Converting part-files from VMC compatible to HMC compatible

[Richard Thomas - Mastercam UK]

Hi There,

I have a customer who has a number of old Mastercam part-files that were programmed way-back-when in Mastercam X7 for  a DMU 70 EVO. These parts typically contain 200+ operations and are a mixture of 2D/3D ops plus Multisurface/Curve/Morph/Swarf 5-axis.  

For some reason they have decided buy a new machine of a totally different configuration recently to continue making these parts; this machine is a Makino A500z horizontal 5-axis.  

Now there are several pain-points here!

1) These old files were created before WCS-awareness was introduced and so all 5-axis toolpaths are marked with a red cross and have to be reviewed.

2) Unsurprisingly the Makino has different rotary limits to the DMU, which can create their own issues when it comes to running toolpaths meant for a different machine.

For the 2D/3D ops, the customer seems to have got away with setting these up with a new WCS and T/CPlane via Edit Common Parameters rather than transforming the whole job to suit a horizontal machine in Mastercam (i.e. WCS Top and T/CPlane Front = B0)

Now when it comes to reviewing a 5-axis toolpath, first of all the operation has to be visually checked to see if there is a problem after switching from a VMC to an HMC, which will involve setting the new WCS and typically setting the T/CPlane to Top, relative to that WCS (assuming you can understand the context of what the original programmer was trying to mill at that point!).  If the path isn't correct then you test different solutions.  Then that operation needs to be posted and checked in Vericut, along with some previous operations so the rotary angles are correct prior to simulating the op being checked).  If Vericut doesn't like the result, you have to go back to Mastercam and rinse and repeat.  Then its on to the next operation... there could be 50+ five axis ops in one part and there are a lot of these old parts.

Anybody out there got any tips to make the transition from VMC to HMC (and from X7 to 2018) any less challenging?

[Aaron Eberhard]

<soapbox mode>

Weelllllll, if you were to define the HMC logically instead of the "default" Mastercam way, there likely won't be any conversion needed for the 5 axis toolpaths.  Now's a prime time to avoid starting a bad habit if they haven't had any previous HMC programs.

The default way of handling HMC in Mastercam is to invert the Z axis (spindle) direction in the machine def, and the post then unrotates it during processing, which is why you have to program everything in the TOP/FRONT/FRONT.

If you can't tell, I've been a long opponent of this way of programming, as to me it's completely illogical.   The Z is spindle... Don't put in an artificial rotation!  TOP/TOP/TOP should be the same on a VMC as an HMC!

If you set up your machine just like a VMC, then you can post just like a VMC to ANY machine!

</soapbox mode>

Other than that, unfortunately, there's no quick way to edit the multiaxis toolpaths.   Because the change meant than any reference to axis has been updated, you can have situations where you have to change from X to Z in Tool Axis Control, Collision Control, Cut Pattern, etc.   And, because we were completely WCS un-aware prior to that, I was never able to figure out a fool-proof conversion so it didn't seem worth the risk to try to make global edits when we might not guess correctly.

[JParis]

5 minutes ago, Aaron Eberhard - CNC Software said:

If you can't tell, I've been a long opponent of this way of programming, as to me it's completely illogical.   The Z is spindle... Don't put in an artificial rotation!  TOP/TOP/TOP should be the same on a VMC as an HMC! 

Hell, I've been hearing for more than a dozen years that something was in the works to make HMC programming easier, more intelligent....it's a good thing I haven't been holding my breath. 

But to the OP question...

You're in a situation not unlike using MT and wanting to move a job for one machine to a completely different machine...you can't just change the machine and go...just doesn't work that way...

So there really isn't a painless way to do what the customer needs.....they just have to go through the process

[Richard Thomas - Mastercam UK]

1 hour ago, Aaron Eberhard - CNC Software said:

Don't put in an artificial rotation!  TOP/TOP/TOP should be the same on a VMC as an HMC!

It's a shame that what became "best practice" in Mastercam wasn't perhaps the best choice... as you know a lot of (but not all!) HMC posts expect the Top/Front approach and don't work properly otherwise, because of this weight of history

At least I can be satisfied that I'm not missing a trick with the particular situation the customer find themselves in.

 

Cheers for your responses 

[Newbeeee™]

1 hour ago, Aaron Eberhard - CNC Software said:

If you can't tell, I've been a long opponent of this way of programming, as to me it's completely illogical.   The Z is spindle... Don't put in an artificial rotation!  TOP/TOP/TOP should be the same on a VMC as an HMC! 

If you set up your machine just like a VMC, then you can post just like a VMC to ANY machine!

 

+1

My *feeling* is that it was changed because the hori boys then had automagic planes set-up that would output correctly (0,90,180,270)

Doesn't make it right though...

Rich - Phil helped me convert my VMC 4th axis post to a Hori and we did exactly as Aaron said - TOP/TOP/TOP. As your customer has this new machine, perhaps they should go this way too from the start?

 

[Richard Thomas - Mastercam UK]

10 minutes ago, Newbeeee™ said:

+1

My *feeling* is that it was changed because the hori boys then had automagic planes set-up that would output correctly (0,90,180,270)

Doesn't make it right though...

Rich - Phil helped me convert my VMC 4th axis post to a Hori and we did exactly as Aaron said - TOP/TOP/TOP. As your customer has this new machine, perhaps they should go this way too from the start?

 

Hi Terry,

The post is from an outside supplier that I'm not even familiar with.  Its a suggestion I will make to our customer but as to whether their post people can/will do it is another matter....

[nickbe10]

6 hours ago, Rich Thomas 4D Engineering said:

Anybody out there got any tips to make the transition from VMC to HMC (and from X7 to 2018) any less challenging?

TOP/TOP all he way.

Worked in several shops where we would prove out on VMCs and then move to a production Horizontal.

MC looks like the machine axis which certainly helps me keep oriented.

In aerospace non right angle rotations are so common that having "pre defined" views is of little benefit.

[nickbe10]

2 hours ago, Rich Thomas 4D Engineering said:

The post is from an outside supplier that I'm not even familiar with.  Its a suggestion I will make to our customer but as to whether their post people can/will do it is another matter....

Don't think you need them to actually edit code in the post .

You will have to change a few switches (for things like axis rotation address output), but a lot of it is handled in the MD/CD. 

Is the post binned?

[JParis]

I can understand the drive for Top/Top if you make 1 part....

We do our prototype and low qty production on our VMC's.....typically, one at a time, thru multiple vises....parts can take 11 different setups

When a part graduates to our high-production HMC's, I can have anywhere between 12 & 100 parts on a single tombstone....on top of that I RARELY use any code from our VMC programs...as prototype, they are simply programmed to make the part. Cycle time while paid attention to, is not the driving factor. Couple that with being able to tilt at different angle to make features easier to cut.....you don't do that on a 3ax VMC without multiple setups....100,000 parts for a total part lifecycle is not uncommon.

So how you approach your programming and setup can be very different based on a companies work.

I could live in a Top/Top world but if they pushed that change, I would have reteach myself many years of programming HMC's...wit all the other changes and things getting broken, I am already tempted to look at something else....

 

:I'll get off my soapbox now:

[Richard Thomas - Mastercam UK]

22 hours ago, nickbe10 said:

Don't think you need them to actually edit code in the post .

You will have to change a few switches (for things like axis rotation address output), but a lot of it is handled in the MD/CD. 

Is the post binned?

I'm not sure if the post is binned to be honest, I never took a look while I was on site.  It might be something I can experiment with if I'm allowed a copy of the post.

[Aaron Eberhard]

Yeah, I believe newer-style posts should be looking at the Machine Def to get their layout.  If you check the spindle and the Z axis, they should be both align to the Z, not X or Y.    Older posts often have an unbinned section that allows you to put what type of machine it is and toggle it... But I don't deal in those black arts much

[nickbe10]

23 hours ago, Old_Bear said:

:I'll get off my soapbox now:

Absolutely not, we all bring different experience and work packages. I for instance spend most of my time in Aeospace job shops where we could never get that many parts on our tombstones, so this is definitely a horses for courses situation.

The more potential solutions we can give to Rich, the more likely he is to get the right solution, it might even be a combo...

[pete_hull]

Someone at cnc software thought they could one-up Rene Descartes, the genius that came up with the original, insanely elegant system for defining  coordinate systems. I feel that Mastercam's insistence on Top/Front etc.  was a sorely misguided 'new coca-cola' moment.