[Alexsandr]

Hello, dear professionals.

How to add to the block the post responsible for changing the tool parameters:

$------------------------ TOOL CHANGES --------------------------------------
$70 Cancel current tool. Use [T] for current tool number if required.
N[N] M09 ''M09 = Coolant Off
$75 Code for CLOCKWISE spindle rotation - entered into variable ROT (or RT)
M03
$76 Code for COUNTER-CLOCKWISE spindle rotation - entered into variable ROT
M04
$80 Select new tool. Use [T] for new tool number, [S] for spindle speed.
N[N] T[T][OFS] [ROT] 'Select tool and offset
N[N] S[S] H[OFS] M06 'Next tool is [NT], Next XY is [NX], [NY]
$LET FIRST_RAPID = 1
$---------------------

so that the program executes this code
when changing tools

N540 Z80
N550 M5
N560 Y0
N570 M0
so that the program executes this code when changing the tool. Machine without autotool changer. It is necessary for the program to stop and the spindle to go up and go to the given coordinate for a manual tool change.
I have to insert this piece of code manually each time in a notebook when a new tool is being used.

And also switch to the coordinate system specified by the operator
G54

:0000
N10 (PROGRAM PRODUCED - 05 SEP 17)
N20 G90 G71
N30 G40 G80
It is not necessary.
Thank you


P.S
G54 I replaced myself.

[FrankCNC]

Hello, dear professionals.

How to add to the block the post responsible for changing the tool parameters:

$------------------------ TOOL CHANGES --------------------------------------
$70 Cancel current tool. Use [T] for current tool number if required.
N[N] M09 ''M09 = Coolant Off
$75 Code for CLOCKWISE spindle rotation - entered into variable ROT (or RT)
M03
$76 Code for COUNTER-CLOCKWISE spindle rotation - entered into variable ROT
M04
$80 Select new tool. Use [T] for new tool number, [S] for spindle speed.
N[N] T[T][OFS] [ROT] 'Select tool and offset
N[N] S[S] H[OFS] M06 'Next tool is [NT], Next XY is [NX], [NY]
$LET FIRST_RAPID = 1
$---------------------

so that the program executes this code
when changing tools

N540 Z80
N550 M5
N560 Y0
N570 M0
so that the program executes this code when changing the tool. Machine without autotool changer. It is necessary for the program to stop and the spindle to go up and go to the given coordinate for a manual tool change.
I have to insert this piece of code manually each time in a notebook when a new tool is being used.

And also switch to the coordinate system specified by the operator
G54

:0000
N10 (PROGRAM PRODUCED - 05 SEP 17)
N20 G90 G71
N30 G40 G80
It is not necessary.
Thank you


P.S
G54 I replaced myself.

Hi,

The easiest way is to just hard code it in the Tool Cancel $70 section of the Post overwriting the existing N[N] M09 with

N[N] G0 Z80 M9
N[N] M5
N[N] Y0
N[N] M0

or you could also set up user variables to ask the user the tool change positions
The following would go in the Tool Cancel $70 section of the Post

N[N] G0 Z[TOOLCHANGE_Z] M9
N[N] M5
N[N] Y[TOOLCHANGE_Y]
N[N] M0

and the following would go into the User Variables $1000 section of the Post

TOOLCHANGE_Z ( ) "Enter Z Axis Tool Change Position. <80>"
TOOLCHANGE_Y ( ) "Enter Y Axis Tool Change Position. <0>"

This way the first time the post encounters the variable it will ask the user for the position with 80 as the default for Z and 0 as the default for Y.

Cheers.

[Alexsandr]

Thank you so much!
I just had a long time without a computer and could not immediately answer