I have an IFC file with 1000's of box section (all identical in tekla) but solidworks converts them all into separate parts.
Is there any way of getting SW to just reuse the one part file for all of these box sections? (and fixings and plates etc).
using SW 2019 sp 5.0
You'd think that'd work except it doesn't. Simply because the imported bodies (in the part) are all in different locations and orientations.
Besides who wants to do a replace on over 10000 parts? I want to know if solidworks can automatically do this while it's calculating the import?
Orientation and location shouldn't matter if they are identical, and you can replace more than one at a time (as shown, use shift-select). I haven't tested with more parts, but in principle this coud work, why not try?
Ups - didn't catch that the parts are NOT identical. In that case i believe you are out of luck.
The problem is they are identical bodies but SW doesn't create identical parts with these bodies.
(They are identical parts in Tekla)
Owen Johnstone wrote:
The problem is they are identical bodies but SW doesn't create identical parts with these bodies.
(They are identical parts in Tekla)
This depends mostly on export, some on import.
Your export program must export the bodies in such a way that the exported file lists them as copies of one another. This is possible in SolidWorks: When you are exporting from SolidWorks, this is achieved (per my memory) by making sure that you do NOT select "Flatten assembly heiarchy" in the export option. This will export the full assembly/subassembly structure, along with the required information that some bodies are instances of the same part in different orientations/locations/etc. If you flatten, then when you import back into SolidWorks every body becomes its own file.
If your other software can't export properly, SolidWorks won't be able to import it. I'm pretty sure there's no way to tell SW to analyze the geometry of every body, compare that geometry to every other body, and determine that they're identical.
Hi Owen
This probably won't work for you, but...
In my work (woodwork) I create identical parts in sub assemblies that I would like to combine.
One way I achieve this is to save as a multibody part and allow the cutlist to combine identical items.
It's not ideal by any means but for me it's a fast way to get a toplevel cutlist.
It would be possible to then save out the bodies in individual files if required by using the Derive resulting parts from similar bodies of cut lists option.
Hi Rob,
This gets me 50% of the way there. Now all I need to do is go back and replace all the common parts in the assembly....
I was creating an assembly from a multibody part the other day when I noticed the "Derive resulting parts from similar bodies or cut list".
It creats an assembly with only one part per cut list item.
This works perfectly for what I want it to do!
for those interested in where this is
insert -> features -> Save Bodies
That's the badger
Replace component: