---

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

Example
G00 Z0 G98 G82 X10 Y10 Z-3 F300 P100

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.

Example
G98 G82 X20 Y20 Z-3 F300 P100 ; Repeat drilling cycle at three points X30 Y20 X40 Y20 X50 Y20 ; Delete drilling cycle G80

---

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

Example
G00 Z0 G98 G83 X10 Y10 Z-9 F300 P100 Q3

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).

WRONG	CORRECT
$IF R200==0 ; G-Code: Contents $IF R1==1 ; G-Code: Contents $ENDIF ; G-Code: Contents $ENDIF	$IF R200==0 ; G-Code: Contents $ENDIF $IF R1==1 ; G-Code: Contents $ENDIF

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