Pro E Users?

[Ocean Lacky™]

I'm working with a customer, trying to get a decent model into Mastercam using parasolids. Currently, I'm getting solids with many faces missing

 

What parasolid version is best? I think I recall JParis reccommending stepping back to V16 or so, but that may have been for Solidworks?

 

Where in ProE would you look to see what export version?

 

IGES files generally yield poorly trimmed surfaces, STP works but take forever to load in MC....

[Pete Rimkus from CNC Software Inc.]

In my experience Parasolid is not the first choice to get from Pro/E --> Mastercam. This is based upon the "Pro/E-exported" Parasolid files that have been sent to us to investigate problems in.

I think you'll like the STEP results better.

 

Of course, the best way to get Pro/E --> Mastercam is via Mastercam's Pro/E reader addon. Does that sound like a sales pitch coming from a CNC employee? Just trying to help...

[Thee Rickster ™]

quote:

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Does that sound like a sales pitch coming from a CNC employee?

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Sounds like it should be free in X5...

[peon]

Pete is correct. I step out models all day without grief. Parasolids export great using UG, but NOT Pro/e. If the step file is missing faces, IGES has always been a solid format. If you are still having problems, then you must look elsewhere within Pro/e.

[CJep]

step files will work sometimes coming out of Pro-E it depends on the complexity of the part file and how the geom was generated (did the designer/engineer take short cuts?)

 

The best results typically come from the native file type.

 

If you're getting step files from a vendor that are seriously "jacked up" we have used a seat of SWorks to open the step then let SWorks run the diagnostic utility and fix the issues. The usually sldprt opens in Mcam with no missing faces.

[strabe]

I usually don't have a problem with step files unless they're complex like peon said. I never use iges. But I also have the ProE translator option installed so if your boss will spring for it, get it.

 

HTH

 

Ken

[Mr. Wizzard]

Look some more for topics on the same issue. I had the same problem here. Some engineers were experimenting with Pro-E. It seems that if the tolerance settings in pro-e are "wide open" , they could create complex surface models that were not necessarily correct. The models would come into mcam with gaps, missing faces, etc....

Mcam, i'm guessing, did know what to do with the surfaces or features that were not seamless or with out fault.

I ended up having them save as .prt (pro-E) files and step files. So far, i've never had a problem with the step files. And let's just say you can be sure the surfaces ARE definitely created with flaws!

works so far

[Müřlıń®]

Proe is a very powerful tool. Problem is, not many know how to use it.

 

I think the default tolerance is Proe is .0012.

That is a freaking mile when calculating NURBS endpoints/tangents.

 

Very small models should be built with no greater than .0001 tolerance and then you must also have Mastercam set up on a small cordial deviation when dealing with NURBS.

[Müřlıń®]

I see this topic come up allot about missing /non trimmed surfs coming from ProE IGES/STEP files.

There is nothing wrong with ProE except operator error.

 

I would like to add something to my above post.

 

Proe has 2 different tolerance configurations.

Relative and absolute. To change the config, click on the edit menu bar at the top of the window and click on the pull down button "setup".

This will prompt another pulled and click on tolerances.

 

The default is a relative format. This means that the tolerance will differ depending on the part size. so very large or very small parts will be problematic if left in the default configuration when it comes to exporting generic formats.

 

However, as in any CAD-CAM software, system performance is greatly affected by changing these settings. So those of us who are still using SUN boxes equivalent to a p III 900 MHz CPU will need to use tolerances as close to default as possible.

 

The max system tolerance for ProE is 6 decimal places. The default is .001, which is 3.

 

The default tolerance config is relative and the min/max values are calculated from the system tolerance.

 

To access the system tolerance from ProE, on the top menu bar is a "tools" button 3rd from the right at the top of the page. Down at the bottom of the pull down will be an options button.

 

This will bring up the main options page and the very first entry is the system tolerance.

 

Most will see .001 there...

 

The min tolerance for this setting will be .0001 for relative, and .0004 for absolute.

 

For most of us here the default will NOT work.

 

For those of us that have to work with customers who will export generic files to us, we will need to be on the same page as far as tolerances go or there will be problems.

 

Most of us will need to use an absolute setting of the SAME tolerance when file sharing especially with IGES.

 

On one last note....changing the tolerance of a part file will cause part regeneration.

On parts with hundreds of features, this may no work out so well.

 

It is way easier to start off building your parts with the correct tolerance you need to insure that the generic file converters will preform as expected.

 

HTH,

 

 

Murlin

[Redfire427]

This has been an ongoing issue our company has had to deal with for roughly 6 years. Merlin makes some good points about tolerance and such, but to no avail. The best solution we have come up with is the Solidworls fix as described above where you can import the file and find all the errors and fix them in Solidworks. We have the ProE translator for Mastercam and it does work fairly well, but in most cases ( if not all ) you still have to open levels that are shut off and then delete all the extra surfaces and wireframe that come in, leaving just the solid.

 

My understanding is that ProE is not capable of building a proper parasolid based on the technology that it utilizes. Something to do with the granite kernal versus another kernal.

 

I wish there was a simple answer to this, but we have just reserved ourselves to the fact that file conversion between different CAM & CAD packages is difficult. Solidworks to Mastercam is a dream compared to all the other formats/systems.

[gcode]

I bring ProE files into Solidworks as an IGES

then run Import Diagnostics.. then export as

a parsolid.. this is normally a bulletproof solution unless the ProE model is really bad.

[Müřlıń®]

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My understanding is that ProE is not capable of building a proper parasolid based on the technology that it utilizes. Something to do with the granite kernal versus another kernal.

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That is true. However it is not a bad thing.

 

A parasolid is a very loose built model. It forgives edge gaps and endpoint errors, overlapping edges ect, and still meshes the features together to achieve a watertight model.

 

The ProE kernal requires a higher degree of accuracy.

 

To achieve high system performance, a large model may adjust itself to an internal tolerance of .03 when it is set to a system tolerance of .001 and a relative tolerance configuration is used. Now this is fine within the boundaries of the ProE kernal.

 

However, when that model is exported in generic surfaces or solids, that loose tolerance will have gaps the size of the grand canyon, especially in IGES.

 

Now take that same model, import it into a different system and then convert it to metric, or vice versa...what is that 25:1 ?

 

Houston we have a problem...

[Mr. Wizzard]

This has been an ongoing, difficult, and mysterious problem facing many of us. Murlin, I thank you for your explaination. It seems to help us, at least me, figure out the "why". The information you have provided here has been tremedously helpful and allows us with an option to suggest certain settings to the designer.

The thing i don't get is how we can be expected to produce some parts with very tight tolerances on a sloppy model.... especially when we don't have a print to go by at times

It's hard to get this through to engineering sometimes.