Can not determine source of alarm on VMC

[Chris91]

We've been going round and round with CNC Software and Haas's application department. Once we got in touch with the right people they have been very helpful, we just don't have a solution yet. So, while we are still working that angle we figured we'd post the issue here.

 

We have 3 Haas VMC, super mill, VF1 & VF2SS. We have been getting alarm 304, "Invalid I, J or K in G02 or G03 radius at start must match radius at end of arc within 0.001 inches". We get the alarm on all 3 machines but it is more frequent on the VF1 (oldest machine). The programs we are running are for molds so it is all 3D machining and the programs are one and done. The run time on the programs can be anywhere from 4 hours to 40 hours, just depends upon the complexity of the geometry. We do not believe that it is an issue with our programs because after the alarm is thrown we can delete the section of the program that has already run and typically finish the program with out issue. On some of the longer programs we need to do this 2-3 times. Haas applications seemed to think it was some type of rounding/tolerance issue. CNC Software was able to recreate the alarm with our program and has been trying to make some adjustments to our post file.

 

Does anyone else having any insight as to what might be going on? Is there some type of tolerance/rounding setting that we are not aware of that would accumulate until it reached the allowable limit on the machines?

 

Thanks for your help,

 

Tim

[gcode]

On the tolerance page of your Control Def.... change the NC Precision (step value) to .00001

 

I have had this problem in the past with older controls and this solved it.

[Chris91]

On the tolerance page of your Control Def.... change the NC Precision (step value) to .00001

 

I have had this problem in the past with older controls and this solved it.

 

 

 

Thanks for the input. We tried what you suggested and it did not work. Any other input would be greatly appreciated.

[Mr. Wizzard]

can you post the line(s) of code that cause the problem, details of what toolpath(s), and filtering used/not used? Might give some more insight.

[Oscar R.]

I have had this problem in the past with older controls and this solved it.

 

+1 on that. I've had the same thing happen with molds running on haas. It's been a while but I seem to recall having to open up my tolarence on these types of programs.

I would play around a bit with the filter and total tolarence setting a bit.

 

We do not believe that it is an issue with our programs because after the alarm is thrown we can delete the section of the program that has already run and typically finish the program with out issue. On some of the longer programs we need to do this 2-3 times.

 

I'm reaching here, but if you're able to delete the code that's already been run at continue with no issues, I'd look into your look ahead limits or lag in DNC if you're using that.

[Hardmill]

Ive actually had this problem on a fanuc control.

And the fix was loosing up the arc tol in the machine control.

 

I think it was set at 2microns and we ended up bumping it to 10 microns. Solved the problem.

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

PEACE

[Chris91]

Our tolerances are in the attached file. The lines of code are in the other file. This problem, it seems, has got worse with every newer version of Mastercam. I don't know if something was mastakenly changed in the machine definition or somewhere else. It's driving us crazy. We have lost at least 6 to 8 days of work because of this problem.

 

 

 

Thanks for the replies

 

TOLERANCES.pdf

CODE.pdf

[JNMFD]

It looks like it's not going back to the G17 plane. Try adding a G17 before the line that alarms and see if that helps....John

[Mr. Wizzard]

I don't know if this will help, but here's my settings for my TM-2. I've used the MPMaster as a base for TM-1, TM-2, VF-2SS, EC-400, EC-300 and never had that alarm. If these settings work for you, give them a try. If not, it may be something in the post.

[Mr. Wizzard]

Before that, try changing your arc settings. I just drew the arc your machine is stuttering on, it's a few thou from 360 degrees. Try arc settings before changing your tol's, or maybe a combination.

[gcode]

It looks like it's not going back to the G17 plane. Try adding a G17 before the line that alarms and see if that helps....John

 

 

^^^^^^ +1 ^^^^^^^

 

 

 

the previous tool is doing arcs is in the XZ plane

and there is no G17 before you do an arc in the XY plane..

adding a G17 should fix this block of code.. but the post needs to be fixed so

the G17, G18 AND G19 are posted when required

[MotorCityMinion]

I'm with Wizzard on this one. MPMaster for the post on our Haases. Only exception here was I never tweaked the precision settings at all. Arc values for arc output in the filter must be set at 500. max on the older machines. 1000 works fine on the new ones.

[Redfire427]

It is definitely the G17 issue. Clearly the previous tool was making arcs in another plane and then you changed tools and are trying to do arcs in the XY plane, but your machine thinks it is still in the XZ plane.

 

Carmen