Do Facet Settings affect parasolid generation? (solved) 1

[CCD429]

Two machinists that I work with have come back to me with parasolid issues.

The first time, a machinist showed me a missing face on one of the parasolids i sent him. The model was perfect on my end. Even when I loaded the extracted parasolid into a new part file. The machinist was able to work around the issue by assuming both sides of the part were symmetric, but what if they were not?! This could have caused a huge problem down the line if it was not caught in time.

The second time was with our in-house machinist using MasterCAM he showed me jagged edges and what looked like gaps between faces on a parasolid I sent to him. Again, the parasolid looked perfectly fine on my end. Also, again, the machinist was able to work around the issue, but in a tedious time consuming fashion.

Also, I have seen edges that should be circular arcs, represented as splines, which causes issues in mastercam.

I have noticed that changing the facet settings from a default value of 1.0 to 20 or 50 greatly improves the graphical representation, but by doing this am I hiding defects?
If i generate a parasolid with a facet refinement factor of 1.0 or 0.5 will i get a lesser quality parasolid than one generated at 20 or 50 refinement factor?

To investigate the issue, we tried exporting step 203 and IGES models which turned out to be worse than the parasolids.

How can i expect a high level of precision from machinists when I dont even know what I am sending them!

Why does a parasolid look perfect in NX and like garbage in MasterCAM?

At the very least, I need to know what the workarounds are. I am using NX 10

 

[jerry1423]

For the most part the parasolid model looks decent to me. I really didn't see anything that would not translate well into another software.

Maybe go into Syncronous Modeling and do an Optimize Face to the parasolid file, it will clean it up nicely.
Doing this will remove your parameters so you may want to import the parasolid in a temporary file, and do the Optimize Face in there.

As far as the facet setting goes . . . I have never seen that in the parasolid export (I am on NX8.5), only in the stl export.

 

[CCD429]

Thank you Jerry, but are you opening it in NX? I know that it looks fine in NX, the problem is when its opened in mastercam or other cad, FreeCad also shows jagged geometry.

I am glad you brought up Synchronous Modelling. When I took the Siemens training course the instructor specifically warned us that synchronous modeling should be used sparingly, as it can lead to "issues" down the line. This was a certified Siemens NX instructor.

For better or for worse, there are A LOT of tools and functions in NX, I assume they have varying degrees of accuracy and precision. It would be nice to know which functions to trust more than others. for example, i imagine the Extrude and Revolve functions are highly trustworthy. However the Heal Geometry and Optimize Face may have different levels of accuracy. On top of that, they may have different levels of accuracy when applied different types of geometry.

 

[CCD429]

thread561-97771

"Part of the problem is system tolerance, and both system should be at the same level....These will case major trim headaches if system tolerance are not identical. Use UG's Analysis->Examine Geometry to check for these errors and a few more to give yourself a fighting chance. " -tteboe (Automotive) 12 Jul 04 18:12

Does anyone know more about this?

How do I check what my "system tolerance" is?

Here is another problematic file. I used the Examine Geometry to find "bad" edges.

 

[SDETERS]

For what it is worth I exported out a STP out of NX and re imported the stp file back into I-Deas. There are a couple free surfaces that now show up. I did the same with NX and the stp file imported nicely wihtout any issues. To find solutions to these translation issues this is the work flow I use. This Will not work to much longer for us, because we are not going to have access to I-Deas much longer. Anyways I attached a parasolid of what I get after I-Deas.

So now I would go in fix these surfaces in this parasolid with fill surface, surface tools and re export out. Usually this fixes the issues.

 

[cowski]

Short answer: No, the visualization facet settings do NOT influence the geometry that is exported.

There are two major steps when sharing geometry between two different systems:
[ul]
[li]export geometry from the first system[/li]
[li]import the geometry into the second system[/li]
[/ul]

Ok, nothing groudbreaking there; but remember that errors can creep into either or both steps. I'm not familiar with MasterCAM, so the only thing I'll say about it is: check to see what version parasolid it supports. When exporting a parasolid from NX, you can choose what version of parasolid to export. Pick a version fully compatible with the version of MasterCAM that you are running, otherwise you may never get a good import.

The rest of my post deals with exporting from NX.

Rule #1: make sure the geometry that you are exorting is valid.

Before exporting anything, be sure to run the examine geometry command. When selecting objects to check, make sure to window select around the entire model; this will ensure that you have selected the solid body along with all faces and edges (single selecting the solid won't get it all). If the geometry that you are exporting is a solid body, it should pass all the "body checks". If any of the body checks don't pass, don't expect good results after the translation. The "self-intersection" test under "face checks" is also a "must pass" type of test. The other checks are of lesser importance.

I imported the first parasolid (bad_geometry.x_t) into NX 9 and it did not pass the face: self-intersection test. NX indicated errors in the same location that SDETERS' file had issues.

The "optimize face" and "heal geometry" can be used in an attempt to clean up the geometry. If you have a fully parametric design in NX and depending on your business needs, you might prefer to edit the model to clean up the geometry yourself.


As to your other questions:
The modeling tolerance, for a given NX part file, can be found by going to: menu -> preferences -> modeling. The distance and angular tolerances will be listed on the "general" tab. Some features will let you specify the tolerance to use for that feature; don't change the tolerance for individual features unless you have a very good reason to do so. I think the default modeling tolerance in NX was tailored to the automotive industry. The values work well for a variety of industries, but if you make something much much larger or much much smaller, you may want to adjust the tolerance to suit.

When I took the Siemens training course the instructor specifically warned us that synchronous modeling should be used sparingly, as it can lead to "issues" down the line.

I'm not sure what "issues" the instructor was specifically alluding to. I've not seen synchronous cause any issues specific to exporting geometry; but if he meant "a model change may cause the synchronous features to error out, requiring you to redefine them", then I would have to agree.

www.nxjournaling.com

 

[CCD429]

Thank you cowski, sdeters and jerry1423.

I've now got a much better understanding of the problem, and some ways to prevent/fix it in the future.