Profile milling, avoiding retract

[raviles]

I've been fighting Creo2 (and WF4 previously), trying to avoid or suppress retracting while in a profile milling sequence. I have the retract plane defined 50mm above the fixture and part, but I have a wide open space where the tool could simply move from the end of one cut to the start of the next with no interference. Creo insists on retracting which is a waste of time and causes unnecessary wear and tear of the machine.

One friend suggested placing the retract plane at the bottom of the feature but that doesn't work either. At this point, I'm simply editing out the offending code in the NC program, but this is a major PITA.

Any help would be greatly appreciated,

Thanks,

Ray Aviles

Manufacturing Engineer 2

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[razmosis]

Do you have the parameter APPR_EXIT_HEIGHT set for DEPTH OF CUT, rather than RETRACT PLANE?

[raviles]

Matt,

Thanks for the reply but unfortunately, it didn't help. APPR_EXIT_HEIGHT was already set to DEPTH OF CUT. I tried setting it to RETRACT PLANE but that made no difference either.

I'll keep plugging away at it.

Ray Aviles

Manufacturing Engineer 2

[SteveLucas]

Ray,

If you change the CUT_TYPE from climb to zig zag it stays in the cut better. I do that for roughing with profile.

Steve

[raviles]

Steve,

I've tried that except that I can do without conventional milling. I'm working with cast steel; I think "JUNK-ALLOY" is the correct brand Anyway, it's loaded with all the goodies that are typically associated with castings, like sand, old taps, chunks-o-carbide...

Seriously, I have enough trouble with the low level of tool life in this material that conventional milling is prohibitive.

Thanks for the suggestion, I appreciate it.

Ray Aviles

Manufacturing Engineer 2

[SteveLucas]

Ray,

I guess I would need to see the part to make anymore suggestions. Profile milling isn't always my first choice for profiling parts. There are some better routines for profiling that stay in the cut but with out at least seing a picture of the part I can't help.

Steve

[raviles]

Steve,

Here's a picture of the retract problem. It may not look too bad, but the machine tool is a MAG Cincinnati U5 with a work envelope of 6705.6 X 3352.8 X 1500.0 mm, many spindle attachments, etc.

Although the control is configured to deal with the acc & dec, mass, all those physics goodies, it helps to avoid unnecesary movement.

As for volume milling, I try to avoid it like the plague. Most of my milling sequences are either profile or custom trajectory and even the occasional face milling type.

Ray Aviles

Manufacturing Engineer 2

[SteveLucas]

Ray,

Seing you said it is a casting I assume the walls are drafted or are you trying to cut the taper on the edge of the part? Kind of hard to see but it looks like a big part. with the opening in the part. I can see why it wants to retract and rapid back to the next cut.

What I might do in a case like this is do a surface copy of the surfaces to cut then add a surface to fill the gap where the tool is retracting and just let it cut all around with a profile of the surfaces or a helical cut line motion. It's a little work but not bad.

Steve

[raviles]

Steve,

That's an interesting concept; I'd never thought of that. However, that gap in the surfaces is about 16" long, which is long way to feed.

I'll have to give volume milling another try, using what both you and Matt have suggested.

Thanks,

Ray Aviles

Manufacturing Engineer 2

[razmosis]

My other thought would be the use of volume milling instead of profile milling, profile only, with optimized retract and retract set to depth of cut. One or the other works most of the time for me, but there are still a lot of times that I can't shake the retracts either.

Matt

[mthompson]

Ray,

Have you tried a cutline milling seq using a mill surface?

When I have a part with a gap thats what I mostly use.

[raviles]

Mike,

No I haven't, but I'll try that tonight. I may back on-line begging for help because this will be a first for me.

Thanks,

Ray Aviles

Manufacturing Engineer 2

[gkoch]

Hi Ramon,

would you share your experience with the suggestions made by Steve, Matt and Mike?

I am sure we are all interested in hearing from you.

Thanks,

Gunter

[SteveLucas]

Gunter,

What would be nice is if they(PTC) included in profile milling a Simultaneous to move between cuts like they have in trajectory milling. The situation that ray has is a common one where the retracts are a pain to deal with and there is no easy fix.

Steve

[raviles]

Gunter,

I had no luck with the cut-line milling solution. I was able to create the milling sequence after major headaches trying to figure out exactly what a cut line was. Painful, but I stumbled my way through until I finally saw some output. But the output was completely useless. I tried many combinations of parameters to no avail.

I expected to see 8 planar cuts (2D moves only) around the profile. What I got was all kinds of 3-axis milling with very strange jumps and that made my jaw drop.

Anyway, I would agree with Steve that a "simultaneous" connection type be added to the profile milling code.

Lastly, I would have included some of these parameters, but there does not seem to be an easy way to export them from within the parameter page. I understand that uploading a manufacturing model could very helpful, but my company's IP policy prohibits this.

Any further ideas regarding this problems would be greatly appreaciated.

Thank you,

Ray Aviles

Manufacturing Engineer 2

[mthompson]

using cutline milling with a helical scan type

[gkoch]

Ramon,

what I understand, the toolpath that would be created by Steve's suggestion (filling the gap with a surface path), is basically what you want, only you need rapid feed when the tool moves in the air, right?

That said, I assume Mike's suggestion is not what you are looking for, as the tool still evades the gap?

Did you also try Matt's suggestion with Volume Milling?

Gunter

[raviles]

Gunter,

I agree, Steve's suggestion is exactly what I need, planar profile cuts, rapid across gap without retract. Mike's toolpath machines the entire profile so it's not quite what I need.

I tried volume milling but had major difficulty creating the mill volume. Once that was done, tried many combinations of parameters but saw no useable toolpath.

Dumb question: Is there a way to create mill surfaces with styles? I created a sweep mill surface, no problemo. I then used COS by intersect to create curves on the surface with a plane, then trimmed the surface so that it can be milled with planar cuts.

But the resulting style is not a mill surface, at least according to the model tree. Profile milling ignores it. So, I created mill surface with boundary blend from the style. The profile module likes it and does its thing.

Obviously, I have very little experience with surfaces and volumes. I still haven't figured out what a mill window is...

Custom Trajectory has been my "Go To" milling module, at least until I discovered profile milling when I encountered my problem casting, which was a first for me. As I said previously, I try to avoid volume milling like the plague; I've not had much luck with it.

FYI, I've taking the manufacturing module training three different times; once with V19, once with 2000i2, and the last with WF2. If I remember correctly, one of the training workpieces was a cell phone, which is completely different that the weldments that I typically machine. Needless to say, I left the instructors scratching their heads as to how to machine some features in our parts (I provided models as the training took place at our facility).

Ah well, I will keep plugging away.

Thanks,

Ray Aviles

Manufacturing Engineer 2

[gkoch]

Designing surfaces is surely an art for itself and often useful when it comes to set up not so simple manufacturing sequences.

But maybe I can help about mill windows:

They are basically equivalent to a mill volume, created by an extrude and bounded by the design part below.

Instead of having you create an extrude with the sketched outline, then trim it with the design part, the mill window is doing this internally and you only have to do the sketching.

So no magic, just a little helpful automation!