HMC programming training?

[Sticky]

Does anyone here know where I could get some training on using MC to program hmc's with multiple parts, planes, workoffsets and in process probing?

 

I'd consider traveling for in classroom training. But text would be preferable. The In House Indexing manual doesn't go anywhere near this level of detail, and so far non of the In House tech guys I have talked to have done anything beyond that. I am wasting about 10 hours a week in programming, trying to get stuff to work either by myself or with In House support and I am getting frustrated.

[Guest]

Have you tried your Machine Tool Dealer? We have offered these in the past and do them on an as requested basis.

[Sticky]

Have you tried your Machine Tool Dealer? We have offered these in the past and do them on an as requested basis.

 

Matsuura Canada and Japan push Gibbs, Matsuura UK pushes Featurecam.

 

Unfortunately all the local machine tool dealers are really small and we don't really have local apps guys.

[Colin Gilchrist]

I'm sure if there was sufficient interest, we could put together a training class through Eapprentice.net.

 

Would anyone else besides Sticky be interested in an online course for HMC's, using multiple parts, work offsets, planes, and probing?

[CADCAM3D5AXIS]

Colin That would be a Good Series to do

[cincy k]

Yes yes!

[?Mark]

It's just like a vertical only with the added "B" rotation

[Sticky]

It's just like a vertical only with the added "B" rotation

 

By G code, yes, by Mastercam... I wish.

 

I think it would be awesome if you guys did a course for this, as I can't find any other training for it. Would you guys modify each users post processor then? Stock Mpmaster lacks some functionality that would be necessary.

[Colin Gilchrist]

We could certainly cover any necessary post modifications during the Office Hours sessions. That is what the Q&A portion of the class is designed for.

 

What post functionality do you find lacking?

[DUANEP]

yes I would that as well

[?Mark]

Hi Colin, you're not with cnc anymore? Just noticed your signature

[Colin Gilchrist]

Hi Colin, you're not with cnc anymore? Just noticed your signature

 

Hi Mark,

 

That is correct, I'm now focusing on doing training full time.

 

Best regards,

 

Colin

[Newbeeee™]

Hi Mark,

 

That is correct, I'm now focusing on doing training full time.

 

Best regards,

 

Colin

All the very best with this Colin.

 

[Sticky]

We could certainly cover any necessary post modifications during the Office Hours sessions. That is what the Q&A portion of the class is designed for.

 

What post functionality do you find lacking?

 

G10 output for WCS's based off COR

Extended workoffsets

A method of being able to transform rotate a transform translate op with extended offsets

Productivity plus integration

 

Those are just some of the things that someone who would want to take this course is going to need help having integrated into their post. Sounds like you won't have any problem doing that, but I thought it was worth mentioning because other people will have some or all of those needs.

[Joe788]

This seems like a good place to mention a potentially spindle destroying disaster that I narrowly avoided a week ago, after translating/rotating safely for many years. I was surprised this is the first time this ever happened to me:

 

I use the MPMaster post, and it retracts to Z home before every B axis move.

 

BUT - if you have consecutive transform/rotate toolpaths with the same tool, and the first B axis orientation of the second path, is the same as the final B axis orientation of the previous path, it will just change work coordinates and move straight through the tombstone in XYZ. Since there's no index call, there's no go-home call.

 

I figured this out 7 hours into the prove out of an 8 hour long program, on about the 35th tool. I got extremely lucky, because the tool went from working on the left side of the tombstone, to working on the front of the tombstone - and cleared the part by about .100.

 

The very next tool had two instances that would have gone straight through the tombstone. (Then I sent Bob a PM, asking him how much he paid for Vericut LOL)

 

You can program around this disaster by paying close attention to how you order your toolpaths that use the same tool, but it's one more thing to worry about.

[Sticky]

Strange one Joe. I'm quite sure I have done that and I haven't seen that problem. In your transform rotate, is your source geometry or NCI? Do you have two different tool planes for this tool then? And do they have their own work offsets tied to them?

[Sticky]

I also had a new to me problem two days ago on a tombstone. I found out that if you have a tool path with only one entity on a plane it ignores the linking parameters "clearance" value, but only on retract, it still uses it on the way in for G43 Needless to say it almost caused a spindle through tombstone situation, luckily I've been on edge with my MC post lately. There had already been a few tools that went to these planes without issues, but because they had more then one entity on that plane they used the clearance value on the way in and OUT.

[?Mark]

Full retract on rotation is your best friend. Unless you have high volume production, I don't see a reason not to use it. We went a little different way and setup our posts to ask for minimum/safe clearance retract. Pretty foolproof, unless someone slaps some additional vises or fixtures on the tombstone and I'm not aware of it

[Colin Gilchrist]

I also had a new to me problem two days ago on a tombstone. I found out that if you have a tool path with only one entity on a plane it ignores the linking parameters "clearance" value, but only on retract, it still uses it on the way in for G43 Needless to say it almost caused a spindle through tombstone situation, luckily I've been on edge with my MC post lately. There had already been a few tools that went to these planes without issues, but because they had more then one entity on that plane they used the clearance value on the way in and OUT.

 

Did you report that to QC as a bug? If not, you should. The move needs to be in the NCI file for the post to output the move. You can work around that by doing some work in the post, but you really shouldn't have too.

[neurosis]

I also had a new to me problem two days ago on a tombstone. I found out that if you have a tool path with only one entity on a plane it ignores the linking parameters "clearance" value, but only on retract, it still uses it on the way in for G43 Needless to say it almost caused a spindle through tombstone situation, luckily I've been on edge with my MC post lately. There had already been a few tools that went to these planes without issues, but because they had more then one entity on that plane they used the clearance value on the way in and OUT.

 

 

I had this exact same thing happen some time ago. I had to make some post changes to fix it. I cant remember what I did it was so long ago but I do know that it is not an issue anymore.

 

My specific problem happened when drilling but ONLY if you were drilling a single hole. If you were drilling two or more holes it worked as expected. I never tried it with any other type of operation (single) to test so it could very well still show itself some day.

 

This issue almost caused a huge crash for us on a very expensive part. Luckily the operator was already wound up so tight that he could have cracked a walnut with his a$$ cheeks so he was lightening fast on the E-Stop.

[Josh Kinney -Elite Engineering]

ALWAYS force z home on index. That is a standard for all my posts including 5 axis. I'll settle for a slower cycle time knowing it won't index the tombstone into the spindle....

[Joe788]

Yeah we always force home on index as well. This problem happens when a final instance of a transform/rotate operation is at the same B axis orientation as the first instance of the next transform rotate operation.

 

If you have an operation on the B90 side of the part, followed by the B0 side of the part, it runs perfectly fine, because it goes home between operations. When you Transform/Rotate those toolpaths to the other 3 sides of the tombstone, the B90 operation goes:

 

B90

B180

B270

B0

 

When it's done, it moves on to the next toolpath.....since that ones starts at B0, there's no index, which means there's no Z home. Bad juju.

[MIL-TFP-41]

Joe, can you throw up a quick sample? I would like to test that w/ our post.

 

 

Sent from my iPhone using Tapatalk

[Guest]

I remember having that issue a LONG time ago. To avert it, I just made sure I had a plane change in between transform ops. Came awful close to shearing off a holder at the diameter behind the flange. I think I was about .100-ish form the crash.

 

#SoiledUnderwear

[Sticky]

Full retract on rotation is your best friend. Unless you have high volume production, I don't see a reason not to use it. We went a little different way and setup our posts to ask for minimum/safe clearance retract. Pretty foolproof, unless someone slaps some additional vises or fixtures on the tombstone and I'm not aware of it

 

ALWAYS force z home on index. That is a standard for all my posts including 5 axis. I'll settle for a slower cycle time knowing it won't index the tombstone into the spindle....

 

My post IS set for full retract on index for the reasons you mentioned! The issue is that I was on the LEFT side of the tombstone, MC ignored the "clearance" value and almost sent my spindle into the tombstone/parts sitting on B0. Luckily I was watching the code like a hawk, and I saw it coming before it happened. What makes this particularly dangerous is that I had a few other tools going to the same plane, and because they had more then two entities, they used the "clearance" value, just like they SHOULD. If I had been the slightest bit complacent in thinking "MC/post is working as it should as shown by the previous tools" I'd be out over 50k right now.

 

I had this exact same thing happen some time ago. I had to make some post changes to fix it. I cant remember what I did it was so long ago but I do know that it is not an issue anymore.

 

My specific problem happened when drilling but ONLY if you were drilling a single hole. If you were drilling two or more holes it worked as expected. I never tried it with any other type of operation (single) to test so it could very well still show itself some day.

 

This issue almost caused a huge crash for us on a very expensive part. Luckily the operator was already wound up so tight that he could have cracked a walnut with his a$$ cheeks so he was lightening fast on the E-Stop.

 

Glad to know I'm not the only one... Yikes.

 

Did you report that to QC as a bug? If not, you should. The move needs to be in the NCI file for the post to output the move. You can work around that by doing some work in the post, but you really shouldn't have too.

 

I sent it to In House. Is there someone else I can send it to? In house doesn't give me bug #'s.

 

 

Joe, I can replicate your problem with my MPMASTER post.