geometry resolution of the imported parasolid

[mlxjliao]

Hi all,

When I import some UG parasolid files (*.x_t) into Cocreate Modeling with UG NX adapter checked on, I found the geometry resolution of the imported models, is different from 0.01 to 0001, can I have all the resolution of the imported models be 1e-6?

Thanks
Best regards
Johnson

[Andy Poulsen]

Originally Posted by mlxjliao

Hi all,

When I import some UG parasolid files (*.x_t) into Cocreate Modeling with UG NX adapter checked on, I found the geometry resolution of the imported models, is different from 0.01 to 0001, can I have all the resolution of the imported models be 1e-6?

Hi Johnson,

You can set the value under "Load Acc" in the "Options" submenu of the Load menu. The default is "Source Acc" but you can specifiy values from 1e-6 to 1e-1. However, if you specify the accuracy yourself, you run a higher risk of getting corrupt models...

I hope this helps!

andy

[BMaverick]

Johnson,

If by chance your company has SolidWorks you can Parasolid the model data from UGNX to SolidWorks. Next go from SolidWorks via ACIS(SAT) into CoCreate.

We have been doing this now for over a year. The translation is by far clean and the accuracy has been identical to the original data found in UGNX.

Earlier in the year, we had discovered that the STEP translator between UGNX and CoCreate made "geometry resolution" changes. So much, that in a few instances it affected our models for part tolerance of injection molded plastics and machined steels.

BMaverick

[Mike Swartz]

Lets discuss Accuracy, or "geometric resolution" a little. Here is some data directly from the CoCreate help files that may help you understand more about this term.

CoCreate Modeling represents the accuracy of a part as a single numerical value expressed in millimeters. The accuracy cannot vary within a part, but an assembly can have parts with different accuracy values. This value is also called model resolution.

Accuracy in CoCreate Modeling is defined as

Any two points separated by a distance less than the accuracy value are considered identical.
A point less than the accuracy value away from an edge or face is considered to be contained in that edge or face.
Two edges are considered identical if one of the edges is contained in a tube of radius accuracy surrounding the other edge.
An edge along which each point is less than the accuracy value away from a face is considered to be contained in that face.
Any edge is valid if and only if its length is greater than the accuracy value.
While the first four items refer to the concept of gap size (distance), the last item is based on the concept of minimum extent (size of edges). However, there is only a single accuracy value for both concepts. These two concepts are opposed to each other: If you reduce the accuracy value for a given part in order to allow for small edges, you may introduce gaps. On the other hand, if you increase the accuracy value to accommodate gaps, you might lose small edges.

Another important aspect when you import data from other systems is the range of possible accuracy values in both the source and the destination system. For best results it is strongly recommended to make sure that the accuracy value of the model to be exchanged is within the common domain of the accuracy value ranges of both systems.

Guidelines from user organizations like VDA (VDA 4955) or ODETTE specify that geometric data must adhere to certain limits. The coarsest recommended distance accuracy is 1.0E-2 mm. The range of accuracy in CoCreate Modeling is between 1.0E-1 mm and 1.0E-6 mm.

So, in VERY simple terms, "geometric resolution" roughly determines how big a gap can be allowed between adjacent edges. (or edges that are supposed to be adjacent) If the gap between adjacent edges on a part exceeds geometric resolution, the part is no longer a solid. It becomes a face part.

Let's take a simple example like a plate with holes punched through it. Loading this part at a higher resolution as opposed to a lower resolution does not mean that the holes are positioned with higher accuracy. It is all about the adjacent edges.

So, when you import a part that has a lower geometric resolution, and you try to force the resolution higher, the system will try to heal faces in order to allow adjacent edges to lie within the new tolerance. If you set the "variable" switch to on (in the import options) the system will lower the geometric resolution enough to give you a solid model (as opposed to a face part, or individual faces)

[Mike Swartz]

Originally Posted by BMaverick

Johnson,

If by chance your company has SolidWorks you can Parasolid the model data from UGNX to SolidWorks. Next go from SolidWorks via ACIS(SAT) into CoCreate.

We have been doing this now for over a year. The translation is by far clean and the accuracy has been identical to the original data found in UGNX.

Earlier in the year, we had discovered that the STEP translator between UGNX and CoCreate made "geometry resolution" changes. So much, that in a few instances it affected our models for part tolerance of injection molded plastics and machined steels.

BMaverick

Not to bad mouth a particular CAD system, but I have found that STEP translations from Unigraphics tend to have more problems than most. Because both UG and SolidWorks share the same kernel (parasolids) you can pass a parasolids file with no issues.
SolidWorks does a much better job of translation. So, (assuming the Parasolids file from UG did not load as a corrupt model in SolidWorks, you would probably get a pretty good translation to CoCreate Modeling. The only thing I would do different, would be to use IGES instead of SAT. Our IGES and SAT translators both use identical healing functionality. However, with IGES, you also preserve things like part names assembly structure and shared parts. SAT does not pass that data on.

[BMaverick]

Mike,

Thanks for the heads up. Sounds great that CoCreate has a decent IGES interface. The only problem with that is the sending system's IGES. IGES in many circles is called IGUESS because the translation is close enough guess to the accuracy.

Yes, with UGNX and STEP, small parts with higher geometic resolution tends to suffer. The ParaSolid to Solidworks retains everything completely. Then the SAT into CoCreate works extremely well.

Solidworks is an excellent package for translations. For the cost of one seat, in many instances, it's cheaper than adding another translator to two CAD packages for communications.