not move. The linear axis words are optional, except that at least one of them must be used. The tool in the spindle must be a probe. It is an error if: - The current point is less than 0.254 millimeters or 0.01 inches from the pro­grammed point - G38.2 is used in inverse time feed rate mode - Any rotational axis is commanded to move - No X, Y, or Z-axis word is used In response to this command, the machine moves the controlled point (which should be at the end of the probe tip) in a straight line at the current feed rate toward the programmed point. If the probe trips, the probe is retracted slightly from the trip point at the end of the command execution. If the probe does not trip even after overshooting the programmed point slightly, an error is signaled. After successful probing, [**System-Parameters/Variables**](docId\:oqHjs3LLCfQkSac_cemc2) `#5061` to `#5066` will be set to the program coordinates of the location of the controlled point at the time the probe tripped. Variables `#5051` to `#5056` will contain the machine coordinates. Useful for measuring tools in absolute machine positions. `G53 G38.2` will move in machine coordinates. ### Using the Straight Probe Command Using the straight probe command, if the probe shank is kept nominally parallel to the Z-axis (i.e., any rotational axes are at zero) and the tool length offset for the probe is used so that the controlled point is at the end of the tip of the probe: - Without additional knowledge about the probe, the parallelism of a face of a part to the XY-plane may, for example, be found. - If the probe tip radius is known approximately, the parallelism of a face of a part to the YZ or XZ-plane may, for example, be found. - If the shank of the probe is known to be well-aligned with the Z-axis and the probe tip radius is known approximately, the center of a circular hole, may, for example, be found. - If the shank of the probe is known to be well-aligned with the Z-axis and the probe tip radius is known precisely, more uses may be made of the straight probe command, such as finding the diameter of a circular hole. If the straightness of the probe shank cannot be adjusted to high accuracy, it is desirable to know the effective radii of the probe tip in at least the +X, -X, +Y, and -Y directions. These quantities can be stored in variables either by being included in the variables file or by being set in an RS274/NGC program. Using the probe with rotational axes not set to zero is also feasible. Doing so is more complex than when rotational axes are at zero, and we do not deal with it here. ### Example Code As a usable example, the code for finding the center and diameter of a circular hole is shown below. For this code to yield accurate results, the probe shank must be well-aligned with the Z-axis, the cross-section of the probe tip at its widest point must be very circular, and the probe tip radius (i.e., the radius of the circular cross-section) must be known precisely. If the probe tip radius is known only approximately (but the other conditions hold), the location of the hole center will still be accurate, but the hole diameter will not. In the code below, an entry of the form `` is meant to be replaced by an actual number that matches the description of the number. After this section of code has been executed, the X-value of the center will be in variable `#1041`, the Y-value of the center in variable `#1022`, and the diameter in variable `#1034`. In addition, the diameter parallel to the X-axis will be in variable `#1024`, the diameter parallel to the Y-axis in variable `#1014`, and the difference (an indicator of circularity) in variable `#1035`. The probe tip will be in the hole at the XY center of the hole. The example does not include a tool change to put a probe in the spindle. Add the tool change code at the beginning, if needed. :::BlockQuote N010 (probe to find the center and diameter of circular hole) N020 (This program will not run as given here. You have to) N030 (insert numbers in place of \.) N040 (Delete lines N020, N030, and N040 when you do that.) N050 G0 Z \ F \ N060 #1001=\ N070 #1002=\ N080 #1003=\ N090 #1004=\ N100 #1005=\[\/2.0 - #1004] N110 G0 X#1001 Y#1002 (move above nominal hole center) N120 G0 Z#1003 (move into the hole - to be cautious, substitute G1 for G0 here) N130 G38.2 X\[#1001 + #1005] (probe +X side of hole) N140 #1011=#5061 (save results) N150 G0 X#1001 Y#1002 (back to the center of the hole) N160 G38.2 X\[#1001 - #1005] (probe -X side of hole) N170 #1021=\[\[#1011 + #5061] / 2.0] (find pretty good X-value of hole center) N180 G0 X#1021 Y#1002 (back to the center of the hole) N190 G38.2 Y\[#1002 + #1005] (probe +Y side of the hole) N200 #1012=#5062 (save results) N210 G0 X#1021 Y#1002 (back to center of hole) N220 G38.2 Y\[#1002 - #1005] (probe -Y side of the hole) N230 #1022=\[\[#1012 + #5062] / 2.0] (find very good Y-value of hole center) N240 #1014=\[#1012 - #5062 + \[2 \* #1004]] (find hole diameter in Y-direction) N250 G0 X#1021 Y#1022 (back to the center of the hole) N260 G38.2 X\[#1021 + #1005] (probe +X side of hole) N270 #1031=#5061 (save results) N280 G0 X#1021 Y#1022 (back to the center of the hole) N290 G38.2 X\[#1021 - #1005] (probe -X side of the hole) N300 #1041=\[\[#1031 + #5061] / 2.0] (find very good X-value of hole center) N310 #1024=\[#1031 - #5061 + \[2 \* #1004]] (find hole diameter in X-direction) N320 #1034=\[\[#1014 + #1024] / 2.0] (find average hole diameter) N330 #1035=\[#1024 - #1014] (find difference in hole diameters) N340 G0 X#1041 Y#1022 (back to the center of the hole) N350 M2 (Probing ended) ::: [title] Order of execution [path] G-code/Macro programming/ The order of execution of items on a line is critical to safe and effective machine operation. Items are executed in the order shown in the table below if they occur on the same line. 1. Comment (includes message). 2. Set feed rate mode (**G93, G94 -inverse time or per minute**). 3. Set feed rate (**F**). 4. Set spindle speed (**S**). 5. Select tool (**T**) 6. Change tool (**M6**) 7. Spindle on or off (**M3, M4, M5**) 8. Coolant on or off (**M7, M8, M9**) 9. Enable or disable overrides (**M48, M49**) 10. Dwell (**G4**) 11. Set active plane (**G17, G18, G19**) 12. Set length units (**G20, G21**) 13. Cutter radius compensation on or off (**G40, G41, G42**) 14. Cutter length compensation on or off (**G43, G49**) 15. Coordinate system selection (**G54, G55, G56, G57, G58, G59, G59.1, G59.2, G59.3**) 16. Set path control mode (**G61, G61.1, G64**) 17. Set distance mode (**G90, G91**) 18. Set retract mode (**G98, G99**) 19. Home (**G28, G30**) or change coordinate system data (**G10**) or set axis offsets (**G92, G92.1, G92.2, G94**). 20. Perform motion (**G0 to G3, G80 to G89**), as modified (possibly) by G53. 21. Stop (**M0,M1, M2,M30,M60**) [title] Software license [path] Software Manual/ # Do I need a license to start using the product? All our boards come with a software license onboard, and no further steps are necessary to start using your controller. # License upgrade Some controllers can be upgraded with extra features such as support for more axes or Ethernet support. After you have purchased an upgrade (from [**our webstore**](https://edingcnc.com/products/) or from one of [**our distributors**](https://edingcnc.com/distributors/)), we will ask you to provide us with a request code. You can obtain the code in the software: ::::::WorkflowBlock :::WorkflowBlockItem Connect the board to the PC (if you have an Ethernet board, please ensure that your [**network adapter is configured first**](https://www.youtube.com/watch?v=mT6eFq6CC9A)) ::: :::WorkflowBlockItem Start the software ::: :::::WorkflowBlockItem Navigate to license settings in the *Setup tab* ::::Tabs :::Tab{title="Version 5"} Go to the *Licenses & Support* ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/95el7qKqvFUnt9wMOsr35_image.png) ::: :::Tab{title="Version 4"} Press the *Setup Licences* button ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/9qMT8G5Q8jFgsUyZiAUxg_image.png) ::: :::: ::::: :::::WorkflowBlockItem ::::Tabs :::Tab{title="Version 5"} In the Request License section, set your name in `Name of the new license holder` field, check all the license options that apply to your newly purchased license and press `Get request code`. ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/x00cmLhKIGPBbtdos_iNo_image.png) ::: :::Tab{title="Version 4"} In the Request License section, set your name in the first text field, check all the license options that apply to your newly purchased license and press `Get Request Code` ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/G32_EnNaX3Xe_qpJyPwKE_image.png) ::: :::: ::::: :::WorkflowBlockItem [**Send us a message**](https://support.edingcnc.com/support/tickets/new) with the request code and order/payment number and we will reply to you with your new license code ::: :::WorkflowBlockItem Set the license code and press *Activate */ *Activate license* - please note that the board has to be connected for this step ::: :::::: [title] Setup tab [path] Getting started/User interface/1. Tab overview/ [title] Configuring an automatic oil pump [path] How to use/ If your machine has a device that needs to be periodically switched on during use, such as an oil pump, you can use the service feature to automate this. This feature will toggle an output as long as the CNC software is on, regardless of the machine's state. # Configuration You can configure this feature under *Pump parameters* in the *Service *tab. ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/aHEQe2Z_tQLzsfNEKTmAx_service-pump-parameters.png) The configuration items are: | Item | Description | | ------------------ | --------------------------------------------------------------------------- | | Pump interval time | Amount of time that the output is switched off (time between pump action) | | Pump pulse time | Amount of time that the output is switched on (duration of one pump action) | | Pump output | AUX output to be switched on/off by this feature | *Pump time to next* value is a status value that can be used to check how much time is left until the output is switched on i.e. time until the next pump action. It is required to press the save button to apply the configuration. # Example Let's assume that there is an oil pump device that we can power on with a relay. The relay is wired to AUX5 output on our CNC controller and we would like the pump to turn on for 3 seconds every hour. In this example, the configuration to achieve this would be: | Item | Value | | ------------------ | ----- | | Pump interval time | 3597 | | Pump pulse time | 3 | | Pump output | AUX5 | [title] Supported M-codes [path] G-code/ | M Code | Meaning | | --------------------------------------------------------------------------------------- | ---------------------------------------------------------------------------------------------------------------------------------------- | | [**M0, M1, M2, M30, M60 (Program Stopping and Ending)**](docId\:LHmMbAy23Q7kqBe9WDV0_) | Program stop | | [**M0, M1, M2, M30, M60 (Program Stopping and Ending)**](docId\:LHmMbAy23Q7kqBe9WDV0_) | Optional program stop | | [**M0, M1, M2, M30, M60 (Program Stopping and Ending)**](docId\:LHmMbAy23Q7kqBe9WDV0_) | Program end | | [**M3, M4, M5, M90 - M97 (Spindle/Tool head Control)**](docId\:LCGnVkPx_hp4rq3G5m9QV) | Turn spindle clockwise | | [**M3, M4, M5, M90 - M97 (Spindle/Tool head Control)**](docId\:LCGnVkPx_hp4rq3G5m9QV) | Turn spindle counterclockwise | | [**M3, M4, M5, M90 - M97 (Spindle/Tool head Control)**](docId\:LCGnVkPx_hp4rq3G5m9QV) | Stop spindle turning | | [**M6 (Tool Change)**](docId\:kQG7dD1dpwUw3hchbArUT) | Tool change | | [**M7, M8, M9 (Coolant Control)**](docId\:CKpEEqps6uVHTMidSiRnR) | Mist coolant on | | [**M7, M8, M9 (Coolant Control)**](docId\:CKpEEqps6uVHTMidSiRnR) | Flood coolant on | | [**M7, M8, M9 (Coolant Control)**](docId\:CKpEEqps6uVHTMidSiRnR) | Mist and flood coolant off | | M10 | Laser off (PWM off) | | M11 | Laser on with Power S | | [**M20, M21, M22 (Torch height control / Plasma THC)**](docId:4KZjVMWs8l4YNN6N5ZmcB) | Plasma Torch Height Control ON | | [**M20, M21, M22 (Torch height control / Plasma THC)**](docId:4KZjVMWs8l4YNN6N5ZmcB) | Plasma Torch Height Control OFF | | [**M20, M21, M22 (Torch height control / Plasma THC)**](docId:4KZjVMWs8l4YNN6N5ZmcB) | M23 Q… Set Plasma THC set point value | | [**M26, M27 (Rotary axis clamping)**](docId\:b-HT95-u-CRzgtMitKpI8) | Enable rotary axis clamping | | [**M26, M27 (Rotary axis clamping)**](docId\:b-HT95-u-CRzgtMitKpI8) | Disable rotary axis clamping | | [**M0, M1, M2, M30, M60 (Program Stopping and Ending)**](docId\:LHmMbAy23Q7kqBe9WDV0_) | Program end, spindle and coolants off, and rewind | | [**M48 - M53 (Feed-Speed Override Control)**](docId\:C9jbUdjZJbt5_JzMT_hWm) | Enable speed and feed overrides | | [**M48 - M53 (Feed-Speed Override Control)**](docId\:C9jbUdjZJbt5_JzMT_hWm) | Disable speed and feed overrides | | [**M48 - M53 (Feed-Speed Override Control)**](docId\:C9jbUdjZJbt5_JzMT_hWm) | Set feed override | | [**M48 - M53 (Feed-Speed Override Control)**](docId\:C9jbUdjZJbt5_JzMT_hWm) | Set speed override | | [**M48 - M53 (Feed-Speed Override Control)**](docId\:C9jbUdjZJbt5_JzMT_hWm) | Enable feed override by analog input | | [**M48 - M53 (Feed-Speed Override Control)**](docId\:C9jbUdjZJbt5_JzMT_hWm) | Enable feed hold input | | [**M54, M55, M56, M57 (General purpose IO)**](docId\:pkHadTeLJOSp0wTTu_1dJ) | Set general-purpose output | | [**M54, M55, M56, M57 (General purpose IO)**](docId\:pkHadTeLJOSp0wTTu_1dJ) | Clear general-purpose output | | [**M54, M55, M56, M57 (General purpose IO)**](docId\:pkHadTeLJOSp0wTTu_1dJ) | Read general-purpose input | | [**M54, M55, M56, M57 (General purpose IO)**](docId\:pkHadTeLJOSp0wTTu_1dJ) | Read general-purpose output | | [**M0, M1, M2, M30, M60 (Program Stopping and Ending)**](docId\:LHmMbAy23Q7kqBe9WDV0_) | Program stop, use this with nesting instead of M30 so that the spindle/coolants remain on during the transition from one to the next run | | M80 | Drive enable ON | | M81 | Drive enable OFF | | [**M3, M4, M5, M90 - M97 (Spindle/Tool head Control)**](docId\:LCGnVkPx_hp4rq3G5m9QV) | Standard Head/spindle | | [**M3, M4, M5, M90 - M97 (Spindle/Tool head Control)**](docId\:LCGnVkPx_hp4rq3G5m9QV) | Alternate Head/2nd spindle | | [**M3, M4, M5, M90 - M97 (Spindle/Tool head Control)**](docId\:LCGnVkPx_hp4rq3G5m9QV) | Alternate Head/3rd spindle | | [**M3, M4, M5, M90 - M97 (Spindle/Tool head Control)**](docId\:LCGnVkPx_hp4rq3G5m9QV) | Alternate Head/4th spindle | | [**M3, M4, M5, M90 - M97 (Spindle/Tool head Control)**](docId\:LCGnVkPx_hp4rq3G5m9QV) | Alternate Head/Probe | | [**M3, M4, M5, M90 - M97 (Spindle/Tool head Control)**](docId\:LCGnVkPx_hp4rq3G5m9QV) | Alternate Head/Camera | :::hint{type="info"} Note that a head may as well be e.g. a tangential knife configuration. ::: ## 3D printing specials | M Code | Meaning | | --------------------------------------------------------------------------------------------------------------------------- | ------------------------------------------------------------ | | [**M1, M100, M104, M106, M107, M109, M140, M143, M190; (3D printer control, discontinued)**](docId\:HHDBn9QPO179onaPOasZL) | Set extruder temperature | | [**M1, M100, M104, M106, M107, M109, M140, M143, M190; (3D printer control, discontinued)**](docId\:HHDBn9QPO179onaPOasZL) | Workpiece cooling fan on | | [**M1, M100, M104, M106, M107, M109, M140, M143, M190; (3D printer control, discontinued)**](docId\:HHDBn9QPO179onaPOasZL) | Workpiece cooling fan off | | [**M1, M100, M104, M106, M107, M109, M140, M143, M190; (3D printer control, discontinued)**](docId\:HHDBn9QPO179onaPOasZL) | M109 S... Set extruder temperature and wait until reached | | [**M1, M100, M104, M106, M107, M109, M140, M143, M190; (3D printer control, discontinued)**](docId\:HHDBn9QPO179onaPOasZL) | M140 S... Bed temperature | | [**M1, M100, M104, M106, M107, M109, M140, M143, M190; (3D printer control, discontinued)**](docId\:HHDBn9QPO179onaPOasZL) | M143 S... Maximum Hot-end temperature to prevent overheating | | [**M1, M100, M104, M106, M107, M109, M140, M143, M190; (3D printer control, discontinued)**](docId\:HHDBn9QPO179onaPOasZL) | M190 Wait for bed temperature to reach the target value | [title] M3, M4, M5, M90 - M97 (Spindle/Tool head Control) [path] G-code/Supported M-codes/ To start the spindle turning clockwise at the currently programmed speed, program `M3`. To start the spindle turning counterclockwise at the currently programmed speed, program `M4`. To stop the spindle from turning, program `M5`. `M3` or `M4` can be used if the spindle speed is set to zero. If this is done (or if the speed override switch is enabled and set to zero), the spindle will not start turning. If, later, the spindle speed is set above zero (or the override switch is turned up), the spindle will start turning. It is OK to use `M3` or `M4` when the spindle is already turning or to use `M5` when the spindle is already stopped. If there is more than one spindle in your machine, or if you have a mounted touch probe on the Z slide or a camera you can select the offset/IO you want - `M90` standard spindle - `M91` alternate 2nd spindle - `M92` alternate 3rd spindle - `M93` alternate 4th spindle - `M95` touch probe - `M97` Camera Each spindle is connected to a different set of outputs and has different parameters. Alternate spindles 1 and 2 may have defined offsets for X, Y, and Z. Because this option is rarely used by customers, it is required to perform the settings yourself by editing the cnc.ini file. There are 5 sets of parameters for each spindle configuration. For the 2nd 3rd 4th and 5th spindle configuration you can set the axis offsets with respect to the 1st spindle. Note that the 5th and 6th spindle configuration is used for a touch probe and camera. Example system: - Main Spindle, - Tangential knife - Oscillating tangential knife - Touch probe [title] How to use... [path] / [title] Getting started [path] / [title] G92, G92.1, G92.2, G92.3 (Coordinate System Offset) [path] G-code/Supported G-code/ To make the current point have the coordinates you want (without motion), program `G92 X... Y... Z... A...`, where the axis words contain the axis numbers you want. All axis words are optional, except that at least one must be used. If an axis word is not used for a given axis, the coordinate on that axis of the current point is not changed. It is an error if: - All axis words are omitted When G92 is executed, the origin of the currently active coordinate system moves. To do this, origin offsets are calculated so that the coordinates of the current point with respect to the moved origin are as specified on the line containing the G92. In addition, parameters `#5211` to `#5216` are set to the X, Y, Z, A, B, and C-axis offsets. The offset for an axis is the amount the origin must be moved so that the coordinate of the controlled point on the axis has the specified value. Here is an example. Suppose the current point is at X=4 in the currently specified coordinate system and the current X-axis offset is zero, then G92 x7 sets the X-axis offset to -3, sets parameter `#5211` to -3, and causes the X-coordinate of the current point to be 7. The axis offsets are always used when motion is specified in absolute distance mode using any of the nine coordinate systems (those designated by G54 - G59.3). Thus all nine coordinate systems are affected by G92. Being in incremental distance mode has no effect on the action of G92. Non-zero offsets may already be in effect when the G92 is called. If this is the case, the new value of each offset is A+B, where A is what the offset would be if the old offset were zero, and B is the old offset. For example, after the previous example, the X-value of the current point is 7. If G92 x9 is then programmed, the new X-axis offset is -5, which is calculated by \[\[7-9] + -3]. To reset axis offsets to zero, program **G92.1** or **G92.2**. G92.1 sets parameters `#5211` to `#5216` to zero, whereas G92.2 leaves their current values alone. To set the axis offset values to the values given in parameters `#5211` to `#5216`, program **G92.3**. You can set axis offsets in one program and use the same offsets in another program. Program G92 in the first program. This will set parameters `#5211` to `#5216`. Do not use G92.1 in the remainder of the first program. The parameter values will be saved when the first program exits and restored when the second one starts up. Use G92.3 near the beginning of the second program. That will restore the offsets saved in the first program. If other programs are to run between the program that sets the offsets and the one that restores them, make a copy of the parameter file written by the first program and use it as the parameter file for the second program. [title] Introduction [path] Software Manual/ To optimally use the software it is of course important to find all the functions of the software. In this chapter we will go the user interface and how to use it. Please note that it's possible that due to development of new features screenshot can sometime be a little different that th software that you are using. [title] How to... [path] Software Manual/ [title] Using the goto menu [path] Software Manual/How to.../ [title] Special features [path] G-code/ [title] Milling un-even surfaces / Z-heigh compensation [path] How to use/ # Milling un-even surfaces. This compensation can compensate for slight unevenness in the material surface. It is intended for relatively small compensation with a smooth, natural behavior. ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/IQ9U9EEMBPQowmXMOxVlr_image.png) ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/c8G6BQ9BnwlF9UdxPQCHK_image.png "Allowed types of compensation") The compensation is applied directly to the motion of the Z axis, therefore the acceleration profile is determined by the shape of the compensation. In cases where the compensation is not continuous, position errors may occur depending on the driver type used, the quantity of the discontinuity, and the speed of the actuators used. In open-loop systems, this may result in lost steps, and in closed-loop systems, this may result in a position following error. ## Start Measurement ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/nGIbg5xt2hK-ZsAMk32U5_z-height-comp-start-measurement.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} This button will pop up an interpreter dialog for the automatic measurement macro using a touch probe. It executes the `zhcmgrid` macro. We provide a default implementation for this in the default macro file, but this may be modified by the machine builder or user. These instructions assume the use of the unmodified macro. ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/a9Tneol3JDsKWj9TNxKzu_z-height-comp-grid-measure-dialog.png) - **nx** The number of points on the x-axis to be measured. This needs to be a whole number. - **ny** The number of points on the y-axis to be measured. This needs to be a whole number (integer). - **maxZ** The z height from where the measurements start. Ensure that this is higher than the highest point on the grid or the probe will collide with the material. - **minZ** The lowest point that the probe operation will travel to. If a point is below this number on the z-axis, this point will not be measured, this is displayed to the user during and after the measurements. - **gridSize** The distance between measurement points on each axis. - **Feed** The feed rate at which the probe operation measures the point. The lateral movements occur at G0 speeds. Pressing **Cancel** will not run the Z Height Calibration macro. Pressing **Submit** will perform the calibration. **Render** will render the movements of the macro in the job view. Executing the macro again after the render is complete will open the dialog again with the previously entered values. Adjustments can be made and the calibration can be started. After the calibration is complete, the measurements will be loaded into the software, but it is not activated yet. This is done by either checking the **Z height compensation on** checkbox or by executing the `ZHC ON` command. Additionally, the compensation is saved to the installation directory as *zHeightCompTable.txt.* ## Save Measurement ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/L-SzZzCKzeCUak0Km3ywJ_z-height-comp-save-measurement.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} This button saves the measurements to a file. A dialog opens where the location and name of the file can be selected. ## Load Measurement ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/vVLlN8UX0JItTvbW_Pgfu_z-height-comp-load-measurement.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} This button will open a file dialog where the file containing the calibrations must be selected. This loads the file, but it does not activate the Z height compensation yet. This is done by either checking the **Z height compensation on** checkbox or by executing the `ZHC ON` command. ## Check Measurement ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/8Pj5qBxPNDrwYO3oh4pQS_z-height-comp-check-measurement.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} This button checks the currently loaded compensation file for completeness. This executes the `ZHCcheck 20` command. ## Move To Start Position ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/s-fr4XMZQuZDN98Q8ZxWY_z-height-comp-move-start-position.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} This button will move the machine to the first measurement point in the Z height compensation grid. It executes the `ZHCMOVETO 0 0` command. ## Z height compensation on ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/JmIPTKhRPhKyegWyjQQrW_z-height-comp-on.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} Checking this checkbox will enable the Z height compensation, unchecking it will disable the Z height compensation. ## Show current compensation value in DRO ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/wf_gUQNvmPqIG2RXpf18s_z-height-comp-show-in-dro.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} Checking this checkbox will show the compensation values in the DRO. ::::VerticalSplit{layout="middle"} :::VerticalSplitItem ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/qzkrJgnwj8_3euZf8hLjY_z-height-comp-off-dro.png "Show current compensation on") ::: :::VerticalSplitItem ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/w6MHfYzlLIDRxllf2zLIx_z-height-comp-on-dro.png "Show current compensation off") ::: :::: **** [title] M7, M8, M9 (Coolant Control) [path] G-code/Supported M-codes/ To turn the mist coolant on, program `M7`. To turn flood coolant on, program `M8`. To turn all coolants off, program `M9`. It is always possible to use any of these commands, regardless of what coolant is on or off. [title] M1, M100, M104, M106, M107, M109, M140, M143, M190; (3D printer control, discontinued) [path] G-code/Supported M-codes/ :::hint{type="warning"} Please note that the default implementation of 3D printing-specific features is discontinued. This does **not **mean that a 3D printer cannot be made to work with our software, it simply means that 3D printer-specific M-commands should be overridden by the macro in order to manipulate the outputs and thus by proxy devices such as fans, and temperature controllers. This approach allows for greater flexibility and the ability to interface with complex machines. Please take a look at how to define custom M-functions in the section [**M-code function override and user M-code functions**](docId\:v5hvlzJR2jO4uJo6txezz) ::: `M1` All heating and Fans off `M100 P...` Change A axis resolution during execution by a factor (factor 1 is standard, 1.01 is 1% more, 0.99 is 1% less. `M104 S...` Set extruder temperature, (`M104 S50` sets the temperature to 50 degrees *Celsius*). `M106 S...` Workpiece cooling fan on optionally with S=0-100, for 0-100% *PWM* `M107` Work piece fan off `M109 S...` Set the extruder temperature and wait until it is reached. `M140 S...` Set bed temperature. `M143 S...` Set maximum hot-end temperature to prevent overheating. `M190 S...` Set the bed temperature and wait until reached. [title] Overview [path] Getting started/User interface/ When the software is started, the primary operations screen is shown. ![](https://app.archbee.com/api/optimize/wP9peVc2bAVBPOh6IboCS/YQ5nEZHhFy4OyS-l62TyT_image.png "Main application screen") The different parts are: 1. Several tabs with different functions 2. Direct I/O Control and input statuses 3. Main graphical display. 4. Homing buttons, DRO with machine and work coordinates 5. Job/macro view 6. Message screen 7. Operations buttons At the top of the window, the software version is shown. In the image below, you see that this is version V5.3. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/L-u7hLe0M3Ioc9kw0DLOO_image.png" signedSrc size="72" width="664" height="206" position="center" caption} Additionally, in this case, it indicates that it is in **simulation **mode. This means there is no connection to the controller. In simulation mode, the software can be used entirely as if it were connected to a controller. The software will still yield the same result as if a controller were connected, with respect to path control. This also offers you the opportunity to experiment with settings and observe the path that the machine would travel without actually needing to run it on a CNC machine. Also, it's an excellent way to develop your macros. However, there are two ***crucial ***differences between running in simulation or not: :::hint{type="info"} 1. It can not simulate input signals, so macros that read inputs will not work correctly in simulation mode. 2. In simulation mode, more or different I/Os can be shown that are not available at the controller that you are using. TIP: It can be helpful to automatically skip macros that will not correctly work in a simulation mode. If you would like more information, please look at the macro programming information. ::: When the software is connected to one of our controllers, it will show the name of the controller and its firmware version. To the right of the version information and controller version, the filename of the currently loaded CNC program file is loaded. # [title] MCAGuard [path] G-code/Special commands/ Switches on or off the machine area guard, no collisions will be given. This is used during the rendering process, where the job file is checked for collisions with the machine area and tool change area. :::BlockQuote MCAGuard \ ::: [title] F; (Feed rate) [path] G-code/Other input codes/ The F parameter in G-code is a versatile value that represents the feed rate, which is the rate at which the machine's tool or device moves relative to the workpiece during the machining process. This parameter can be applied to various machines and processes, such as milling, turning, laser cutting, or 3D printing, and typically determines the speed of linear and curved toolpath movements. The F parameter plays a crucial role in controlling the efficiency, accuracy, and surface finish quality of the machined part or object. To set the feed rate, program `F...`. The application of the feed rate is described in Section 2.1.2.5, unless the inverse time feed rate mode is in effect, in which case the feed rate is as described in Section 3.6.23. [title] Profiles [path] Software Manual/How to.../ :::::Tabs ::::Tab{title="Version 5"} :::hint{type="warning"} Support for profiles was added in version 5.2 of the software. Older versions require separate installations in different directories to work. ::: The default location for configurations is in the install directory in the config folder. In most cases, it is desirable to have separate instances of all settings and macro files. These can then be edited without affecting the other configuration. In this case, it is advisable to have every configuration in a different folder on the PC. To achieve this, there are two ways depending on the situation. ### Setting up a configuration from an existing configuration When the new configuration is based on an existing machine (e.g. when creating two configurations for a machine with changeable tool heads), the files present in the config folder can be copied to a new separate directory. This directory should ideally be located in the config folder with a descriptive folder name. In this example we will be setting up a lathe machine, we therefore will copy the files to a folder named "lathe" ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/GZcEkUFrf-5IjLKalWWqt_image.png" signedSrc size="50" width="268" height="270" position="flex-start" caption} Now the settings below can be followed to complete the setup. ### Setting up a new configuration from scratch When the new machine's configuration differentiates fundamentally from the original (e.g. for a totally different machine), it is recommended to set up the configuration from scratch. Create a copy of the shortcut on the desktop and rename it to be able to differentiate it from the other configuration. In this example, we will be creating a setup for a lathe machine denoted by Eding CNC Lathe. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/0Ye9Nd64MRC52KYqmsIeF_image.png" signedSrc size="50" width="189" height="121" position="flex-start" caption} Right-click on the shortcut for the new configuration and select properties. Under Target, add the location where the new configuration should be stored. In this case, we opt for a folder within the config folder named lathe. Additionally, the name of the configuration file should be specified. :::hint{type="info"} Make sure a space is present between the configuration file ::: ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/YwUzbsmc72l8lNc7qxcol_image.png" signedSrc size="70" width="363" height="543" position="flex-start" caption} Apply and close this window. Clicking this shortcut will now create a new configuration in the specified location. :::: :::Tab{title="Version 4"} If you have multiple machines controlled from the same computer, you can make a copy of the software icon on the desktop and then rename one to “CNC4.03 TURN” and the other “CNC4.03 MILL,” for example. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/ZMQ-Nkp5uDVUyMS1ryj12_image.png" signedSrc size="38" width="191" height="117" position="flex-start" caption} Now right-click the right icon ICON and select “properties”: ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/O0wh8XWmJZ-6BCRAqIT1F_image.png" signedSrc size="50" width="358" height="510" position="flex-start" caption} Add the name of the settings file behind **C:\CNC4.03\cnc.exe** to use for the software, in this case, we use **turn.ini. **The result is that with the left **CNC4.03 Mill** Icon without changes except the name, **cnc.ini** is used as the file name for all settings, and with the right **CNC4.03 Turn** Icon, **turn.ini** is used for the settings. So now you have created 2 configurations. ::: ::::: :::hint{type="info"} Running multiple instances of the Eding CNC software on the same PC is not supported. When multiple machines are supposed to run simultaneously, separate computers must be used. ::: [title] M Function override and user M-functions [path] G-code/Macro programming/ The system allows M functions in the range of M1..M999. This means there are many unused M-functions. The user can create their own M-Function by creating a subroutine for it in the macro.cnc. For example: :::hint{type="info"} sub m100 ;Do your stuff here Msg “my M100” M54 p1; switch on AUX output 1 endsub ::: # Parameters So if the G-code file performs M100, the subroutine will be called. Also, parameters in the form M100 S100 are possible. In the subroutine the parameter can be accessed using #19 (#1 .. #26 accesses parameter A..Z), S is number 19 in the alphabet. This creates further possibilities: It is possible to override existing M functions as well. Suppose you want additional function for M3 which is spindle on standard. If you spindle has an output speed-reached, you can wait for it like this: :::hint{type="info"} sub m3 msg "my customized m3" m3 s#19 ;The real m3, inside sub routine this m3 will execute the real m3 m56 P1 L2 Q60 ; Wait max. 1 minute for input 1 to become low endsub ::: When you are inside your m3 subroutine and perform an m3, then the subroutine is not called, but the default m3 is called instead. There are some limitations on using the M Function override: • There must be nothing else on the G-code line as the M-Function, e.g. :::hint{type="info"} N2000 M3 S1000 is OK. N2000 M3 M8 G1X100 is NOT OK! ::: • The user parameters 1-26 will be used as parameter and will be overwritten when M-Function subroutines are used. Take this into account and do not use #1..#26 in your program if you use this functionality. Variable 1-26 match with the letter of the alphabet, #1 will get the value of parameter A, #26 will get the value of parameter Z. [title] G33, G33.1 (Spindle-Synchronized Motion) [path] G-code/Supported G-code/ For spindle-synchronized motion in one direction, program `G33 X... Y... Z... K...` where K gives the distance moved in XYZ for each revolution of the spindle. For G33 the software performs this: 1. Start a synchronized move with the spindle with K feed per revolution. Assumed is that the spindle already runs ([**M3, M4, M5, M90 - M97 (Spindle/Tool head Control)**](docId\:LCGnVkPx_hp4rq3G5m9QV)) 2. Done For G33.1 the software performs: 1. Start a synchronized move with the spindle with K feed per revolution. Assumed is that the spindle is running (M3) 2. Wait until this motion is done 3. Reverse spindle direction 4. Move back to the original position where we were before the G33.1 5. Done All the axis words are optional, except that at least one must be used. It is an error if: - All axis words are omitted - The spindle is not turning when this command is executed - The requested linear motion exceeds machine velocity limits due to the spindle speed [title] Coordinates [path] Getting started/User interface/1. Tab overview/ ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/diMcV52EO-ozLwfBhI5Rh_coordinates.png) The coordinates tab allows the operator to calibrate and switch between the coordinate systems. Furthermore, Z height compensation and optionally A Cylinder kinematics can be set up here. # Calibrate ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/25yHmSLd38se7rFJlPKRO_coordinates-calibrate.png) Pressing one of the buttons in the calibrate section sets the current position as the origin for that coordinate system. The button performs `G10 L20 P... X... Y... Z...` Where `P...` is the number of the coordinate system and the coordinates are the current position of the machine. For more information on this action see [**G10 (Set Coordinate System Data)**](docId\:b9LKOzR8VYIIM7e85U0X3). The offsets associated with a coordinate system can be seen on the [**Variables tab**](docId\:GXw9wEBk8aZ35cyV-ELYH) tab, where these values can be edited as well. # Activate ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/QknayZpUuqX3M-sa2ZpmB_coordinates-activate.png) Pressing one of the buttons in the activate section activates that coordinate system. This means that the offsets of that coordinate system are applied to the machine's position. The button performs `G54` to `G59.3` depending on the button. For more information on this action see [**G54 - G59.3 (Select Coordinate System)**](docId\:baX8uyfAimzYLPAp9bPJ3). The currently active coordinate system is shown by the accented color of one of the coordinates. Additionally, it can be seen in the list of currently active G-codes. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/QNipqKGLvc_bhXQWHY4kk_image.png" signedSrc size="26" width="178" height="97" position="flex-start" caption="G54 is currently active, G55 is not." alt} ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/9_9UcJomty-U23qWbzrBI_image.png" signedSrc size="72" width="357" height="66" position="flex-start" caption="G54 is currently active." alt} # # Milling un-even surfaces. This compensation can compensate for slight unevenness in the material surface. It is intended for relatively small compensation with a smooth, natural behavior. ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/IQ9U9EEMBPQowmXMOxVlr_image.png) ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/c8G6BQ9BnwlF9UdxPQCHK_image.png "Allowed types of compensation") The compensation is applied directly to the motion of the Z axis, therefore the acceleration profile is determined by the shape of the compensation. In cases where the compensation is not continuous, position errors may occur depending on the driver type used, the quantity of the discontinuity, and the speed of the actuators used. In open-loop systems, this may result in lost steps, and in closed-loop systems, this may result in a position following error. ## Start Measurement ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/nGIbg5xt2hK-ZsAMk32U5_z-height-comp-start-measurement.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} This button will pop up an interpreter dialog for the automatic measurement macro using a touch probe. It executes the `zhcmgrid` macro. We provide a default implementation for this in the default macro file, but this may be modified by the machine builder or user. These instructions assume the use of the unmodified macro. ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/a9Tneol3JDsKWj9TNxKzu_z-height-comp-grid-measure-dialog.png) - **nx** The number of points on the x-axis to be measured. This needs to be a whole number. - **ny** The number of points on the y-axis to be measured. This needs to be a whole number (integer). - **maxZ** The z height from where the measurements start. Ensure that this is higher than the highest point on the grid or the probe will collide with the material. - **minZ** The lowest point that the probe operation will travel to. If a point is below this number on the z-axis, this point will not be measured, this is displayed to the user during and after the measurements. - **gridSize** The distance between measurement points on each axis. - **Feed** The feed rate at which the probe operation measures the point. The lateral movements occur at G0 speeds. Pressing **Cancel** will not run the Z Height Calibration macro. Pressing **Submit** will perform the calibration. **Render** will render the movements of the macro in the job view. Executing the macro again after the render is complete will open the dialog again with the previously entered values. Adjustments can be made and the calibration can be started. After the calibration is complete, the measurements will be loaded into the software, but it is not activated yet. This is done by either checking the **Z height compensation on** checkbox or by executing the `ZHC ON` command. Additionally, the compensation is saved to the installation directory as *zHeightCompTable.txt.* ## Save Measurement ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/L-SzZzCKzeCUak0Km3ywJ_z-height-comp-save-measurement.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} This button saves the measurements to a file. A dialog opens where the location and name of the file can be selected. ## Load Measurement ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/vVLlN8UX0JItTvbW_Pgfu_z-height-comp-load-measurement.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} This button will open a file dialog where the file containing the calibrations must be selected. This loads the file, but it does not activate the Z height compensation yet. This is done by either checking the **Z height compensation on** checkbox or by executing the `ZHC ON` command. ## Check Measurement ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/8Pj5qBxPNDrwYO3oh4pQS_z-height-comp-check-measurement.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} This button checks the currently loaded compensation file for completeness. This executes the `ZHCcheck 20` command. ## Move To Start Position ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/s-fr4XMZQuZDN98Q8ZxWY_z-height-comp-move-start-position.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} This button will move the machine to the first measurement point in the Z height compensation grid. It executes the `ZHCMOVETO 0 0` command. ## Z height compensation on ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/JmIPTKhRPhKyegWyjQQrW_z-height-comp-on.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} Checking this checkbox will enable the Z height compensation, unchecking it will disable the Z height compensation. ## Show current compensation value in DRO ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/wf_gUQNvmPqIG2RXpf18s_z-height-comp-show-in-dro.png" signedSrc size="50" width="361" height="438" position="flex-start" caption} Checking this checkbox will show the compensation values in the DRO. ::::VerticalSplit{layout="middle"} :::VerticalSplitItem ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/qzkrJgnwj8_3euZf8hLjY_z-height-comp-off-dro.png "Show current compensation on") ::: :::VerticalSplitItem ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/w6MHfYzlLIDRxllf2zLIx_z-height-comp-on-dro.png "Show current compensation off") ::: :::: ** # A Cylinder ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/aoAlc8ZXSiqOp0IiYio-f_a-cylinder.png) This feature is useful when milling on the outside of a cylinder using a rotary axis on the A-axis. When enabling this feature, a flat job file can be projected on the cylinder where the movements on the Y-axis are mapped to the A-axis, taking into account the radius of the cylinder. :::hint{type="info"} Note that this configuration is only visible when the A-axis is set to *4th milling axis* and Kinematics DLL is set to *acilinderkins.dll.* ::: This feature requires some configuration to correctly map the Y-axis to the A-axis. It requires both the rotation point and the radius of the cylindrical workpiece. ## Setting Rotation Point ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/n9JY4gRnGt2BWjfGzyb5K_a-cylinder-rotation-point.png" signedSrc size="70" width="458" height="185" position="flex-start" caption} The rotation point can either be set by entering the position and pressing (1) Set position, or by moving to the rotation point and pressing (1) Set to current position. ### (1) Set position ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/iLabS8-WNDjgTzt08Bwhp_a-cylinder-set-position.png" signedSrc size="70" width="458" height="185" position="flex-start" caption} When the exact location of the rotation point is known beforehand, these coordinates (Y- and Z-axis) can be set directly in the respective input boxes. The (1) Set position needs to be pressed to apply and confirm this position. ### (1) Set to current position ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/8QKL616Tm9aQ59B-uEAlF_a-cylinder-set-to-current-position.png" signedSrc size="70" width="458" height="185" position="flex-start" caption} When the exact position is not known beforehand, usually because the A-axis is removable and cannot be repositioned exactly, the position can be calibrated manually. To calibrate the position, move the machine to the rotation point on the Y- and Z-axis, and press (1) Set to current position. ## Setting Cylinder Radius ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/drcRxZHSGilMsLHxpV0fw_a-cylinder-radius.png" signedSrc size="70" width="458" height="185" position="flex-start" caption} The cylinder radius can be set either by entering the radius in the input box labeled R and pressing (2) Set radius, or by moving to the machine so the tool touches the top of the material and pressing (2) Calibrate radius. ### (2) Set radius ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/l9g-F70ZIqcS5U5t1qgoh_a-cylinder-set-radius.png" signedSrc size="70" width="458" height="185" position="flex-start" caption} When the exact radius of the material is known beforehand, the value can be entered in the input box labeled R. To confirm this position, the (2) Set radius button needs to be pressed. ### (2) Calibrate radius ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/kjdZ1vJ-JoPAsPK4pY7sw_a-cylinder-calibrate-radius.png" signedSrc size="70" width="458" height="185" position="flex-start" caption} When the radius of the cylinder is not known beforehand, the radius can be determined by moving the tooltip on top of the material and pressing (2) Calibrate radius. This calculates the radius from the current position of the machine and the previously set rotation point. ## Reset calibration ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Gsz-nyIpV7ojcisIGI-A5_a-cylinder-reset-calibration.png" signedSrc size="70" width="458" height="185" position="flex-start" caption} Pressing the Reset calibration button will reset the rotation point and radius settings, in case Map Y -> A was turned on, it will be turned off after. ## Save calibration ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Ireztnl4PU82RUpZ9Alz1_a-cylinder-save-calibration.png" signedSrc size="70" width="458" height="185" position="flex-start" caption} Pressing the Save calibration button will save the rotation point and radius to the configuration file, so these values will automatically reload when restarting the software. Do note that Map Y -> A is not turned on automatically every time the software starts. This needs to be done either by moving the Y-axis to the rotation point and checking the checkbox or by executing the `KIN ON` command. ## Move to Y rotation point ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/bPgLklV9fkpoDPLK222yj_a-cylinder-move-to-y-rotation-point.png" signedSrc size="70" width="458" height="185" position="flex-start" caption} Pressing the Move to Y rotation point button will move the machine to the Y coordinate of the rotation point. :::hint{type="info"} Note that the machine will move to the Y coordinate of the rotation point at the current X and Z coordinate. It is therefore important to ensure that the Z axis is at an appropriate height and there are no obstructions in the path. ::: ## Map Y -> A ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/r6W9YcxGiDObbQJpbu7UK_a-cylinder-map-y-to-a.png" signedSrc size="70" width="458" height="185" position="flex-start" caption} Checking the Map Y -> A checkbox will turn the A Cylinder options on if all conditions are met. Ensure that: - The rotation point is set - The radius is set - The Y-axis is at the rotation point In case these conditions are not met, the option will not turn on and an error message will be visible in the message window. [title] WaitForRLYUpdate [path] G-code/Special commands/ This command will hold execution of further commands until the next relay board value update. The relay board values are updated automatically at an interval, so while usage of this command is not necessary for most applications, if it is expected that the input state changed less than 100 ms before a value read, using this command right before the reading command will ensure that the read value is current. [title] LogMsg [path] G-code/Special commands/ Logs message to a text file. The file has to be specified prior by the [**LogFile**](docId\:O8uMNjPOxJ29-g_tKKAsN) command. :::BlockQuote LogMsg "\" ::: ### Parameters - message text parameter specifies the message to be displayed - if [**Variables**](docId\:oqHjs3LLCfQkSac_cemc2) numbers are included outside of quotation marks, this results in the value of that variable being appended to the message e.g. `Msg "value of variable 4000 is " #4000` - if `%t...` is included outside of quotation marks, this results in the tool description of the tool number being appended to the message e.g. `Msg "T1 is " %t1` or `msg "Current tool: " %t#5011` - if `%d` is included outside of quotation marks, this results in the current date and time being appended to the message e.g. `Msg "Time: "%d` will output *Time: 2022-10-28 13:35:52* ### Example :::BlockQuote LogFile "text.txt" 1 LogMsg "Current position of X is "#5001 ::: Now check the contents of file text.txt will now contain Msg, LogMsg, WarnMsg, ErrMsg can now use %txx (xx = 0-99) and this will show the tool description text. Example: msg %t#5011 " is changed to "Tool number 5" this is text from the tool table. [title] MistOff [path] G-code/Special commands/ Turns off the mist output on the controller. :::hint{type="warning"} If a custom override for M9 exists, this subroutine is not executed by the MistOff command. Refrain from using MistOff in this case. ::: [title] G10 (Set Coordinate System Data) [path] G-code/Supported G-code/ To set the coordinate values for the origin of a coordinate system, program `G10 L2 P X... Y... Z... A...`, where the P number must evaluate to an integer in the range 1 to 9 (corresponding to [**G54 - G59.3 (Select Coordinate System)**](docId\:baX8uyfAimzYLPAp9bPJ3)), and all axis words are optional. The coordinates of the origin of the coordinate system specified by the P number are reset to the coordinate values given (in terms of the absolute coordinate system). Only those coordinates for which an axis word is included on the line will be reset. It is an error if: - the P number does not evaluate as an integer in the range 1 to 9. If origin offsets (made by [**G92, G92.1, G92.2, G92.3 (Coordinate System Offset)**](docId:-_dARrxY7XSFSM2Qp6jJL)) were in effect before G10 is used, they will continue to be in effect afterward. The coordinate system whose origin is set by a G10 command may be active or inactive at the time the G10 is executed. Example: `G10 L2 P1 x 3.5 y 17.2` sets the origin of the first coordinate system (the one selected by G54) to a point where X is 3.5 and Y is 17.2 (in absolute coordinates). The Z coordinate of the origin (and the coordinates for any rotational axes) are whatever those coordinates of the origin were before the line was executed. `G10 L20 P... X... Y... Z... A...` Set coordinate system given by P number relative to actual machine position. Working is similar to G92. Jog to any position, then apply e.g. `G10 L20 P1 X0 Y0` to set G54 coordinate system zero point at the current machine position. [title] Run behavior during loading of job file and simulation [path] G-code/Macro programming/ Simulation refers to the software mode that is used when no hardware is connected. During the loading of a G-Code file, the interpreter runs the file while generating output for the graphic. During this no actions to the machine are applied, no motion and no I/O, only checks if the g-code is valid and stays within the machine limits. If there is advanced macro programming, e.g. because the machine has automatic tool change, it is important to take into account that in simulation and render mode no machine actions take place. ## Check example that should be always executed Suppose we have a machine with a 6-tool automatic tool changer. A check is programmed that generates an error if a g-code file is loaded that tries to change the tool to a number that the machine does not have: :::BlockQuote if \[#5011 > 6] ErrMsg “Please select a tool in the range of 1 to 6” Else ; Code to perform the tool change Endif ::: It stands to reason that we want this “ErrMsg …” line to be executed always, when running but also in simulation mode and when loading the file. Check example that should be only executed during the job --------------------------------------------------------------- :::BlockQuote sub check\_airpresure m56 p5 if \[#5399 == 0] errmsg "Error, No Air pressure" else msg "Air Pressure OK" endif endsub ::: This check on air pressure will not work correctly while loading a g-code file or while the system is in simulation mode, because no actual inputs are read. :::BlockQuote sub check\_airpresure ; Check only if not rendering and not during simulation if \[\[#5380 == 0] and \[#5397 == 0]] m56 p5 if \[#5399 == 0] errmsg "Error, No Air pressure" else msg "Air Pressure OK" endif endif endsub ::: Here we see the modification to make the on the air pressure sensor input 5 simulation and render proof, the check is only performed when we are not in render or simulation mode, only an extra if statement that checks variable `#5380` (contains the value of 1 when simulation mode) and `#5397` (contains the value of 1 when rendering) is added. [title] DlgMsg [path] G-code/Special commands/ :::hint{type="warning"} Please note that mentioned commands may fail during loading and/or simulation. To make your macro code avoid these errors please take a look at the manual section [**Run behavior during loading of job file and simulation**](docId\:p2Jh9fFRvp0WCb5jCD9px) ::: Opens a dialog window that the operator can interact with. The dialog can be used to input up to 12 [**Variables**](docId\:oqHjs3LLCfQkSac_cemc2) values. The dialog will show the current values of the specified variables. The specified variable values are changed according to the users' input once the dialog is submitted. :::BlockQuote DlgMsg \ \ \ ... \ \ ::: The dialog has an OK and a Cancel button. When the user selects OK, variable `#5398` is set to 1. When the user selects CANCEL, variable `#5398` is set to -1. During the job loading process, the dialog display is skipped and `#5398` is automatically set to the value of 1. The macro can give the queried variables a value before the `DlgMsg` command takes place which will serve as a default value. The macro file can then query check these variables and proceed accordingly. If \.png file exists in the *dialogPictures* directory located inside the installation directory then it will be displayed in the dialog. ### Example `DlgMsg "Please input job parameters" width 100 height 101` :::BlockQuote Sub user\_3 ;Example of dlgmsg \#1 = 0 \#2 = 0 \#3 = 0 \#4 = 0 \#5 = 0 \#6 = 0 \#7 = 0 \#8 = 0 \#9 = 0 \#10 = 0 \#11 = 0 \#12 = 0 ;dlgmsg will show a dialog with picture edingcnc.png from the installation directory\dialogPictures dlgmsg "edingcnc" "A" 1 "B" 2 "C" 3 "D" 4 "E" 5 "F" 6 "G" 7 "H" 8 "I" 9 "J" 10 "K" 11 "L" 12 if \[#5398 == 1] msg "OK #1="#1 "#2="#2 "#3="#3 "#4="#4 "#5="#5 "#6="#6 "#7="#7 "#8="#8 "#9="#9 "#10="#10 "#11="#11 "#12="#12 else msg "CANCEL #1="#1 "#2="#2 "#3="#3 "#4="#4 "#5="#5 "#6="#6 "#7="#7 "#8="#8 "#9="#9 "#10="#10 "#11="#11 "#12="#12 endif Endsub ::: ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Mnsi8OwGFvy9ptgjyLBTB_image.png) [title] 1. Tab overview [path] Getting started/User interface/ At the top, several tabs are displayed. Based on your configuration, some might have been hidden. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/H5hRLGrsCCJO5nyymcshs_image.png" signedSrc size="64" width="966" height="187" position="center" caption="Tabs in the main window" alt} Each tab has a separate function: | **Tab name** | **Function** | | ------------ | -------------------------------------------------------------------------- | | Operate | The main operations screen | | Coordinates | Setting up different coordinate systems, surface compensatio, and 4th axis | | Program | An interface to external CAM software | | Tools | An overview of available tools | | Variables | Information about internal variables, also for debugging purpose | | IO | Information about inputs, and controlling manually outputs | | Service | Service-related information | | Setup | The Setup screen for configuring hard and software | | Help | Information about software, support and more. | It's also possible to navigate the tabs through the keyboard shortcuts. **Tab navigation** It's possible to navigate the tabs by using keyboard shortcuts: | Keyboard keys | Function | | ------------------------ | ----------------------- | | `CTRL `+ `TAB` | Select tab to the left | | `CTRL `+ `SHIFT `+ `TAB` | Select tab to the right | | `ALT `+ `O` | Jump to operate tab | In the next pages we're [title] Software installation [path] Getting started/ ## Installation of the Eding CNC software To find the latest version of the software alongside the release notes, visit the [**download page**](https://edingcnc.com/download-software/) on the website. ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/8NGsWbM68owz5ir383SAH_image.png) Download the executable for the software version you wish to install, and start the installer. :::hint{type="info"} Windows might not recognize the installer and flag it as unsafe, in this case, a pop-up will show. If the installer was downloaded from our website it is safe to install. Click ***More info*** to continue with the installation process. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/gdhwIPMtazlS9e9h0PHIn_image.png" size="50" width="665" height="624" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/gdhwIPMtazlS9e9h0PHIn_image.png"} Click ***Run anyway*** ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/6eY6gkajBKS-nZ-qEiQXi_image.png" size="50" width="663" height="622" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/6eY6gkajBKS-nZ-qEiQXi_image.png"} The installation of the software will continue ::: When the installation starts, a window will be presented. Click ***Yes ***to start the installation. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Js0dREjZwkbP6WN6NFHke_image.png" size="50" width="541" height="259" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Js0dREjZwkbP6WN6NFHke_image.png"} The installer will start by asking the language for the installation. Select the appropriate language and press ***OK*** to continue. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/LkWmpATKKNFKiAtScdqau_image.png" size="40" width="345" height="208" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/LkWmpATKKNFKiAtScdqau_image.png"} A window with the License Agreement will show. If you agree, select ***I accept the agreement*** and press ***Next*** ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Lpgkw2RoBNX4sQkV0OMa0_image.png" size="70" width="579" height="479" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Lpgkw2RoBNX4sQkV0OMa0_image.png"} The installation location is shown. In this case, the software will be installed in folder ***C:\EdingCNC5.00***. To change the install directory, click on ***Browse…*** and select a different folder. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/VAKGW9b0DtCT1eOPA5UBF_image.png" size="70" width="578" height="478" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/VAKGW9b0DtCT1eOPA5UBF_image.png"} The next screen will ask whether to create a desktop shortcut and/or Quick Launch shortcut. Make the selection and press ***Next*** ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/gvTaoYShtsA_ykX5RXIxL_image.png" size="70" width="579" height="478" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/gvTaoYShtsA_ykX5RXIxL_image.png"} On the last screen of the installation, an overview is shown of the selected settings for installation. Click ***Install*** to start the installation. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Q64h7wmRwYRkvPwPEaBVm_image.png" size="70" width="578" height="479" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Q64h7wmRwYRkvPwPEaBVm_image.png"} The progress of the installation can be monitored. It can be stopped by clicking on ***Cancel***. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/n1jlr95bjs02gmmBnku8f_image.png" size="70" width="579" height="479" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/n1jlr95bjs02gmmBnku8f_image.png"} When the installation has finished, a new window appears in which several options can be selected. These settings will help in using the software, some are mandatory others are optional but recommended. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/YNNHVf41uakPc1EsWUjYE_image.png" size="70" width="578" height="479" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/YNNHVf41uakPc1EsWUjYE_image.png"} The options that are greyed out are mandatory. The settings are: - **Start EdingCNC.exe as administrator.** This setting is recommended because starting the software as an administrator ensures it will utilize the maximum system performance. Without it, the software might experience dropouts. - **Virtual keyboard (osk) compatibility mode.** This option makes sure that the virtual keyboard can be used in the software. - **Disable User Account Control prompt.** This will stops Windows from interfering with the installed application; you can deselect the option. However, the OS can ask you whether you are sure you want to start the software, which can be very annoying. - **Network drives visible for cnc.exe.** By default, applications running in administrator mode cannot see the network drives from the logged-in user. - **Disable Windows Update.** Disabling Windows Update is highly recommended, because you do not want Windows to update and interrupt a 200-hour CNC job. Better update Windows manually when you want to. - **Show known Windows file extensions.** This will help in recognizing files and selecting the correct ones by displaying the file extensions. For example, ‘mickey.cnc’ or ‘cnc.ini’. Although not vital, it is strongly advised to enable it to help you operate the software. By clicking on ‘**Next**’, these settings will be set. The next screen shows options to install additional third-party software that can be used in combination with the Eding CNC software. Select what software to install and press ***Next***. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Rcf-Q5fhLHrEKUg6meqqD_image.png" size="70" width="578" height="479" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Rcf-Q5fhLHrEKUg6meqqD_image.png"} The final step of the installation is installing the USB drivers. This is also done through a simple installer. Click the checkboxes to install the USB drivers or/and view the release note for the software if desired. When this is the first time installing the software, make sure to also install the USB drivers. Click on ***Finish*** to finalize the installation. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/_VfX5oEaz6-q9GZzNgbZv_image.png" size="70" width="577" height="479" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/_VfX5oEaz6-q9GZzNgbZv_image.png"} If ‘View the ReleaseNotes.txt’ is selected, immediately after pressing ‘Finish’ the release note will be shown. The release notes sum up what has changed or is new for this release of the software. Shown below is part of a release note. ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/cb6da0FOOciHK4vwbii7K_image.png) If the ***Install USB drivers*** option was selected, a window will appear to install these. Click ***Next*** to start installing the drivers. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/CcLV_a2s44be1C4ykziRF_image.png" size="70" width="619" height="481" caption position="flex-start" signedSrc} Upon completion, click ***Finish*** to close the wizard. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/1WCEG-lRFS7gvZ8aixFKN_image.png" size="70" width="619" height="480" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/1WCEG-lRFS7gvZ8aixFKN_image.png"} :::hint{type="info"} Please note, the driver will contain the name USBCNC, this is Eding CNCs previous name. ::: After the installation, please reboot the PC. After rebooting, connect the machine. The machine is now found by Windows if the machine is connected using USB. To check that the USB driver was installed correctly, open Device Manager in Windows by pressing the ***Win key + X***, then choose Device Manager. This will show the device manager. If a USB-based controller is connected it will show under ***Ports*** as ***USBCNC COM Port***. The port that is indicated, which is COM17 in this case, may vary per configuration. ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/LYjQKgOgX5Hz1lNZElSIy_image.png) :::hint{type="info"} If your machine is connected to the PC using Ethernet, follow the [**Network setup**](docId:1TgQjqVfRjXCVg0VjcGw1) to ensure a connection to the machine can be established. When using a USB controller this step can be skipped. ::: [title] Software Manual [path] / This software manual describes how to use the software, and it's intended audiences are end-user how operate a machine. [title] Macro programming [path] G-code/ The macro file provides a place to add functionality or override existing behavior specific to the machine. The contents of this file are treated the same way as a job and accept the same commands. [title] GetHeightControlVact [path] G-code/Special commands/ :::hint{type="info"} This command will only be executed when the machine type is set to **plasma **or **laser**. ::: Retrieves the current value of the Vact of the height control. :::BlockQuote GetHeightControlVact \ ::: The resulting value is stored in the specified variable. ### Example :::BlockQuote GetHeighControlVact 5399 ::: [title] Supported G-code [path] G-code/ G codes of the RS274/NGC language are shown on a specific page each. The descriptions contain command prototypes, formatted as `a code block`. In the command prototypes, three dots `…` substitute a real value. As described earlier, a real value may be (1) an explicit number, 4, for example, (2) an expression like `[2+2]`, (3) a parameter value, `#86`, for example, or (4) a unary function value like `acos[0]`. In most cases, if axis words (any or all of `X…`, `Y…`, `Z…`, `A…`, `B…`, `C…`) are given, they specify a destination point. Axis numbers are in the currently active coordinate system unless explicitly described as being in the absolute coordinate system. Where axis words are optional, any omitted axes will have their current value. Any items in the command prototypes not explicitly described as optional are required. It is an error if a required item is omitted. In the prototypes, the values following letters are often given as explicit numbers. Unless stated otherwise, the explicit numbers can be real values. For example, `G10 L2` could equally well be written `G[2*5] L[1+1]`. If the value of parameter 100 were 2, `G10 L#100` would also mean the same. Using real values that are not explicit numbers, as just shown in the examples, is rarely useful. If `L…` is written in a prototype, the `…` will often be referred to as the "L number". Similarly, the `…` in `H…` may be called the "H number", and so on for any other letter. | G Code | Meaning | | --------------------------------------------------------------------------------------------- | ------------------------------------------------------------- | | [**G0 (Rapid Linear Motion)**](docId\:sMEIPmfNLzqwnk8pfSSZC) | Rapid positioning | | [**G1 (Linear Motion Feed at Feed Rate)**](docId\:rIq0kXPLy7LFjPIEIK24B) | Linear interpolation | | [**G2, G3 (Arc at Linear Feed)**](docId\:DpEeyJKCmM8gHOFGpx91b) | Circular/helical interpolation (clockwise) | | [**G2, G3 (Arc at Linear Feed)**](docId\:DpEeyJKCmM8gHOFGpx91b) | Circular/helical interpolation (counterclockwise) | | [**G4 (Dwell)**](docId\:G-JGI-faoUvo1TqR5NO78) | Dwell | | [**G10 (Set Coordinate System Data)**](docId\:b9LKOzR8VYIIM7e85U0X3) | Coordinate system origin setting | | [**G17, G18, G19 (Plane Selection)**](docId\:Uo-PghD6GWTJ4p9XJ2NzP) | XY-plane selection | | [**G17, G18, G19 (Plane Selection)**](docId\:Uo-PghD6GWTJ4p9XJ2NzP) | XZ-plane selection | | [**G17, G18, G19 (Plane Selection)**](docId\:Uo-PghD6GWTJ4p9XJ2NzP) | YZ-plane selection | | [**G20, G21, G70, G71 (Length Units)**](docId\:tMFh7VgzKxLCgKy5DalRG) | Imperial system selection | | [**G20, G21, G70, G71 (Length Units)**](docId\:tMFh7VgzKxLCgKy5DalRG) | Millimeter system selection | | [**G28, G30 (Return to Home)**](docId\:hiQpVG7ODggc7wQsV-aNk) | Move to park position 1, setup on the variable page | | [**G28, G30 (Return to Home)**](docId\:hiQpVG7ODggc7wQsV-aNk) | Move to park position 2, setup on the variable page | | [**G33, G33.1 (Spindle-Synchronized Motion)**](docId\:fWBx0fGEp7FiOiEzUhpa5) | Lathe, motion synchronized to the spindle | | [**G38.2 (Straight Probe)**](docId\:F-KbF-l0L8hsYegslP9Xs) | Straight probe | | [**G40, G41, G41.1, G42, G42.1 (Cutter Radius Compensation)**](docId\:fyQHuNSflfSdBpEnqYkQJ) | Cancel cutter radius compensation | | [**G40, G41, G41.1, G42, G42.1 (Cutter Radius Compensation)**](docId\:fyQHuNSflfSdBpEnqYkQJ) | Start cutter radius compensation left | | [**G40, G41, G41.1, G42, G42.1 (Cutter Radius Compensation)**](docId\:fyQHuNSflfSdBpEnqYkQJ) | Start cutter radius compensation right | | [**G43, G43.1, G49 (Tool Length Offset)**](docId\:DcUuepSG6YTe-sD5BBvdh) | Tool length offset (plus), tool X offset for lathe | | [**G43, G43.1, G49 (Tool Length Offset)**](docId\:DcUuepSG6YTe-sD5BBvdh) | Cancel tool length offset | | [**G53 (Move in Absolute Coordinates)**](docId\:LcnWMZ2I2Ii08f90oBaL-) | Motion in machine coordinate system | | [**G54 - G59.3 (Select Coordinate System)**](docId\:baX8uyfAimzYLPAp9bPJ3) | Use preset work coordinate system 1 | | [**G54 - G59.3 (Select Coordinate System)**](docId\:baX8uyfAimzYLPAp9bPJ3) | Use preset work coordinate system 2 | | [**G54 - G59.3 (Select Coordinate System)**](docId\:baX8uyfAimzYLPAp9bPJ3) | Use preset work coordinate system 3 | | [**G54 - G59.3 (Select Coordinate System)**](docId\:baX8uyfAimzYLPAp9bPJ3) | Use preset work coordinate system 4 | | [**G54 - G59.3 (Select Coordinate System)**](docId\:baX8uyfAimzYLPAp9bPJ3) | Use preset work coordinate system 5 | | [**G54 - G59.3 (Select Coordinate System)**](docId\:baX8uyfAimzYLPAp9bPJ3) | Use preset work coordinate system 6 | | [**G54 - G59.3 (Select Coordinate System)**](docId\:baX8uyfAimzYLPAp9bPJ3) | Use preset work coordinate system 7 | | [**G54 - G59.3 (Select Coordinate System)**](docId\:baX8uyfAimzYLPAp9bPJ3) | Use preset work coordinate system 8 | | [**G54 - G59.3 (Select Coordinate System)**](docId\:baX8uyfAimzYLPAp9bPJ3) | Use preset work coordinate system 9 | | [**G61, G64 (Path Control Mode and Look Ahead Feed)**](docId:2bjZDN24vLTY2JWZO_Txw) | Set path control mode: exact path | | [**G61, G64 (Path Control Mode and Look Ahead Feed)**](docId:2bjZDN24vLTY2JWZO_Txw) | Set path control mode: exact stop | | [**G61, G64 (Path Control Mode and Look Ahead Feed)**](docId:2bjZDN24vLTY2JWZO_Txw) | Set path control mode: continuous | | [**G68 (Coordinate System Rotation)**](docId\:VpyIB1fwdN7BZilxiuRb6) | XY rotation | | [**G76 (Threading lathe)**](docId\:D1pnA2zyfWITU3ZQNDH54) | Lathe, threading | | [**G80 (Cancel Modal Motion)**](docId:_FSUESGLv1pm3hKfV84FL) | Cancel motion mode (including any canned cycle) | | [**G81 - G89 (Canned Cycles)**](docId\:bMnlFQH73fIoeAmGBFFvk) | Canned cycle: drilling | | [**G81 - G89 (Canned Cycles)**](docId\:bMnlFQH73fIoeAmGBFFvk) | Canned cycle: drilling with dwell | | [**G81 - G89 (Canned Cycles)**](docId\:bMnlFQH73fIoeAmGBFFvk) | Canned cycle: peck drilling | | [**G81 - G89 (Canned Cycles)**](docId\:bMnlFQH73fIoeAmGBFFvk) | Canned cycle: right-hand tapping | | [**G81 - G89 (Canned Cycles)**](docId\:bMnlFQH73fIoeAmGBFFvk) | Canned cycle: boring, no dwell, feed out | | [**G81 - G89 (Canned Cycles)**](docId\:bMnlFQH73fIoeAmGBFFvk) | Canned cycle: boring, spindle stop, rapid out | | [**G81 - G89 (Canned Cycles)**](docId\:bMnlFQH73fIoeAmGBFFvk) | Canned cycle: back boring | | [**G81 - G89 (Canned Cycles)**](docId\:bMnlFQH73fIoeAmGBFFvk) | Canned cycle: boring, spindle stop, manual out | | [**G81 - G89 (Canned Cycles)**](docId\:bMnlFQH73fIoeAmGBFFvk) | Canned cycle: boring, dwell, feed out | | [**G90, G91 (Set Distance Mode)**](docId\:nwnlRN2wTcaF7W5zIc62j) | Absolute distance mode | | [**G90, G91 (Set Distance Mode)**](docId\:nwnlRN2wTcaF7W5zIc62j) | Incremental distance mode | | [**G92, G92.1, G92.2, G92.3 (Coordinate System Offset)**](docId:-_dARrxY7XSFSM2Qp6jJL) | Offset coordinate systems and set parameters | | [**G92, G92.1, G92.2, G92.3 (Coordinate System Offset)**](docId:-_dARrxY7XSFSM2Qp6jJL) | Cancel offset coordinate systems and set parameters to zero | | [**G92, G92.1, G92.2, G92.3 (Coordinate System Offset)**](docId:-_dARrxY7XSFSM2Qp6jJL) | Cancel offset coordinate systems but do not reset parameters | | [**G92, G92.1, G92.2, G92.3 (Coordinate System Offset)**](docId:-_dARrxY7XSFSM2Qp6jJL) | Apply parameters to offset coordinate systems | | [**G93, G94, G95 (Set Feed Rate Mode)**](docId\:KTxMEPfXIFobiWMm13_uW) | Inverse time feed rate mode | | [**G93, G94, G95 (Set Feed Rate Mode)**](docId\:KTxMEPfXIFobiWMm13_uW) | Units per minute feed rate mode | | [**G98, G99 (Set Canned Cycle Return Level)**](docId\:Em_0wL_Cftu_Bq5_Bezue) | Initial level return in canned cycles | | [**G98, G99 (Set Canned Cycle Return Level)**](docId\:Em_0wL_Cftu_Bq5_Bezue) | R-point level return in canned cycles | [title] Modbus [path] G-code/Special commands/ Modbus command can be used to communicate with other devices over Modbus protocol. Please note that your controller board needs to have the Modbus feature and that the controller board has to be the master device. :::BlockQuote ModBus \ \ \ \ \ \ \ \ \ \ ::: ### Parameters - **s** defines the slave number. - **f **function number - **a **address - **n** number of bits or registers - **v** value - **u** user variable - **b **baud rate - If not specified, baud rate of 115200 is used - **fb** parity / stop bits configuration designation - If not specified, no parity and 2 stop bits are used - **t** data type used in RMR/3 and WMR/16 - **o** the data ordering used in RMR/3 and WMR/16 ### Supported baud rates - 9600 - 19200 - 38400 - 57600 - 76800 - 115200 ### Supported function numbers | | | | | -- | ---- | ----------------------------- | | 1 | RMC | Read Multiple Coils | | 2 | RDI | Read Discrete Inputs | | 3 | RMR | Read Multiple Registers | | 4 | RMIR | Read Multiple Input Registers | | 5 | WSI | Write Single Coil | | 6 | WSR | Write Single Registers | | 15 | WMC | Write Multiple Coils | | 16 | WMR | Write Multiple Registers | | 17 | RS | Report SlaveID | The abbreviation can be used instead of the number, so `F=RMC` or `F RMC` is equal to `F1` ### Parity / stop bits configuration designations | Setting | Parity | Stop bits | | ------- | ------ | --------- | | E1 | even | 1 | | O1 | odd | 1 | | N2 | none | 2 | | N1 | none | 1 | ### Data type designations (introduced in version 5.3) | Value | Type information | | ----- | --------------------------------- | | u16 | 16-bit unsigned integer (default) | | u32 | 32-bit unsigned integer | | u64 | 64-bit unsigned integer | | i16 | 16-bit signed integer | | i32 | 32-bit signed integer | | i64 | 64-bit signed integer | | d32 | 32-bit floating point number | | d64 | 64-bit floating point number | ### Data ordering designation (introduced in version 5.3) | Value | Ordering information | | ----- | --------------------------------------------------------------- | | n | No reordering of data (default) | | b | Swap the bytes within each register(16-bits) | | w | Swap the placement of each register used in the combined value | | bw | Swap both the register placement and the bytes in each register | ### Example Write single coil :::BlockQuote Modbus s1 f5 a0 v1 ::: Write single coil, baud rate of 19200, even parity with 1 stop bit :::BlockQuote Modbus s1 f5 a0 v1 b19200 fb=e1 ::: Read multiple coils, store beginning at user variable #300 :::BlockQuote modbus s1 f=rmc a0 n8 u300 msg "c0="#300 " c1="#301 " c2="#302 " c3="#303 " c4="#304 " c5="#305 " c6="#306 " c7="#307 ::: Read discrete inputs :::BlockQuote modbus s1 f=rdi a0 n8 u400 msg "i0="#400 " i1="#401 " i2="#402 " i3="#403 " i4="#404 " i5="#405 " i6="#406 " i7="#407 ::: Write single register :::BlockQuote modbus s1 f6 a0 v255 ::: Write multiple coils :::BlockQuote \#500=0 \#501=1 \#502=0 \#503=1 \#504=0 \#505=1 \#506=0 \#507=1 modbus s1 f15 a0 n8 u500 ::: Write multiple holding registers :::BlockQuote \#600 = 1 \#601 = 2 modbus s1 f16 a0 n2 u600 ::: Report slave id :::BlockQuote modbus s1 f17 ::: Read a double value (64-bit floating point) from a slave device with no data reordering. (introduced in version 5.3) :::BlockQuote modbus s1 f3 a0 n1 u700 t=d64 o=n ::: [title] G61, G64 (Path Control Mode and Look Ahead Feed) [path] G-code/Supported G-code/ Ideally one would like to have constant cutting speed during the work and maximum accuracy. This ideal is **physically** not possible, similar to driving a racecar on curvy roads is not possible with constant velocity. It is trivial that it needs to brake in the curves and accelerate on straight roads. If you would do the same speed in the curves as on a straight road, the car will spin out of control and collide. This analogy holds for CNC machines, constant speed and accuracy together are physically not possible. It would require infinite acceleration to go through a corner from one direction to another. In a CNC machine, this would result in position/step loss of stepper motors or high following error with servos. If a motion path consists of small lines (G1) it is even worse than driving a racecar because there is a sharp corner between every line. This is often the case with CAM-generated motion paths (g-code). So a compromise has to be made. There are various options to choose the optimum between accuracy and constant speed or fast speed versus jerkiness. ## G61 `G61` puts the machine into exact path mode, In G61, the motion velocity between motion segments goes to zero, and the end position in corners is exactly reached, use this if you require maximum accuracy. When a workpiece consists of many small lines this gives a quite jerky/vibrating machine because of the continuous acceleration-deceleration-stop behavior. It is more practical to use G64 and G64 P… as specified below. ## G64 G64 is to be used for more smooth and fast motion. There are 4 parameters that can be used, they are explained below individually but they can be combined on one line. ### G64 `G64` without additional parameters switches on continuous/smooth velocity mode. In G64, subsequent moves are blended, when the previous move starts to decelerate and reaches a velocity such that the specified accuracy isn’t violated, the next move starts to accelerate, and the two motions are added. The result is smooth motion with the highest constant speed. The corners however are rounded. The amount of rounding is depending on the max acceleration of the machine. The higher the acceleration, the less rounding. ### G64 P… The optional P value specifies the distance reached to the corner while blending. The next move is blended with the current such that the tool path remains no more than P from the corner. This will cause a velocity ramp down in the corner but not to zero. The figure below is a rectangle of 10x10 milled with `F2000`. This is done with P values from 0.1 to 1, you can see the impact. This gives the best compromise between accuracy and smooth motion. So you can say `G64 P...` is like a compromise between G61 and G64 without P. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/NneXCnLx9_McBc-ZpG-D8_image.png" size="54" width="546" height="500" caption="This figure shows the impact of the P parameter on the amount of rounding." position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/NneXCnLx9_McBc-ZpG-D8_image.png"} You may also conclude here that it is very important to have high acceleration on the machine because we can ramp down faster in the corner and have more accurate corners at higher speeds. ### G64 Q… The optional Q parameter activates an embedded line simplification algorithm, which tries to combine short lines and make one long line. The optional Q parameter gives the tolerance used in the algorithm. Again to reduce the number of small corners. The behavior of a long g-code program with short line segments is further optimized by the look ahead feed, see next page. ## Look Ahead feed To explain this, we will compare a running CNC machine again with driving a race car. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Uc1X1aHXS2fg1-IC5SEBv_image.png" size="40" width="434" height="414" caption="Example race track" position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Uc1X1aHXS2fg1-IC5SEBv_image.png"} The road maximum velocity signs have to be obeyed and you have to drive your car exactly over the white line in the middle of the road. You will try to reach the maximum allowed velocity where possible. When you see a curve coming up ahead, you will brake so that you will not drift off the white line. You will try to look ahead as far as you can see and you take care that you can stop in time if the road suddenly stops. When you would maintain your speed in sharp curves, you will drift off the road possibly resulting in a car accident. When the road has many short curves, then you will not be able to reach the desired speed. The more power you have in the car, the higher speed you will reach because you can accelerate faster. This is a good comparison with a CNC machine, the same issues apply. A machine cannot suddenly change velocity, to reach a velocity the motors must accelerate first for a certain time to reach the velocity. Eding CNC LAF behaves like the ideal racecar driver, it will reach the highest possible velocity without violating the maximum motor accelerations. There is one additional problem while running CNC programs, some programs consist of short line segments. When the line pieces connect tangentially (are in line), then LAF will accelerate through over the lines, reaching the maximum allowed speed. Without LAF the speed would not be reached. The angle to which LAF considers the segments in line is a setup parameter. The theoretical ideal value would be very small so that no acceleration value occurs. More practical values are in the range of 1 to 4 degrees, the experience learns that most machines can handle acceleration spikes up to a certain limit. The value can be set up to 180 degrees, in this case, you must know what you are doing, it can be useful during e.g. foam cutting. Be aware however that if the curve contains real sharp angles that step pulse loss may be the result when using large minimum LAF angles. In practice, we have seen that milling times of complex 3D workpieces can be done within 50% of the time compared to competitors who do not have LAF. With `G64 R...` the LAF angle can be changed in the g-code file. The standard LAF angle is in the software setup. To give some realistic values: A value of 3 is good for most machines. A value of 6 may already give too much Jerky ness on some machines. Still, there are customers using values of 20 here, but they have quite specific machine constructions and applications e.g. dental milling. ### G64 F... The F parameter defines the value of the Accel/Decel filter placed behind LAF. LAF with high R values (Angle) can cause acceleration spikes because LAF will travel through corners without stopping. The F parameter filters the trajectory generated by LAF and takes care the acceleration is never violated. `F1` will give a RAMP time that matches with the max velocity / max acceleration from the setup and so `F1` and maximum speed will lead to the max acceleration that is allowed. Smaller F values filter less. This can be used if the milling velocity is less than the max velocity of the machine. Example: The max velocity in the setup is 200 and the used milling velocity is `F6000` (100 mm/s), Then F0.5 is safe to use. So now you can do this `G64 R100 F1` and you will not get acceleration spikes but a very smooth and fast movement. The price to pay is corner rounding which is depending on the max acceleration of the machine, the higher the max acceleration, the less corner rounding. A good application example is with milling rubber or similar flexible material, the milling speed must be constant otherwise more material is removed in the corners due to the lower speed and the flexibility of the rubber. The `F1` in combination with `R100` will give constant and high speed for good milling surface quality of the rubber. :::hint{type="info"} For milling e.g. rubber when constant speed is more important than rounding. To have an acceptable amount of rounding the machine needs to have very high acceleration. This function was tested and used on a machine with a relatively low speed (100 mm/sec) and very high acceleration (4000 mm/sec \* sec). ::: ### G64 R… The R parameter is the look-ahead feed angle. When subsequent lines/arcs have an angle together less than this value, the trajectory-generator will accelerate through these segments and this way optimizes the production time. With `R0`, LAF is switched off, and with LAF off a (much) lower but more constant speed is achieved. The higher the angle, the higher the speed, but the jerkier the motion becomes because of high acceleration peaks. This needs to be tuned depending on the quality of the machine and the power of the used motors. A compromise is to be found between speed and machine behavior. ### G64 R... S... D... (NEW for V4.03.xx) New algorithm (Still experimental, but successfully used by a few customers): With the standard LAF setting `G64 R...` (no `S...` and no `D...`), the velocity in corners will be zero if the angle between the segments is bigger than LAF angle in the set-up. But there are angles that are big and also smaller angles, so we found a solution where depending on the angle size, the speed in the corner the velocity is limited but not to zero and further limited if the angle gets bigger. This allows faster production, especially for 3D work. Putting a circle to the original path would be a solution. But this cannot be done in real-time and is also not always wanted because we want the contour to be milled as specified in the g-code. However, we can calculate a circle between 2 segments when knowing their start and end vectors. The circle radius can then be used to calculate an allowable velocity in the corner taking the max acceleration into account like this: **Vcorner = SQRT ( Amax \* R) **Where A max is the maximum possible acceleration which is known by the setup and R is the calculated Radius depending on the angle between the segments and the D value supplied in the G64 command. This is basically the idea. If we draw it, it gets more clear: ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/bFMtboPzqNeJQqYcurImx_image.png" size="70" width="1195" height="886" caption position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/bFMtboPzqNeJQqYcurImx_image.png"} **Segment 1** and **Segment 2** are 2 subsequent motion segments. **Alfa** is the change of direction angle between the segments. **Beta** is the angle between the lines to fit the circle. **D** is the user-supplied max deviation between the junction and the circle, this determines how far the junction speed is limited. **R** is the calculated radius from D and Beta. So **D** is the parameter that determines the amount of speed reduction in the corner. Practical values are in the order of 0.01 to 0.0001 for **D**. The smaller the value the smaller the circle radius, the smaller the velocity in the corner becomes. This value needs to be tuned by experimenting on the target machine, if the value is too high the machine will move jerkily. Note that the original path is traveled, but the corner velocity is limited in the corner as if there was an arc between the segments. Both new and old algorithms co-exist in the software. So the user can specify 2 angles and the D parameters now with G64 together with the existing P parameter. ### G64 P... R... S... D... **P**: Parameter for max rounding when blending **R**: LAF angle for standard algorithm where LAF will travel full speed of angle is lower. **S**: 2nd angle, the new algorithm will work between the `R...` angle and `S...` angle. **D**: deviation of the virtual circle in the corner used in the algorithm. Example: `G64 P0.1 R3 S90 D0.001` The machine operates at full speed when the angle is less than the R angle. Reduced speed depends on D when the angle is between the R and S angle. For angles bigger than S... angle blending kicks in and uses the P... as tolerance. ### G64 P... Q... R... S... D... F... There are 6 parameters that can be combined with G64. For normal milling, mostly G64 P... is used. [title] Flow control [path] G-code/Macro programming/ You can use the following flow control commands in a job: **IF\[x]-ELSE-ENDIF** constructs to define x-dependent execution **WHILE\[x]-ENDWHILE** constructs to define x-dependent repeated execution **SUB** \-**ENDSUB **constructs to define a subroutine **GOSUB** \ construct to call a subroutine [title] G90, G91 (Set Distance Mode) [path] G-code/Supported G-code/ To make the current point have the coordinates you want (without motion), program G92 X… Interpretation of RS274/NGC code can be in one of two distance modes: absolute or incremental. To go into absolute distance mode, program G90. In absolute distance mode, axis numbers (X, Y, Z, A, B, C) usually represent positions in terms of the currently active coordinate system. To go into incremental distance mode, program G91. In incremental distance mode, axis numbers (X, Y, Z, A, B, C) usually represent a distance from the current values of the numbers. I and J numbers always represent increments, regardless of the distance mode. [title] TCAGuard [path] G-code/Special commands/ Switches on or off the tool change area guard. This can be used during the rendering process, where the job file is checked for collisions with the machine area and tool change area. :::BlockQuote TCAGuard \ ::: [title] FloodOff [path] G-code/Special commands/ Turns off the flood output on the controller. :::hint{type="warning"} If a custom override for M9 exists, this subroutine is not executed by the FloodOff command. Refrain from using FloodOff in this case. ::: [title] EdingCNC Documentation [path] / On the left side, you can find numerous subjects. On the top left, there is a search bar so you can try to quickly find relevant information. ![](https://archbee-image-uploads.s3.amazonaws.com/CkesZuDJRdQOxJSzCi_9_-0v7vxub8ulGqxDC5aQ585-20241216-220845.jpg) Legacy documents can be found here: [**V4.03 Full manual**](https://edingcnc.com/wp-content/uploads/2021/11/edingcnc_manual_v4.03.pdf) [**Customizing V4.03 manual**](https://edingcnc.com/wp-content/uploads/2021/11/gui-customizing-manual.pdf) [**Basic User Manual V4.03**](https://edingcnc.com/wp-content/uploads/2021/11/Basic_User_manual_EdingCNC_GUI.pdf) [title] G17, G18, G19 (Plane Selection) [path] G-code/Supported G-code/ Program `G17` to select the XY-plane, `G18` to select the XZ-plane, or `G19` to select the YZ-plane. [title] ErrMsg [path] G-code/Special commands/ Shows an error message in the message log and stops current action of the machine. :::BlockQuote ErrMsg "\" ::: ### Parameters - message text parameter specifies the message to be displayed - if [**Variables**](docId\:oqHjs3LLCfQkSac_cemc2) numbers are included outside of quotation marks, this results in the value of that variable being appended to the message e.g. `Msg "value of variable 4000 is " #4000` - if `%t...` is included outside of quotation marks, this results in the tool description of the tool number being appended to the message e.g. `Msg "T1 is " %t1` or `msg "Current tool: " %t#5011` - if `%d` is included outside of quotation marks, this results in the current date and time being appended to the message e.g. `Msg "Time: "%d` will output *Time: 2022-10-28 13:35:52* [title] G80 (Cancel Modal Motion) [path] G-code/Supported G-code/ Program G80 to ensure no axis motion will occur. It is an error if: - Axis words are programmed when G80 is active unless a [**Modal groups**](docId\:wwCKgqqdL1JYxmBZy8GYf) 0 code is programmed which uses axis words. [title] G20, G21, G70, G71 (Length Units) [path] G-code/Supported G-code/ Program `G20` to use inches for length units. Program `G21` to use millimeters. It is usually a good idea to program either `G20` or `G21` near the beginning of a program before any motion occurs, and not to use either one anywhere else in the program. It is the responsibility of the user to be sure all numbers are appropriate for use with the current length units. `G70` and `G71` are added for CAM software compatibility. [title] SP (Store Position) [path] G-code/Special commands/ Store the current work position in a text file. :::BlockQuote SP "\" \[mode] ::: ### Parameters - The file path parameter is a text parameter that specifies the file path to be used to write to - mode parameter needs to be a value of either 0 or 1 - **0** specifies that the file is to be overwritten - **1** specifies that the file is to be appended to - If this parameter is omitted, the file is appended to [title] G54 - G59.3 (Select Coordinate System) [path] G-code/Supported G-code/ To select coordinate system 1, program G54, and similarly for other coordinate systems. The system-number-G-code pairs are (1`G54`), (2`G55`), (3`G56`), (4`G57`), (5`G58`), (6`G59`), (7`G59.1`), (8`G59.2`), and (9`G59.3`). It is an error if: - one of these G-codes is used while cutter radius compensation is on. [title] PC Requirements [path] Getting started/ | | Minimum requirement | Recommended | | ---------------- | ------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- | --------------------------------- | | Processor | Intel Core i3 / 1.4 GHz | Intel Core i3 / 2.0 GHz or better | | Memory | 4GB RAM | 8GB RAM or more | | Graphics | Any with OpenGL2.1 support or better | | | Display | 1280 x 768 | | | Operating System | Windows 10 ¹ 32 or 64-bit | | | Connection Ports | 1x Free USB 2.0 for USB controllers.
1x Free Ethernet port for Ethernet controllers.
1x Additional free USB 2.0 if a wireless pendant is used.
1x Additional free USB 2.0 if a UIO-10 or Operator Panel is used. | | | Storage | At least 250MB free, SSD is strongly recommended | | | Speakers | Only for the "probe beep" feature | | 1: Windows XP supported up to software version 4.03.46 [title] User interface [path] Getting started/ [title] Service tab [path] Getting started/User interface/1. Tab overview/ ![](https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/JEna4hLUg5mlwxb1vJNcn_service.png) The service tab shows information relevant to servicing the machine. It shows the times and distances that the machine has run. # Service status ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/Tt_6NwMKDtQIh9qMLxjK6_service-service-status.png" signedSrc size="70" width="876" height="560" position="flex-start" caption} - **Job time \[h]** - The time in hours that the machine has performed jobs since receiving service. - **Job distance \[unit]** - The distance that the machine has cut in the units selected by the user since receiving service. - **Number of jobs done** - The number of jobs the machine has performed since receiving service. - **Reset** - Pressing this button resets the service status when the machine has received service. # Machine working status totals ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/yaT4CHJsBLyC6BTnVvthj_service-machine-working-status-totals.png" signedSrc size="70" width="876" height="560" position="flex-start" caption} - **Total job time \[h]** - The total time in hours that the machine has performed jobs - **Total distance \[unit]** - The total distance that the machine has cut in the units selected by the user - **Total number of jobs done** - The total number of jobs the machine has performed # Service parameters ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/EULUcj7pl0PL0if4G_gXH_service-service-parameters.png" signedSrc size="70" width="876" height="560" position="flex-start" caption} - **Service time interval \[h]** - The time interval for service, the software will show a message when this time has elapsed at the end of a job. - **Service distance interval \[unit]** - The traveled distance interval for service, the software will show a message to indicate the machine needs service. - **Save service interval changes** - Pressing this button saves the interval settings # Pump parameters ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/vb0tN3HRY9xEM90ZM0xKy_service-pump-parameters.png" signedSrc size="70" width="876" height="560" position="flex-start" caption} Configuring the pump settings is explained on its specific page [**Configuring an automatic oil pump**](docId:0ZdtgcXnxakIhbvmR1Yph). [title] M10, M11; Laser control (CNC7xx series only) [path] G-code/Supported M-codes/ For the ***CNC7xx controller***, we have extra commands to control a laser 'on-the-fly' eg. for engraving. Please note, to use them, an extra command is required to be executed first: `LaserEngrave XY`. ## M10 - Laser off `M10` - laser off ## M11 - Laser on :::BlockQuote M11 S\<0-100> - to switch laser on ::: M11 will turn the laser on at a specified power or change the power. :::BlockQuote S-parameter: The percentage 0-100% at which the laser power needs to be set. ::: ## Example This enables the feature where motion can be performed without a stop in between: :::BlockQuote LaserEngrave ON M10 G1 F... X... M11 G1 X... M10 X... G1 X... LaserEngrave OFF M30 ::: The laser on/off `M11` and `M10` are executed while moving exactly at the right position. It is possible to do a lot of small line moves (G1s) with these laser commands in between. The motion will continue while doing this with constant speed. So this is ideal for photo laser engraving. ## See also Laserengrave [title] G76 (Threading lathe) [path] G-code/Supported G-code/ ### G76 P... Z... I... J... R... K... Q... H... E... L... **P** Pitch **Z** driveline endpoint **I** Outside thread diameter, always positive. **J** First cut is **J** beyond **I**, always positive. **R** Depth regression, use 1.0 for constant cutting depths or discard the parameter. **K** Full thread depth beyond thread peak, always positive. **Q** Compound slide angle, typical 30. **H** Additional spring passes at full depth, use 0 for none. **E** Taper distance along the drive line. **L** Taper place, none, enter, exit, both. :::BlockQuote ;Create a thread from z=20 to z=10, outside diameter=15, inside diameter=14, 10 passes. G0 X20 Z20 G76 P1.0 Z10 I15 J0.1 K1.0 ::: It is an error if: - The active plane is not the ZX plane - Other axis words, such as `X...` or `Y...`, are specified - The `R...` degression value is less than 1.0. - All the required words are not specified - `P...`, `J...`, `K...` or `H...` is negative - `E...` is greater than half the drive line length The “drive line” is a safe line outside the thread material. The “drive line” goes from the initial location to the `Z...` value specified with G76. The Z extent of the thread is the same as the drive line. The “thread pitch”, or distance per revolution, is given by the `P...` value. The “thread peak” is given by the `I...` value, which is an offset from the drive line. A negative I value indicates external threads and a positive I value indicates internal threads. Generally, the material has been turned to this size before the G76 cycle. The “initial cut depth” is given by the `J...` value. The first threading cut will be J beyond the “thread peak” position. `J...` is positive, even when `I...` is negative. The “full thread depth” is given by the `K...` value. The final threading cut will be K beyond the “thread peak” position. `K...` is positive, even when `I...` is negative. The “depth degression” is given by the `R...` value. `R1.0` selects constant depth on successive threading passes. `R2.0` selects constant area. Values between 1.0 and 2.0 select decreasing depth and increasing area. Values above 2.0 select decreasing area. Beware that unnecessarily high degression values will cause a large number of passes to be used. :::hint{type="info"} (degression = a descent by stages or steps.), every next cutting pass less material is removed during the cutting process. ::: The “compound slide angle” `Q...` is the angle (in degrees) describing to what extent successive passes should be offset along the drive line. This is used to cause one side of the tool to remove more material than the other. A positive Q value causes the leading edge of the tool to cut more heavily. Typical values are 29, 29.5, or 30. The number of “spring passes” is given by the `H...` value. Spring passes are additional passes at full thread depth. If no additional passes are desired, program `H0`. Tapered entry and exit moves can be programmed using `E...` and `L...`. `E...` gives a distance along the drive line used for the taper. `E0.2` will give a taper for the first/last 0.2 length units along the thread. `L...` is used to specify which ends of the thread get the taper. Program `L0` for no taper (the default), `L1` for entry taper, `L2` for exit taper, or `L3` for both entry and exit tapers. The tool will pause briefly for synchronization before each threading pass, so a relief groove will be required at the entry unless the beginning of the thread is past the end of the material or an entry taper is used. Unless using an exit taper, the exit move (traverse to original X) is not synchronized to the spindle speed. With a slow spindle, the exit move might take only a small fraction of a revolution. If the spindle speed is increased after several passes are complete, subsequent exit moves will require a larger portion of a revolution, resulting in a very heavy cut during the exit move. This can be avoided by providing a relief groove at the exit, or by not changing the spindle speed while threading. The sample program g76.ngc shows the use of the G76 canned cycle and can be previewed and executed on any machine using the sim/lathe.ini configuration. ::Image[]{src="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/k3wwM8e7YGUo64Vr_d47l_image.png" size="70" width="602" height="238" caption="Figure: G76 canned cycle" position="flex-start" signedSrc="https://archbee-image-uploads.s3.amazonaws.com/wP9peVc2bAVBPOh6IboCS/k3wwM8e7YGUo64Vr_d47l_image.png"} This is how it works: 1. Before the start, the spindle rate is measured. 2. The feed for de z-axis is calculated: F = pitch \* spindleRate 3. The controller is programmed such that a movement is started on the spindle pulse. 4. The movement is calculated and sent to the machine. 5. The movement is started when the spindle pulse passes. 6. Before the treading starts, the spindle rate is measured, averaged, and the feed is calculated from this. Not that the inside and outside thread diameter is determined by the start position, the position before G76, and the I, and K parameters. [title] SetPos (set position) [path] G-code/Special commands/ To set the current position of an axis to a certain value, program `SetPos X... Y... Z... A... B... C...`, where all axis words are optional, except that at least one must be used. It is an error if: - All axis words are omitted. ### Example Set the machine position of the X axis to 100 :::BlockQuote SetPos x100 ::: Set the machine position of the X axis to the value stored in var #4000 :::BlockQuote SetPos x#4000 ::: Set the machine position of multiple axes :::BlockQuote Setpos x#4000 y#4001 z#4002 a0 b0 c10 ::: Read a position from a Modbus device and set the position to this value; this can be used in a homing routine, for example. For more information on the modbus command reference the [**Modbus**](docId\:dkUObkUk2JT5u2v2PkZF4) document. :::BlockQuote Modbus s1 f3 a0 n1 u700 t=d32 SetPos x#700 ::: [title] WarnMsg [path] G-code/Special commands/ Shows a warning message in the message log. :::BlockQuote WarnMsg "\" ::: ### Parameters - message text parameter specifies the message to be displayed - if [**Variables**](docId\:oqHjs3LLCfQkSac_cemc2) numbers are included outside of quotation marks, this results in the value of that variable being appended to the message e.g. `Msg "value of variable 4000 is " #4000` - if `%t...` is included outside of quotation marks, this results in the tool description of the tool number being appended to the message e.g. `Msg "T1 is " %t1` or `msg "Current tool: " %t#5011` - if `%d` is included outside of quotation marks, this results in the current date and time being appended to the message e.g. `Msg "Time: "%d` will output *Time: 2022-10-28 13:35:52* [title] M20, M21, M22 (Torch height control / Plasma THC) [path] G-code/Supported M-codes/ `M20` - THC on `M21` - THC off `M22 Q...` - THC setpoint voltage [title] S (Tool intensity/spindle speed) [path] G-code/Other input codes/ The S parameter in G-code can be described as a value that controls the primary output intensity or speed of the machine's tool or device, such as spindle speed in milling machines, or laser intensity in laser cutters and engravers. This parameter can be adapted to suit different machines and is used to manage the performance or effectiveness of the working tool or device within the machine's operation. To set the speed in revolutions per minute (rpm) of the spindle, program `S...`. The spindle will turn at that speed when it has been programmed to start turning. The S-word can be used regardless of whether the spindle is turning or not. If the speed override switch is enabled and not set at 100%, the speed will be different from what is programmed. It is permitted to program `S0`; the spindle will not turn if that is done. The controllers that support PWM output will have their PWM value set corresponding to the requested spindle speed if the spindle is turned on. An error is issued if: • the S value is negative. [title] G98, G99 (Set Canned Cycle Return Level) [path] G-code/Supported G-code/ When the spindle retracts during canned cycles, there is a choice of how far it retracts: 1. retract perpendicular to the selected plane to the position indicated by the R-word 2. retract perpendicular to the selected plane to the position that axis was in just before the canned cycle started (unless that position is lower than the position indicated by the R-word, in which case use the R-word position). To use option (1), program G99. To use option (2), program G98. Remember that the R-word has different meanings in absolute distance mode and incremental distance mode. [title] G50, G51 (Scaling) [path] G-code/Supported G-code/ `G50` turns scaling off. ### UNIFORM Scaling `G51 P... I... J...` P is the scaling factor. ### NON-UNIFORM Scaling (X, Y different, only applicable when NO Arcs) `G51 X... Y... I... J...` X is the scaling factor for X coordinates. Y is the scaling factor for Y coordinates. I is the X coordinate scaling point J is the Y coordinate scaling point :::hint{type="info"} When used in combination with [**G68 (Coordinate System Rotation)**](docId\:VpyIB1fwdN7BZilxiuRb6), the rotation point and scaling point are the same. ::: [title] G0 (Rapid Linear Motion) [path] G-code/Supported G-code/ For rapid linear motion, program `G0 X... Y... Z... A...`, where all the axis words are optional, except that at least one must be used. The G0 is optional if the current motion mode is G0. This will produce coordinated linear motion to the destination point at the current traverse rate (or slower if the machine will not go that fast). It is expected that cutting will not take place when a G0 command is executing. An error occurs if: • All axis words are omitted. If cutter radius compensation is active, the motion will differ from the above; see Appendix A. If [**G53 (Move in Absolute Coordinates)**](docId\:LcnWMZ2I2Ii08f90oBaL-) is programmed on the same line, the motion will also differ. [title] SetAcc (set acceleration) [path] G-code/Special commands/ Changes in the maximum acceleration of an axis. :::BlockQuote SetAcc \ \ ::: ### Example `SetAcc Y 400` Set the max acceleration value for the Y-Axis to 400. [title] Laserengrave [path] G-code/Special commands/ laserengrave enables the laser motion mode. Use this command in MDI or in G-code at the start of a jobThis command changes the working mode of your controller board, restricting it to XYZ axes. ## Laserengrave XY Turns the laser engraving mode on ## laserengrave OFF Turns the laser engraving mode on [title] MistOn [path] G-code/Special commands/ Turns on the mist output on the controller. :::hint{type="warning"} If a custom override for M8 exists, this subroutine is not executed by the MistOn command. Refrain from using MistOn in this case. ::: [title] HomeIsEStop [path] G-code/Special commands/ The HomeIsEStop feature can be used to guard the home sensor inputs while operating the machine. When the feature is turned on using the `HomeIsEStop on` command, any activation of one of the sensors triggers an error, causing the machine to stop moving. Because the machine needs to be able to home correctly, it is important to turn the feature off before starting any home operation. This can be done using the `HomeIsEStop off` command. It is advisable to place these commands at the start and end of all homing subroutines (either in the `sub home_all` or in each `sub home_x, y...`). Switches ON or OFF the "Home Switch triggers E-Stop" feature. :::BlockQuote HomeIsEStop \ ::: [title] G28, G30 (Return to Home) [path] G-code/Supported G-code/ Two home positions are defined (by [**System-Parameters/Variables**](docId\:oqHjs3LLCfQkSac_cemc2) `#5161` to `#5166` for G28 and variables `#5181` to `#5186` for G30). The variable's values are in terms of the absolute coordinate system but are in unspecified length units. To return to the home position by way of the programmed position, program `G28 X... Y... Z... A...` (or use G30). All axis words are optional. The path is made by a traverse move from the current position to the programmed position, followed by a traverse move to the home position. If no axis words are programmed, the intermediate point is the current point, so only one move is made. The order of Z depends on its position, if the end position is higher than the current Z position Z will move first, otherwise Z will move last, this is to prevent collisions. :::hint{type="warning"} Addition for lathe: For a lathe the X axis is moved first, the assumption is that X moves away from the turning center. ::: [title] M48 - M53 (Feed-Speed Override Control) [path] G-code/Supported M-codes/ `M48` Enable feed and speed override, set back to last user feed override value. `M49` Disable feed and speed override and set to 100% `M50 P...` Set feed Override to a given P value, if the P value is less than zero feed override is disabled and the value remains as is. `M51 P...` Set speed Override to given P value, if the P value is less than zero speed override is switched off. `M52 P...`Enable feed Override by analog input. `M52 P0` disables feed override by analog input. P1 is optional. `M53 P...` Enable feed Hold input. M53 P0 disable feed Hold input. P1 is optional. To enable the speed and feed override switches, program `M48`. To disable both switches, program `M49`. [title] G43, G43.1, G49 (Tool Length Offset) [path] G-code/Supported G-code/ 1. To use the tool offset of the tool in the spindle use `G43`. This assures that always the tool length of the tool in the spindle is compensated. 2. To use a tool length offset from the tool table, program `G43 H...`, where the H number is the desired index in the tool table. ( H = 1-99) 3. To use dynamic tool compensation (not from the tool table), use `G43.1 I... K...` where `I...` gives the tool X offset (turning) and `K...` gives the tool Z offset (for turning and milling) :::hint{type="warning"} Warning: If you use option 2 or 3, the tool-length compensation will not adapt to the new tool after `M6T…` ::: To have no tool length offset compensation, program `G49` [**System-Parameters/Variables**](docId\:oqHjs3LLCfQkSac_cemc2) `#5401` to `#5499` is the tool length of tool 1-99 Variables `#5501` to `#5599` is the tool diameter of tool 1-99 Variables `#5601` to `#5699` is the tool x-offset (width for turning) offset. The variables can be modified runtime (in the G-Code file) if needed to compensate for tool-wear. [title] LogFile [path] G-code/Special commands/ Specifies the file to be used by the [**LogMsg**](docId:66N8dnIbKJn8fJX6mVJ-R) command. :::BlockQuote LogFile "\" \ ::: ### Parameters - the file path parameter is a text parameter that specifies the file path to be used to write to - mode parameter needs to be a value of either 0 or 1 - 0 specifies that the file is to be overwritten - 1 specifies that the file is to be appended to ### Example :::BlockQuote LogFile "C:\log.txt" 0 ::: :::BlockQuote LogFile "log.txt" 1 ::: [title] G96, G97 (Spindle Control Mode) [path] G-code/Supported G-code/ Two spindle control modes are possible, depending on the mode the spindle speed is calculated differently: ### G96 (Only for Lathe) Select constant surface speed, S is now specified as meters per minute in mm mode (G21) or Feet per minute in inch mode (G20). This means that the spindle speed is adapted automatically when the Radius changes. Suppose you program `G96 S150` in millimeter mode, the spindle speed is calculated by: RPM = S / (2 \* PI \* X), and X is the radius. So your X zero must be where the diameter is zero. Example: Your actual X position is 100 (100 millimeters = 0.1 meter), and you program `G96 S150 D1000`, this would result in a spindle RPM of 150 / (2 \* PI \* 0.1) = 238.7 rev/min. D1000 limits the maximum speed to 1000 RPM. ### G97 `G97` is normal RPM mode, and `S...` specifies the RPM. [title] G68 (Coordinate System Rotation) [path] G-code/Supported G-code/ ### G68 X... Y... Z... I... J... K... R... `X... Y... Z...` Optionally points to a rotation point, if not given, the current Work Zero point is used. `I... J... K...` Optionally, without I, J, or K the rotation takes place in the actual plane [**G17, G18, G19 (Plane Selection)**](docId\:Uo-PghD6GWTJ4p9XJ2NzP). Either `I1`, `J1`, or `K1` can be used, not a combination. `I1` specifies a rotation about X in the YZ plane, `J1` rotates about Y in the XZ plane, and `K1` rotates about Z in the XY plane. `R…` Is the rotation angle in degrees, positive is counter-clockwise while negative is clockwise. [title] T (Tool number) [path] G-code/Other input codes/ The T parameter in G-code is a value that represents the tool selection or tool change command, which is used to specify the machine's tool or device being employed for a particular operation. This parameter can be applied to various machines and processes, such as milling, turning, or laser cutting, where multiple tools or devices may be used within a single program. The T parameter is typically followed by a tool number, which corresponds to a specific tool in the machine's tool library or carousel. It plays a significant role in managing the sequence of operations and ensuring that the correct tool is engaged for each process in a multi-tool machining setup. To select a tool, program `T...`, where the number is the tool changer slot for the tool. The tool is not changed until an [**M6 (Tool Change)**](docId\:kQG7dD1dpwUw3hchbArUT) command is programmed. The T-word may appear on the same line as the `M6` command or on a previous line. It is possible to program a T word more than once before a tool change takes place, but only the last issued statement is taken into consideration. The carousel may move a lot, but only the most recent T-word will take effect at the next tool change. It is OK to It is possible to issue `T0` this means that no tool will be selected. This is useful if the spindle needs to be empty after a tool change. An error occurs if: • a negative T number is used, • a T number larger than the number of slots in the tool changer is used. [title] Vacuum [path] G-code/Special commands/ Switches on or off vacuum sections that are used this is especially useful for large machines with different vacuum sections. The software will determine in which section will be machined, then this command will switch only the used sections. :::BlockQuote Vacuum \ ::: ### Enabling the feature The configuration of the vacuum sections is currently not available in the GUI settings, and it must be entered in the configuration file, which contains all settings. The definition of the vacuum sections is manually in the cnc.ini for version 4 of the software and server.ini file inside the *config* directory for version 5 of the software, under section *\[VACUUMBED]*. To enable this feature please modify the files (while the software is turned off) by specifying `automaticMode = 1` to turn the automatic management of vacuum sections on, and specify the number of vacuum sections: :::BlockQuote \[VACUUMBED] automaticMode = 1 numberOfSections = 14 ::: Afterwards please start the software. The software will modify the file further with definitions of individual sections. Close the software and open the file again to modify the individual sections: :::BlockQuote \[VACUUMBED] ... section\_1\_OutputID = 101 ;0: none, 1-10: AUX1-AUX10, GPIO101 GPIO408 section\_1\_XPosition = 0.000000 section\_1\_YPosition = 0.000000 section\_1\_XWidth = 999.000000 section\_1\_YWidth = 3000.000000 ::: [title] Msg [path] G-code/Special commands/ Shows a message in the message log. :::BlockQuote Msg "\" ::: ### Parameters - message text parameter specifies the message to be displayed - if [**Variables**](docId\:oqHjs3LLCfQkSac_cemc2) numbers are included outside of quotation marks, this results in the value of that variable being appended to the message e.g. `Msg "value of variable 4000 is " #4000` - if `%t...` is included outside of quotation marks, this results in the tool description of the tool number being appended to the message e.g. `Msg "T1 is " %t1` or `msg "Current tool: " %t#5011` - if `%d` is included outside of quotation marks, this results in the current date and time being appended to the message e.g. `Msg "Time: "%d` will output *Time: 2022-10-28 13:35:52* Example :::BlockQuote Msg "Spindle dust cap lowered" ::: :::BlockQuote Msg "The value of #1 = "#1" and the value of #2 = "#2 ::: [title] Exec [path] G-code/Special commands/ Starts an external program within the job/macro and waits until the program exits. The return value of the program is stored in [**Variables**](docId\:oqHjs3LLCfQkSac_cemc2) `#5399` :::BlockQuote Exec "\" "\" \ ::: The maximum wait time is 10 minutes. ### Example :::BlockQuote Exec "notepad.exe" "hello.txt" 6000 ::: This executes notepad.exe and waits 1 minute for it to exit. An error is generated if it does not exit within the specified time. [title] G53 (Move in Absolute Coordinates) [path] G-code/Supported G-code/ For the linear motion to a point expressed in absolute coordinates, program `G1 G53 X... Y... Z... A…` (or use [**G0 (Rapid Linear Motion)**](docId\:sMEIPmfNLzqwnk8pfSSZC) instead of [**G1 (Linear Motion Feed at Feed Rate)**](docId\:rIq0kXPLy7LFjPIEIK24B)), where all the axis words are optional, except that at least one must be used. The G0 or G1 is optional if it is the current motion mode. G53 is not [**Modal groups**](docId\:wwCKgqqdL1JYxmBZy8GYf) and must be programmed on each line on which it is intended to be active. This will produce coordinated linear motion to the programmed point. If G1 is active, the speed of motion is the current feed rate (or slower if the machine will not go that fast). If G0 is active, the speed of motion is the current traverse rate (or slower if the machine will not go that fast). It is an error if: - G53 is used without G0 or G1 being active, - G53 is used while cutter radius compensation is on. [title] G1 (Linear Motion Feed at Feed Rate) [path] G-code/Supported G-code/ For linear motion at feed rate (for cutting or not), program `G1 X... Y... Z... A...`, where all the axis words are optional, except that at least one must be used. The G1 is optional if the current motion mode is G1. This will produce coordinated linear motion to the destination point at the current feed rate (or slower if the machine will not go that fast). It is an error if: - All axis words are omitted. If cutter radius compensation is active, the motion will differ from the above; see Appendix A. If [**G53 (Move in Absolute Coordinates)**](docId\:LcnWMZ2I2Ii08f90oBaL-) is programmed on the same line, the motion will also differ. [title] Dwell [path] G-code/Special commands/ The `dwell