I thought it might be nice to gather some CAD translation tips here in one spot. I’ll start out with a couple.
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Some formats like IGES and SAT have scale factors built into the headers, so you can scale parts before you bring them in, or scale them if the units settings are messed up.
Do a round trip on your data before sending it to someone else. If you can’t read your own data, how is anyone else going to do it?
Always ask for settings or formats you want right up front. It is easier to fix data translation problems by preventing them in the first place.
Solidworks actually has 2 separate built in import translator algorithms (at least as far as SW 2018 is concerned…they may have consolidated it in later versions…I have no way of testing it)
If you import a file using 3D interconnect, and then import the same file without using 3D interconnect, then it has been imported using a different algorithm.
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The 3D interconnect algorithm is much more robust and does a significantly better import than without it.
So I always import using 3D interconnect on, and then immediately dissolve the feature.
I have no reason at all to keep the link with the original file that 3D interconnect creates.
Generating a Parasolid file (X_T or X_B) from Parasolid based apps (Solid Edge, NX, SolidWorks, Onshape, etc…) is not a translation. It simply writes the parasolid body out to a file, so it gives the most reliable way to transport 3D data between those systems.
Quite likely but have lacked time and enthusiasm to solve. Given the frequency with which SW fouls up importing its own step exports, I tend to just shrug my shoulders and use a different format.
Every format has its foibles. A few years ago STEP had a habit of inverting spheres and toruses (commonly on corner blends), especially coming from Pro/E.
Never tried dissolving this after import, but I’ve had users default disable 3D interconnect since I’ve run into too many instances of someone using it to import a STEP file, but having the reference outside of the PDM vault. I’ll have to test out the dissolving method, but for now we import without 3D interconnect unless we absolutely need it (but I make sure the STEP file is saved to the vault first).
Any time you have an error with the process where you are not using 3d interconnect, try it with it on and dissolve it. Test it on a problematic import.
As was said above…if you are exporting from solidworks to solidworks, you should always use parasolid (X_T). Parasolid is the native kernel for Solidworks and there is actually no translation happening. It is just saving out the geometry.
I do export as parasolid if going to other SW users but don’t always have the luxury of knowing what system the downstream user will be on.
I always dissolve step features as mentioned above (if I haven’t remembered to disable 3d interconnect) as a lot of body check errors disappear after doing so. Reading above I now understand why this would be the case. I would have thought that round trip via step should be okay …
Communicate the Coordinate system you need if it matter to you (Y up, Z up etc)
If you are getting neutral files from 3rd part, try to get different format (eg: STEP, IGES) at once…
Sometime the export messed up and the other format work better…
The last thing you want is to get a bad exported file and need to wait 12hr because of timezone difference
Importing STEP 242 can be a mess… or so i heard
Hole Wizard data will not be exported…
If you are dealing with parts with tons of hole, clearance, tapped, etc, plan out earlier how can the the data be exported (Drawing works but can get rather confusing with large number of hole, sometime it just take 5min to setup the proper appearance for different hole )
If the neutral file you created is huge, you might want to use a different approach (eg: export subassembly instead hla, etc)
(Importing a 600mb step file take a huge tons of time)
Appearance can be useful but can also mess up the performance.
If your PDM does not support 3DInterconnect from SOLIDWORKS (eg: Windchill), turn it off before importing
I agree with this… but also found myself guilty for not following it most of the time
If i am exporting a large number of STEP file (eg: for fabrication), doing the round trip can be really time consuming…
It might be easier to just assume everything is fine and reexport when there is issue…
Sometimes what work on my side might not work on the other.
I’ll bet you heard this from a SW user or sales guy. When you import (Solidworks parts via) STEP 242 with dimensions on the 3d parts into Solid Edge, those dimensions are live in synchronous. That makes imports a lot less dumb.
Unless they specifically request STEP file (then 2 separate translations are happening…1 from parasolid to STEP, then from STEP to their system), I always give Parasolid files to suppliers/customers. If they can deal with it…great. Then that means that only 1 translation happened (from parasolid to their system).
