Best legacy file format for integration/Model compare utility in NX8.5 1

[jchurch]

First post here; I searched the forum for threads on the "Model Compare" utility and didn't see anything on this specific topic:
Can anyone comment on what (if any) imported file type works best with the NX 8.5 model compare tool? My company recently changed CAD platforms from Solidworks and Pro/E to NX 8.5. The conversion work for the legacy Solidworks/ProE file library was farmed out to a company based in India; so far, I have not been able to run a successful model compare on any model that was imported into the NX file format from another software package.

Is the model compare tool only useful for comparing two files that were originally modeled in NX? This is my assumption based on what I'm seeing, but I wanted to make sure I wasn't missing a trick to get it to work.

 

[SDETERS]

Are you using teamcenter? And yes you can do a model compare on two different parts and you can also do it on two different revision of a part.

The revisions is a teamcenter thing that I have used that works great.

Your imported file has to be in a new part separate from the oriningal part for your compare.

For Example start a new part and import your step parasolid and or what have you.

Open your newer NX part in the same session of NX. You now have two parts loaded.

Now do a model compare. Select your NX part. Go to Window switch to your new part you created above. Then select this part. You will get a message about the parts not being the same revision or something like that. Just hit ok and hit calculate. It should show the difference with in the tolerance you tell Nx in the Model Compare dialogue form./

 

[jchurch]

Yes, I am using Teamcenter 9; it's strange that you mention TC working well with Model Compare to evaluate revision differences, because that's always been my main complaint about it. The way we have Teamcenter set up, you can only have one revision of a given file open at the same time. So, if you have part number 123456 Rev A open, you can't open up 123456 Rev B at the same time to perform your model compare. I've alsways saved 123456 Rev A to a new part file (prefixed with TEMP_ so I know it's only for check purposes) so I can get both of my models open at the same time. Will your Teamcenter settings allow you to open multiple revisions at once? I wasn't aware that was something Teamcenter could allow.

Regarding the model compare on imported part files, I may not have phrased my question clearly. I have imported files from ProE or Solidworks already converted to NX and released as a .prt. For new revisions, we have been modeling the parts in NX scratch (in cases where Synchronous Modeling won't easily accomplish all of the necessary changes to the imported model). What I'm seeing on attempt to do a model compare between two files like this is one of two things.

1) NX will not see the imported file as selectable for the model compare (won't even highlight the body when you mouse over it, while the model compare dialog is open). In this case, the "Type" description in the Open dialogue in NX says "Multi-CAD". Not sure what that indicates, but it seems to result in the file not working with Model Compare (or Synchronous modeling, for that matter).

2. NX will output a warning stating that the imported file failed geometry check, and the compare results may not be valid. See attached.

It seems like model compare just isn't well suited to comparing solid bodies imported from other CAD packages...works great for comparing NX models to NX models though. I guess this is a good reason to pick a CAD package and stick with it; too bad my company doesn't seem to share the same opinion.

 

[SDETERS]

For your teamcenter there is a command so you do not have to make a new part. Look into prepare for compare in NX. This seems to be hidden use the command finder to find this functionality.

1) This sounds like you are opening up the Light weight JT file VS a parasolid or step file from teamcenter. Multicad indicates to me a lightweight JT file.

2. This is the error message I was mentioning in my response above. YOu could at least run this compare and research the results. But I have found even if the surfaces lay on top of each other the software still says they do not match. This could be because of small little fillets not matching within tolerance or what have ya.

There is a trick of subtracing one part from another. Seeing what is left over. There are other options. My favorite is doing a drawing overlay in teamcenter and using track drawing changes. But if you are recreating the model I guess the drawing (If Any) is being redone also.

 

[jchurch]

That's right; the drafting isn't much help, since it was all redrawn in NX after the software switch. I was hoping to use model compare for the more tedious, high volume part checks until we had a more well-established NX part library. Looks like it won't work out that way though; lots of measuring will be in order

That's a great tip on the "prepare for compare" feature though! That makes the process way more streamlined. I've been doing model compare the hard way for years; thanks!