[mbbert]

When calling the RAPID TO TOOLCHANGE command, I want to have the code output two different options depending on whether or not it is the same tool coming back in, or a new tool.
If the next tool is different from the current tool, I need the machine to travel to the G28 home position to update the offsets.
However, in many cases we use this command to move the tool away from the part and stop the program for an insert change or to measure the part.
In these cases, the same tool is coming back in again and we do not want to move all the way to the home position.
The code below shows the additional logic (in red) that I think will handle this, but unfortunately I do not know the correct Edgecam syntax.
Can anyone tell me what the Code Wizard format should be.




;CODE: @ZFIRST
[DELETE][BLKNUM][RAPIDGCODE][ZMOVE][<C>COOLANT OFF]
[DELETE][BLKNUM][RAPIDGCODE][XMOVE]
IF NEXTTOOL = current tool %GOTO @END
;CODE: %GOTO @ALWAYS

;CODE: @DEFAULT
[DELETE][BLKNUM][RAPIDGCODE][XMOVE][ZMOVE][<C>COOLANT OFF]
IF NEXTTOOL = current tool %GOTO @END
;CODE: %GOTO @ALWAYS

;CODE: @ALWAYS
[DELETE][BLKNUM] M5
[DELETE][BLKNUM] G28 U0 W0
[DELETE][BLKNUM] M0

;CODE: @END

[tummen]

Some tips that might help you:

in the directory C:\Program Files (x86)\Planit\Edgecam 2011 R1\Language you can find cgcomp.chm. it´s the help file for the compiler and contains syntax for many things.

after you compile your post you will get an intermediate .mxt file in
C:\Users\%username%\Documents\Planit\2011.10\Edgec am\cam\Machdef

this contains all the output from code wizzard.
don´t edit this file, but steal syntax and read about why things happend.

%LOAD SUBFUNCT
loads info about tools (i did not do any full scale testing of this)

I´m not sure that your approach is the best anyway. Move to toolchange will probably always give you next tool although you are not about to change tools yet.
try outputing nexttool as a comment and se if it is unchanged when you just use this as a "move away"

Another way of getting what you want is to declare your own M function

Give it a good name (it will pop up in the sequence tree) and then add different options, give it a fake M number that is not common to other functions

then under construct you can put your own code with if statments to check what options you used and output different codes including a comment with instruction like "change inserts" " meassure" and so on. i think this approach would give your programs better documentation at the same time.

[tummen]

;CODE: %IF $MCODE=100 %THEN
[DELETE][BLKNUM] L M0 ; Change something
;CODE: %ELSEIF $MCODE=101 %THEN
[DELETE][BLKNUM] L M0 ; Measure something
;CODE: %ELSE
[DELETE][BLKNUM] ; Totaly unexpected to end up here
;CODE: %ENDIF

Added to options 100 and 101
You can then later add an instruction under m_Functions -> mashine m-Functions

if you name your macro: "ProgramHalt"
and your options 101 named "Meassure"
then you would see in the sequence tree a row with
ProgramHalt : Meassure

[meegers]

Bert,

Use the following two variables in the 'rapid after' code con.

Position will output the current tool number, and #nexttool will output the next tool number. Only #nexttool has the #prefix.

Cheers

[meegers]

Forgot to add the line of ;code ....

;CODE: %IF #NEXTTOOL=POSITION @END

Cheers

[mbbert]

Thanks everyone who offered solutions. I went with meegers suggestion as, being limited in my Code Wizard knowledge, it appeared to be the simplest.
It works exactly as I hoped it would -only change was that I put the suggested code in the 'RAPID TO TOOLCHANGE' code constructor, not the 'RAPID AFTER' as suggested.

[meegers]

Glad to be of help.

Apologies for getting the code constructors mixed up, 'rapid from' instead of 'rapid to', but at least the same variables work.

[crazycnc]

The cgcomp help file is interesting, but kinda hard to understand by itself. Does anybody know of any resources or tutorials to learn the language? I have some Basic, some C++ experience, so I should be able to learn this if I had the resources.