[tummen]

Im using Heidenhain TNC in my mashine and to change the S parameter i need to output:
123 TOOL CALL 1 Z S2000
at the normal toolchange
or later a
456 TOOL CALL S3000
line when the speed changes.
my problem is that if i change the speed between different instructions but still using the same tool I don´t get a new tool call
I think in ISO you just add Sxxxx on a normal line and you are done.
I guess there are two solutions.
one is to force a toolchange at every speed change
and one is to check if speed is not = old speed and then output my new speed value.
Does anyone have a solution or atleast a hint to offer?

[jsanders]

You're 2nd idea is the way to go, a check on logic to see if the speed is changed. Keep in mind that "negative logic" works best here. The layout is below. Refer to the Code Wizard help or *.MXT source code for the variable names and syntax. You may also need to create a variable to hold the old speed value.

%If NEWSPEED = OLDSPEED @NO_SPEED_CHANGE
CNC code output "456 TOOL CALL S3000" goes here
@NO_SPEED_CHANGE

[tummen]

All values that are used in code wizzard has a flag if they should be skipped if they did not change. there must be some value behind every value that it checks against.
Anyone seen how to reach for this old value?
i can in this case save the old speed for later but since edgecam can deside in every output if it is needed (modal) then maybe i could do the same?

[jsanders]

Save the old speed. That is the only way you have to determine if the value is changed.

[tummen]

After reading the intermediate file from compiling of the post i found that almost all vars have a xxxHOLD that holds xxx´s old value
the code below was therefore my attempt.

;CODE:%IF #SPEED=#SPEEDHOLD @SKIP1
[DELETE][BLKNUM] TOOL CALL S[<C>SPEED]
;CODE:@SKIP1

but i did not need it in the end i found a reference to another variable that i then traced to misc funktions, outpuut speed change on separat row.
this solved my problem.