Matrix Nexus - Change Max RPM mid Program?

[Isak Andersson]

Hello. How can I change the "max turning spindle rpm limit" in the middle of a program? The thing is, I need about 2500 rpm for the main spindle but the sub needs 5000 rpm. How can I achieve this in a Mazatrol program? Thanks!

 

[Scruffy887]

MAX RPM at top of program needs to be 0. Then program the speeds you need per spindle. May need to disable constant sfm. You could also change that in one of the forbidden parameters. Bad idea. For sure that will F up a Fusion control when transferring main to sub. Spindles will not sync when parting off.

 

[CNC Hacker]

i've done this by jumping to an EIA subprogram with a G92 in it.

For the main spindle:
G92 R1 S2500
M99

For the sub spindle:
G92 R2 S5000
M99

You can either make 2 subprograms or if you know macros do it all in one with some GOTO statements.

 

[Isak Andersson]

G92 R2 S5000
M99

This gives me error 807: illegal format. Any ideas?

You can either make 2 subprograms or if you know macros do it all in one with some GOTO statements.

This got me thinking. There's no way of passing arguments in a Mazatrol program, right? But, maybe it's possible to set two global variables instead? One for R and one for S. What do you think?

 

[CNC Hacker]

Oh you probably need an M902 for Head select 2 before that. You can pass arguments in a subprogram unit, once you fill in the first line it can pop in another row for A, B, C, etc. I do it frequently.

 

[Isak Andersson]

Oh you probably need an M902 for Head select 2 before that.

Some error. G92 is a threading cycle according to the manual. Could it be a G50 that it needs instead? Something simple like G50 S5000?

You can pass arguments in a subprogram unit, once you fill in the first line it can pop in another row for A, B, C, etc.

Aha. So if I wanted to pass S5000 I would simply add to ARGM 1 S 5000 and this would then be stored in variable #19? The same as using a G65, or is there something else I need to do?

 

[CNC Hacker]

Some error. G92 is a threading cycle according to the manual. Could it be a G50 that it needs instead? Something simple like G50 S5000?


Aha. So if I wanted to pass S5000 I would simply add to ARGM 1 S 5000 and this would then be stored in variable #19? The same as using a G65, or is there something else I need to do?

Ah shit you're right, I was thinking Integrex . G50 should do it.

Yes the subprogram unit can work exactly the same as a G65 in EIA.

 

[Isak Andersson]

Sorry for resurrecting this thread, but I'm still struggling with this.

I've tried doing an EIA sub-program with G50 S5000. Didn't work.
I've tried doing a Manual Program unit with G50 S5000. Didn't work.
I've tried doing a Mazatrol sub-program with a different materials shape unit. Also didn't work.

Is there really no way of changing RPM mid-program? How in the world am I supposed to do any kind of bar work if I cant change RPM? Like I'm supposed to run bars at 4000 RPM (max for main) just so I can get 5000 RPM on the sub? That would be damn near suicidal. There's gotta be a way, right?

 

[CNC Hacker]

Did you put an R2 after the G50 S5000 to select the subspindle?

Subprogram should be something like this:

M902 (HD2 SELECT)
G50 S5000 R2 (clamp speed for HD2)
M99
%

 

[Isak Andersson]

Yes, and it also did not work.

I'm starting to think changing parameters to limit main spindle rpm is the only way to do it. Maybe it's possible to change parameters directly in an EIA program through system variables. Then I could pass an S value to this sub-program and set the parameter this way. The only downside is I would need to use this sub-program in all of my programs. Not ideal.

 

[CNC Hacker]

Isak

I think I found what may have been happening. Parameter TC145 bit 5. If it's set to a 0, the maximum RPM from the common unit it output at every unit. If it's a 1, it is only output once at the beginning or during a restart. I'm guessing your machine has it set as a 0, so it's undoing the G50 in the subprogram as soon as you get back to a turning unit.

 

[Isak Andersson]

Parameter TC145 bit 5.

OMG, that was it! I didn't even need a subprogram. A manual program with a G50 S5000 simply does it.

Why that even is a parameter in the first place is completely beyond me. Anyway, I can't thank you enough. I might actually be able to run bars properly now. Now I just need to figure out how to use the bar feeder. Let me guess. More parameters.

 

[MazatrolMatrix]

OMG, that was it! I didn't even need a subprogram. A manual program with a G50 S5000 simply does it.

Why that even is a parameter in the first place is completely beyond me. Anyway, I can't thank you enough. I might actually be able to run bars properly now. Now I just need to figure out how to use the bar feeder. Let me guess. More parameters.

Haha I’ve read through the parameter manual 100s of times I think everything is always so ultra complex with Mazaks.. at least with Mazatrol.

Nice to see another Swede btw.