2. assembly and preparation of the 3D measuring probe

The 3D finder must be mounted next to the milling cutter on a fixing rail. By lowering the 3D Finder onto this rail - whether manually or automatically - the device is ready for use. It is essential that the 3D finder is always lowered lower than the longest milling cutter and is always set to the same position.

4. use of the 3D touch probe in the cncGraF software

The 3D touch probe is operated in the cncGraF software via integrated dialogues. The following functions are implemented:

• Determination of the outer corners including Z-height
• Determining the inner corners
• Determination of the outer centre of the circle including Z-height
• Determining the centre of the circle inside
• Determining the centre of a rectangle outside including Z-height
• Determining the centre of a rectangle inside
• Surface measurement in the X, Y and Z axes
• Scanning the outer corner and the side: Based on the values determined, the drawing is positioned so that it corresponds to the alignment of the material on the machine.

Screenshots of the various dialogues can be found in the gallery below.

Tip: Checking the 3D Finder before touching it

Before the scanning process is started, you can check the functionality of the 3D finder.

In each dialogue window for these functions, the status of the input is shown by a green round dot. If you press the 3D finder with your finger, the status should change (the green dot goes out or lights up).

5. use measurement results for zero point determination

The measurement results can be used to determine the zero point either automatically or manually. For manual zero point determination, the dialogue window „ Set zero point “ must be called up after the successful measurement. In this dialogue, the option „Last scan position“ is active and already preselected in the „Coordinates“ option selection group for existing measurement results.

Automatic zero point determination can be activated. The corresponding option can be found in the window frame of every dialogue relating to measuring with the 3D measuring probe.

6. summary

We hope that this guide has provided you with helpful information on using the 3D touch probe and the cncGraF software for zero point determination and measurement.

Yours sincerely, Your BOENIGK-electronics Team

G-code drilling cycle: G81 and G82

The simplest drilling cycle is the G-code command G81. This drilling cycle is used for simple drilling, while the command G82 additionally enables drilling with a dwell time at the bottom of the hole.

The G81/G82-command has the following syntax:
G98(G99) G81(G82) X Y Z R F (P)

The parameters are as follows:

1. With the parameter G98/G99 The retraction height to which the tool should move after the drilling cycle is defined.
   G98 - The starting height (starting height) is approached after the drilling cycle.
   G99 - the retraction height (defined in the parameter R) is approached after the drilling cycle.
   Note: If no parameter G98 or G99 is specified, then G98.
2. The parameters X,Y,Z:
   X - Position X
   Y - Position Y
   Z - Depth Z (absolute)
3. R - Incremental value of the retraction plane, in relation to the starting point in the Z-axis
4. F - Feed speed in mm/min
5. The G-Code drilling cycle G82 also has the parameter P for waiting time in milliseconds
   (1000ms = 1sec.) at the bottom of the hole

In the example above, a hole is drilled at positions X10 and Y10, with a drilling depth of 3 millimetres. In addition, a dwell time (parameter P) of 100 milliseconds, during which the milling machine pauses. At the end of the drilling process, the starting height, which in this case is Z=0, is approached again.

G-Code command: G80

The drilling cycle is started with the command G80 or by another G-code command such as G00 or G01 deleted.

G-code drilling cycle: G83 Deep-hole drilling with chip removal

Compared to the drilling cycles G81/G82 this drilling cycle contains an additional parameter Q. The parameter Q is used to control the chip removal. As chips are produced during drilling, this drilling cycle is particularly recommended for deep hole drilling.

The G83-command has the following syntax:
G98(G99) G83 X Y Z R F P Q

The parameters are the same as for the G-code drilling cycle G81/G82, but with an additional parameter:
Q - Drilling depth per infeed defined in millimetres

In the example above, a hole is drilled at positions X10 and Y10, with a drilling depth of 9 millimetres. In addition, a dwell time of 100 milliseconds is executed at the bottom of the hole, during which the milling machine pauses. The hole is drilled with a triple infeed, as the plunge depth per infeed is 3 millimetres (parameter Q). At the end of the drilling process, the initial height Z=0 is approached. The graphic below explains the parameter Q.

G-code drilling cycle: G73 Deep hole drilling

This drilling cycle corresponds to drilling cycle G83, with the difference that a short lift-off distance is approached after each chip removal with Q. The setting for the lift-off distance can be made in cncGraF under „Settings -> Options -> G-Code“.

We hope that this article will help you to quickly find your way around the world of drilling cycles.

Yours sincerely, Your BOENIGK-electronics Team

G-Code: Subroutines

First, we add a subroutine. We will use the G-code example from the first part of this series „CNC programming: Learn G-code - Quick and easy„. The extended G-code lines are colour-coded in Light red highlighted. The G-code then looks like this:

The G-code (see above) describes the processing of a rectangle and a circle, whereby the two shapes are described in the sub-programme 1 are defined. The sub-programme is started with the command P1 in the main programme.

The definition of the sub-programme begins with the command M99 P1 and ends with M99. All subroutines are located at the end of the main programme, i.e. after the command M30, which marks the end of the main programme. The number of the sub-programme is indicated by the number after ‚P‚ labelled - in this case 1.

G-code subroutines have the following structure:

G91 ; Relative dimensioning (incremental dimension) is activated
; Main programme
P1 ; Subprogramme 1 is called up
; Main programme
M30 ; End of the main programme

M99 P1
; Contents of the sub-programme 1
M99

Note: Please note that at the beginning of the main programme the command G91 must be set to activate relative dimensioning (incremental dimension). All subsequent coordinate specifications are therefore relative values. This is necessary so that the sub-programmes can be placed at any position.

Sub-programme management

The CNC control software cncGraF has an integrated sub-programme management function. All subroutines can be saved there. In such a case, the subroutine does not have to be contained in the G-code file; instead, the subroutine is only called in the main programme with the G-code command ‚P‚ and the sub-programme number (here P1).

Note: If a sub-programme with the same sub-programme number (the number after ‚P‚) is present both in the G-code file and in the subroutine management, the subroutine from the G-code file is used. The software first searches for the subroutine in the file and only then in the G-code management. This makes it possible to ‚overwrite‘ the subroutine in the administration.

G-Code: Loops

To duplicate the shapes defined in the subroutine, the subroutine must be called several times. This is done with the G-code commands G25 Q and G26 realised for loops.
The G-code section in the main programme then looks as follows:

G25 Q4
P1 ; Subprogramme 1 is called up
G00 X110
G26

With G25 Q and G26 a loop is programmed. G25 defines the start of the loop, and with G26 the loop is ended. The parameter Q defines the number of runs. In our example 4 runs are defined. After each sub-programme call, there is a relative position shift in X for the next sub-programme with the line: G00 X110.

What is an R parameter?

An R parameter is a placeholder (variable) in the range from R1 to R999 in which a value is saved. Example: R10 = 99.567. This line defines the parameter R10, which represents the value 99.567 contains.
By calling the R parameter (here R10), its value can be accessed in the G code. Please note the following when using the R parameters:

• Basic arithmetic operations Addition, subtraction, multiplication and division can be executed within a parameter. When calculating the values, the rule „Dot before dash“ is applied. The brackets are not supported.
  Example:
  R56 = 10/2 - 2*2
  The result is 1
• R parameters can be used within the calculation.
  Example:
  R55 = 10
  R56 = R55/2 - 2*2
  The result is 1
• R parameters can be assigned in the following places in the G code:
  Command G00, example G00 X=R10
  Command G01, example G01 X=R10 Y=R11 + 6 / 2
  Command G02/G03 X/Y (arc commands), example: G02 I20 J20 X=R10 Y=R10
  Command G25 Q (loop), example: G25 Q=R4
  Command G53-G60 X/Y/Z, example G54 X=R20
  IF statement command, example: $IF R100==1
• R parameters are global parameters, i.e. if they are defined at the beginning of the G-code file, they are available for the entire file.
• R parameters can also be used in sub-programmes.
• The values of the R parameters are displayed at the bottom of the status bar of the text editor (see screenshot below)

In the following, we add parameters to our loop. The G-code snippet then looks like this in the main programme:

R4=4 ; R4 Parameter (placeholder) with the value 4 as the number of passes create
R5=110 ; R5 parameter (placeholder) with the value 110 for new X position of the sub-programme

; Assignment of the value via parameter R4
G25 Q=R4
P1 ; Subprogramme 1 is called up
G00 X=R5 ; Relative displacement, defined in the R5 parameter
G26

What is an IF statement?

The IF statement is used to check a condition. If this condition is fulfilled, the commands within the condition are executed. The following operations are available:
equal ==
unequal !=
greater than or equal to >=
less than or equal to <=

The IF statement consists of the following commands $IF $ENDIF $ELSE $ELSEIF. The IF statement must stand alone in the line. IF statement can be contained in the main programme and in the sub-programme.

Example 1: $IF $ENDIF

R57=10 ; Create parameter R57 (placeholder) with the value 10

$IF R57== 10
; This G-code content is executed because parameter R57 has the value 10 (equals is fulfilled)
$ENDIF

Example 2: $IF $ELSEIF $ENDIF

R57=9
$IF R57<=9
; This content is executed because parameter R57=9 (less than or equal to is fulfilled)
$ELSEIF R57>=10
; This content is NOT executed because parameter R57 has the value 9.
; Changing the value to 10 or higher in parameter R57 means that
; this content is executed.
$ENDIF

Please note! An IF statement within another IF statement is not supported (see table below).

Several R parameters, loops and IF statements are used in the G code (see above). The G-code file can be changed very easily using the R parameters. The R parameters R3 and R4 define the number of parts in X and Y. The R parameters R5 and R6 determine the distance between the parts in X and Y, and the last parameter, R7, defines whether a circle is to be output or not (see IF statement in the subroutine).

Summary

In this blog article, we have looked at the various facets of CNC programming. Starting with the basics, which are explained in the article
‚CNC programming: Learn G-code - Quick and easy‚ to advanced topics such as R parameters, loops and IF statements. We have thus covered the breadth and depth of CNC programming.

We hope that this blog article will help you to achieve the desired success.
Yours sincerely, Your BOENIGK-electronics Team

What do I need for G-code programming?

The G-code consists of a series of text instructions that are stored in a text file (ASCII file). The CNC machine executes these commands in the sequence from the beginning of the text file to the end.

Only a text editor is required for CNC programming and G-code. However, as a visual check of the programmed G-code is necessary, a CNC simulation must be used.

Free G-code simulator: cncGraF

The CNC control software cncGraF is ideal for training purposes: It offers a built-in G-code simulator and CNC machine emulator, is free of charge (freeware) and does not require a real CNC controller.

Click here to download cncGraF free of charge.

The screenshot below presents CNC control cncGraF, including the G-code text editor and the 2D view. The CNC machine emulator is switched on and the G-code file is executed in emulator mode.
To find out more, click on the blog article
cncGraF: Free G-code simulator and CNC machine emulator.

Structure of a G-code file

The following example of a G-code file is available:

; G-code file: Production of a rectangle, created on 24/10/2023
; Activate tool number 1
T1
; Lift the tool at rapid speed to the height Z = 10 mm above the zero point
G00 Z10
; Move to position X = 10 and Y = 10 at rapid speed
G00 X10 Y10
; Switch on the work spindle with M3 at a speed of 20000 rpm
M3 S20000
; Wait 5 seconds until the spindle speed is reached
G04 H5
; plunge 2 mm into the workpiece at a feed rate of 600 mm per minute
G01 Z-2 F600
; Traverse rectangle 100×100 mm at a feed rate of 600 mm per minute
G01 X110
G01 Y110
G01 X10
G01 Y10
; Lift the tool at rapid speed to the height Z = 10 mm above the zero point
G00 Z10
; End of programme
M5 M30

This G-code describes the machining of a rectangle with a CNC machine. The G-code begins with comments that are separated by a semicolon (;) are labelled. These comments are not relevant for the machine, but help the operator to understand the code.

• Tool selection: First, tool 1 is selected with the command T1 selected.
• Positioning of the tool: The command G00 Z10 lifts the tool to 10 mm above the zero point of the machine. G00 the machine travels at rapid traverse, i.e. at maximum speed.
• Moving to the start position: The machine runs with G00 X10 Y10 to position X=10 Y=10.
• Switch on the spindle: With M3 S20000 the spindle is switched on and set to 20000 revolutions per minute.
• Waiting time: The command G04 H5 ensures that the machine waits 5 seconds for the spindle to reach the desired speed.
• Immerse yourself in the material: With G01 Z-2 F600 the tool plunges 2 mm deep into the material at a feed rate of 600 mm per minute. G01 is used for the milling movements.
• Rectangular machining: The next commands (G01 X110, G01 Y110, G01 X10, G01 Y10) move the tool to mill a 100×100 mm rectangle.
• Return to the starting position Z: G00 Z10 lifts the tool back to 10 mm above the zero point.
• End of programme: The command M05 switches the spindle and the command M30 ends the programme.

G-Code: Circles and arcs

Next, we extend our example with a circular milling that must be carried out before the rectangle. The extended and modified G-code lines are colour-coded in Light red highlighted. The G-code then looks like this:

; G-code file: Production of a rectangle, created on 24/10/2023
; Tool number 1 is selected
T1
; Lift the tool at rapid speed to the height Z = 10 mm above the zero point
G00 Z10
; Move to position X = 10 and Y = 10 at rapid speed
G00 X10 Y10
; Switch on the work spindle with M3 at a speed of 2000 rpm
M3 S2000
; Wait 5 seconds until the spindle speed is reached
G04 H5
; Move to the centre of the rectangle
G00 X60 Y40
; plunge 2 mm into the workpiece at a feed rate of 600 mm per minute
G01 Z-2 F600
; Circle (d=20mm, centre 60×60) clockwise
; with feed 600 mm per minute drive
G02 I60 J60 X60 Y40
; Lift tool at rapid speed : Z = 10mm above the zero point
G00 Z10
; Move to position X = 10 and Y = 10 at rapid speed
G00 X10 Y10
; plunge 2 mm into the workpiece at a feed rate of 600 mm per minute
G01 Z-2
; Traverse rectangle 100×100 mm at a feed rate of 600 mm per minute
G01 X110
G01 Y110
G01 X10
G01 Y10
; Lift tool at rapid speed : Z = 10mm above the zero point
G00 Z10
; End of programme
M5 M30

The G-code simulator (see screenshot) shows a rectangle and a circle placed in the centre of the rectangle.

Important: If the drawing is not displayed correctly, this may be due to the incorrect setting for the G02/G03 circle (arc) commands. The G02/G03 commands can be interpreted as relative or absolute. This example refers to G02/G03 in absolute form. In this case, the „G02/03 relative“ option must be deactivated in the cncGraF G-code simulator in the main menu „Settings → Options → File → G-code“.“

G-Code: Sheet command G02/G03

The G02 command is used to programme a circular or arc-shaped movement in a clockwise direction. Command G03 does the same, but in an anti-clockwise direction.

The G02 command in the G code has the following syntax:
G02 X... Y... I... J...
It says:

• ‚G02‚ for the command itself, which represents a clockwise arc. The last position of the previous G-code command is the start position of the circle or arc.
• X... and Y... indicate the end coordinates of the circle or arc.
• I... and J... indicate the distance from the current point to the centre of the arc on the X and Y axes.

G00 X60 Y40 ; This is the start position X,Y of the arc.
G02 I60 J60 X60 Y40 ; This command moves the tool in a clockwise arc.

• I60 J60: These are the coordinates of the centre of the circle relative to the current position
  X = 60 Y = 40 In this case, the centre point is at X = 60, Y = 60.
• X60 Y40: These are the end coordinates of the arc. The tool moves to the point X = 60, Y = 40.
• The diameter of the circle (d = 20 mm) is determined by the position of the tool and the coordinates of the centre point.

Table with the most important G-code commands

In this example, you have learnt the basic G-code commands: G01 and G00 for simple movements, the arc command G02, switching the spindle on and off with M03 (and M05), the ‚S‘ command for the spindle speed, the tool number command ‚T‘, G04 for waiting times, ‚F‘ for the working speed and M30 for the end of file. These commands form the basis and are already sufficient for writing your own simple G-code programmes.

Below you will find a tabular overview of all the most important G-code commands.

Command overview of the most important G-code commands

The tabular list of G commands (G code) contains only those commands that are suitable for manual programming as they are easy to use. The complete list of all G-code commands can be found in the cncGraF CNC simulator in the online help [F1 key].

Summary

G-code programming for CNC machines is not that difficult. With an understanding of only about ten basic G-code commands, you can already achieve impressive results. Learning G-code is definitely worthwhile as it allows you to better understand and utilise your CNC machines.

I hope this blog article helps you to quickly familiarise yourself with G-code programming.

4. test spindle speed

The spindle speed can now be tested. To do this, perform the test in the „Manual movement“ window, which is normally docked on the right. If this window is not visible, you can display it in the main menu by selecting „Window -> Move manually“.

In the „Move manually“ window, you will find the „Spindle speed“ button. However, first click on the „Spindle“ button to switch on the spindle and then on the „Spindle speed“ button. The dialogue window for the spindle speed then appears. In this dialogue window, you can change the speed by clicking and holding on the graphic. The spindle speed is adjusted accordingly.

Hinweis: Da das „Manuell Bewegen“-Fenster individuell anpassbar ist, könnte es sein, dass dieser Button nicht vorhanden ist. In diesem Fall müssen Sie den Button für die Spindeldrehzahl einblenden lassen. Gehen Sie dazu mit der Maus in das „Manuell Bewegen“-Fenster irgendwo zwischen die Elemente und klicken Sie die rechte Maustaste, um das Kontextmenü aufzurufen. Wählen Sie „Customize Layout“ aus. In dem Dialog „Layout Customization“ suchen Sie nach dem Button „Spindle Speed Button“ und ziehen Sie diesen per Drag-and-Drop in das „Manuell Bewegen“-Fenster ein.

5. troubleshooting

If the speed does not work, the following points should be checked:

Check the +24 volt power supply for the interface card

This can be checked with a voltmeter. All you need to do is measure the DC voltage at pins 3 and 4 (see image below). During the measurement process, the spindle speed must of course be adjusted in the software at the same time.

Hinweis: Der häufigste Fehler ist die fehlende Stromversorgung von +24 Volt.

6. use

The spindle speed setting in the cncGraF software varies depending on the file type.

For 2D file formats such as DXF or HPGL, the spindle speed is set in the „Tool storage“ dialogue. This is because DXF and HPGL files do not have the command for the spindle speed.

G-code files, on the other hand, contain an ‚S‘ command for the spindle speed. The speed is therefore taken from the G-code file. The setting for the speed in G-code files is then made in your CAD/CAM software.

Note: Preheating the spindle of the CNC machine reduces the load on its components. This means that the spindle can last longer and is less susceptible to repairs.
In this video, I show how to set up the „Spindle warm-up“ function for CNC machines in cncGraF 8.

We hope that this article has been helpful to you in handling the spindle speed. If you have any questions, please do not hesitate to contact us.

Yours sincerely, Your BOENIGK-electronics Team