X4 mpmaster post and first_tool$ value

[Tom Anderson]

I've used the X4 Mpmaster.pst as the base for a custom post. I'm trying to get the first tool call at the end of the file, but this machine does not support staging tools.

 

So, I have:

> Control Def. "enable stage tool routines" = off

> this line in peof = pbld, n$, first_tool$, protretinc, e$

 

I get NO first tool output. If I force first tool(*first_tool$) I get T0 . If I turn on tool staging in the control def, I get T# output at every tool change, which I can’t have.

 

Am I crazy(ok don't answer that), missing something here, or does mpmaster not track first_tool$ if tool staging is off?

 

Thanks,

[Colin Gilchrist]

Hi Tom,

 

When you force the "first_tool$" variable, you are getting T0, because the value of the first tool variable is "0" at that point in the posting process.

 

You should setup a custom variable to hold the value of "first_tool$" in the 'psof' section of the post.

 

Something like:

 

myfirsttool = first_tool$

 

You'll have to initialize the variable and setup a format assignment string as well.

 

This custom variable will hold the first tool's number as there is no other mechanism in the post to reset it's value.

 

HTH,

[Colin Gilchrist]

One more crazy question that I have to ask. Did you check to make sure that your program does in fact use multiple tools that aren't T0?

[Guest CNC Apps Guy 1]

Normally when I have a machine that does not support staged tools, I still turn on Stage Tools, but then I remove the next_tool$ calls, then at the end of the program I put in first_tool$, "M6", e$ and it does what I need.

 

HTH

[Colin Gilchrist]

That is actually a better idea James...

[Guest CNC Apps Guy 1]

Oooops. Forgot, you'll need to force the next_tool$ with * at the end.

[Tom Anderson]

Thanks guys. I finally got the output, using James' suggestion was easiest way.

 

In the process I did some more searching/testing and found this. Since it is different then pre-X versions it had me confused. Thought I'd pass it along for others.

 

The "enable staged tool routines" checkbox in the CDef = bldnxtool$ used in pre-X posts. So, if bldnxtool$ = 0, first_tool$ & next_tool$ is not assigned a value. Then, when bldnxtool$ = 0,forcing *first_tool$ produces the T0.

 

It's just onther one of those things that was moved from the .pst to the MDef/CDef, but not named the same, so ya have figure what it is.

 

Recommended reference McamX4 NCI Parameter Ref.pdf !!!

[Guest CNC Apps Guy 1]

quote:

---

...It's just onther one of those things that was moved from the .pst to the MDef/CDef, but not named the same, so ya have figure what it is.

---

Oh joy... I just love those. 8-/

 

Always glad to help.

[Tom Anderson]

Oh, and yes Colin, I did have more than one tool in my program. But, I have made that mistake before . . . . more than once! Programmer error not post error.

[john316]

.

 

quote:

---

I finally got the output, using James' suggestion was easiest way.

---

That's the way I have mine set up also. I put a forced M0 at the beginning of the program with a note alerting the operator what tool should be in the spindle because on the Fanuc controllers the tool changer goes wacko if you have an M6 with the same tool that's in the spindle.

 

.

[Colin Gilchrist]

Glad you got it solved Tom. I can't tell you how many times I've made Post edits and forgot to save the PST file. Then you sit there forever trying to figure out why the code hasn't changed...

[Guest CNC Apps Guy 1]

john316, on some machines the M6 error if the same tool is in the spindle is a Keep Relay setting (On older Mori Seiki machines), or Data Bits. You shoudl be able to change that behaviour.

 

HTH