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gmcfadden1-Visitor
1-Visitor
December 9, 2015
Question

Surface generated by toolpath

  • December 9, 2015
  • 6 replies
  • 5391 views

Unfortunately I have a feature I simply can not figure out how to model in Creo, and I would prefer not to model it in solidworks (which can easily create this feature) and then import to creo.

The feature is a cut on a planar surface (call it X-Y plane for datuming purposes) generated by a 5/16 diameter , 0.06 radius tipped end mill moving in an arc defined from the tip center of the tool.  the arc is in the X-Z plane and the tool stays parallel to Z while traversing the arc.

I can not figure out how to create the feature correctly.  It must be correct for FEA analysis, and has been vetted by experiment to be vastly superior to our older geometry for making similar features, otherwise I would just use different geometry.

Any tutorials (I could not find any) or tips to create this geometry?


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6 replies

K
KenFarley21-Topaz II
21-Topaz II
December 9, 2015

It would be a lot easier to figure out what you are trying to do if there was an image. However, and I could be wrong, but what you are describing sounds like a simple revolved cut. If it's not a complete circle, you could do a revolved cut for the arc it sweeps, then do two cuts at the ends that are full revolutions of the tool profile. Hopefully I'm not being an idiot and misunderstanding what you're asking, but then again, it's happened before...

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gmcfadden1-VisitorAuthor
1-Visitor
December 9, 2015

unfortunately that is not the case.   No 2d profile sweep or revolved cut will create the geometry because if you take a 2d profile of the tool, it is only correct at the 2d location you draw the profile, everywhere else the surface is wrong.  Think of it as a boolean subtract between the sweep of the tool and the material.  As the tool moves up the arc in the x-z plane, it is not leaving behind a profile at any position that is the 2d cross section of the tool because the leading tip of the tool cuts into the material more than the swept 2d profile does.   I may have to snag a solidworks license, draw it, and upload the picture if necessary.

R
RonSt.Pierre12-Amethyst
12-Amethyst
December 9, 2015

assuming this is a 2 dimensional cut....

create a datum curve that depicts cut path

then drive a section the shape of your end mill using the curve as a trajectory

finish with the round

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gmcfadden1-VisitorAuthor
1-Visitor
December 9, 2015

See above.  this results in incorrect geometry.

R
RonSt.Pierre12-Amethyst
12-Amethyst
December 9, 2015

So as I understand it...

on one leg of the arc, you are generating a circular cut and as you approach the top of the arc, this becomes flat and then transitions back to being circular as you finish out the other leg of the arc?

S
23-Emerald III
StephenW23-Emerald III
23-Emerald III
December 9, 2015

Ahh, the ever allusive 3-d solid body sweep. It gets me or I get asked about it once every other year or so.

Using Solid Body Sweeps

And there are many more links discussing this under various names.

The closest I have come to it in CREO is to make the end mill as a 3d surface, then pattern it along the cutting path MANY times and then use solidify to cut out the solid.

It's not perfect and can't ever be truly smooth but may be adequate for your needs.

There is a product IDEA for this but I can't find it right off hand.

S
23-Emerald III
StephenW23-Emerald III
23-Emerald III
December 9, 2015

I'm not sure exactly what his geometry looks like but this is one I worked on. We never really got it truly correct to manufacturing.

Sweeping a ball end mill or radius end mill along a 3d path can't be duplicated precisely with Creo.

j-slot.jpg

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RonSt.Pierre12-Amethyst
12-Amethyst
December 9, 2015

The ball mill is by far easier than a flat end

This is what I'm toying with...

multi_new13.png

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gmcfadden1-VisitorAuthor
1-Visitor
December 9, 2015

Thanks.  I was afraid this was the answer.   I will probably have to go back to solidworks to build the structural model and then do the production model as an approximation with a drawing note specifying fab method (I hate doing that, and so does our inspection group).  

D
dschenken1-Visitor
1-Visitor
December 10, 2015

It can probably be done in a piecewise manner. I did a similar task with wire-frame and surface modeling ages ago. Check "Boundary of the volume swept by a free-form solid in screw motion" ftp://coffeetalk.cc.gatech.edu/pub/gvu/tech-reports/2006/06-19.pdf for hints.

S
23-Emerald III
StephenW23-Emerald III
23-Emerald III
December 10, 2015

Holy Moly David!!! Can you dumb that down to a 6th grade level?

You can definitely do it using a curve and patterning a surface of the shape of the cutter along that curve. The more pattern members, the closer you are to perfection.

If anyone attempts the pattern method, I suggest only doing it in the areas that the 3D body cut would make a difference. It will take a large pattern number to get a reasonably smooth surface.

J
JonathanHodgson13-Aquamarine
13-Aquamarine
December 10, 2015

I recently posted an example where I'd done the cutter-patterning approach for a generated gear form:

Re: Remove interference material as a result of mechansim

K
KenFarley21-Topaz II
21-Topaz II
December 10, 2015

The manufacturing module, if you run "NC Check", generates shaded imagery of what the tool does. This might be helpful if:

(1) It's capable of saving the geometry, which I think it does?

(2) The data it saves is not in some weird proprietary or special format. I fear this one has a bad answer.

(3) The resultant geometry is accurate enough, and not a crude approximation meant for "visualization only".

I'll have to take a look at this.

K
KenFarley21-Topaz II
21-Topaz II
December 10, 2015

I looked into it. It puts out a ".nck" file, which appears to be only for rendering, a "RAYREP" file? Seems to be pretty useless for what we are seeking.

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