Hey everyone,
I created a plastic housing use a multi-body part file (master file). I saved out each individual part file using "Insert into New Part", and then added engineering details into each of these parts. Lastly I created an assembly from these parts.
After getting pretty far into the process, I realized there was an issue with my housing design. I went back into the master file and made some pretty major changes. I ended up splitting one of the bodies into multiple smaller bodies. After finishing these changes, I went back to the individual part files and got the error: "The base part has no solid".
I want to reattached my part files to their corresponding bodies in the master file. I listed external references in the individual part file and it points back to the master file. So it seems like the unique body ID in the master file changed, causing all of the individual part files to lose their references.
I know if I had used the "save bodies" command, I could open up that command and point it back to the correct body in the master file. Is there a way to do this using the insert into new part command? I'd like to avoid needing to remake all of the individual part details .
Thanks for any help!
SolidworksParts And Features
Hi Maxwell, if you have access to the Customer Portal, you can use the Knowledge Base to research SPR 506725, this details this error message. I am guessing it is indeed because the ID of the master part body has altered and seemingly eludes to a boolean type operation. Was the split feature the only thing you did, as i have tried a very simple use case and the child part maintained the reference okay.
My thoughts are, a) future strategy is instead to have the master part modelled, and then create a new part for the child and use Insert > Part and bring the entire master model in and then delete the bodies you do not need as your first feature. It still has the external reference to the master but as you pulled in everything to start with, it should react more reliably to changes. b) Save bodies would work, but as this places a historical feature in the tree you may need to rollback, or reorder this feature to keep at the bottom of the tree, otherwise additional changes to the master that appear beneath the save bodies command won't filter down to the child parts. c) this is a bit obscure and I haven't tested this, but how about doing another "Insert into new part" from the master model with the bodies split up further. Then for your original (broken) child part, use File > Open and change its reference to the newly saved "Insert into New Part" - now I would think some downstream references would need tidying up but you may get lucky- it will also give you an extra level of references that you would have to manage (Master > New Child Part > Original Child Part) but it may work.
Hey Adam,
In additional to the split, I also changed the geometry using a bunch of pre-existing splines, lines, etc and added new fillets/chamfers.
For strategy a), I have seen it used before and that sounds like it could be more robust than just creating a new part for the individual body. The downfall is the file size now gets much larger. I've heard this can increase file sizes by 5x (depending on how complex the master file is).
If I had used saved bodies in this case, I wouldn't be having this issue because I could go back into the save body command and reattach the missing references. I am surprised the "insert into new part" tool does not allow this same control.
Your strategy c is very interesting and might work. I'll give it a shot. Thanks!
This seemed to re attach my solid body when using insert body into new part.
The issue is that the stock body cant pick which body to use in the master multi body file, (somehow your solid body got rearranged in the solid bodies list).
What i did was:
1) open the multi body file and the part file with the stock body error.
2) Use delete/keep body command (use search commands in upper right of screen if you can't find it) and delete all bodies except the solid body your trying to re-attach.
(this gives SolidWorks only one option but to use the one body that is left behind)
Maybe rename this feature so it could be more descriptive like (like body #5 editing feature)
3) Ctrl Q (on both files, This should bring back your model)
4) Right click the stock feature and left click list external references. Then Lock all References. This lets you suppress the delete/keep body command on the master part file. (if you don't do this the part will error out again.)
5)Suppress the delete/keep body command. By suppressing that last command you can bring all you bodies back.
6)Ctrl Q both files
7)Save both files.
This worked for me, Let me know if it works for you.
If you have to go back and edit this part file.
1)Unsuppress Delete/keep body command. [Multi body master file]
2)unlock external references. [part file] the one that will error out
3)roll back so new features appear above delete/keep body command. Make edits, then roll back down after changes.
4)Ctrl Q both files
5)Lock external references on part file
6)Suppress delete keep body command
7) Save both files
I would also suggest adding in a comment with these instructions to the part file so if you or anyone else has to make a change down the line the know the correct procedure. Name the comment Editing instructions.
If SW is "listening", it would be nice to have the ability to redefine the feature that has been "inserted into new part..." so that you could select the appropriate solid or surface body if it is confused.
Does anyone know how SW keeps track of solid/surface bodies (internal ID or something) and what are the conditions where it will not recognize an updated body that was formally "inserted into a new part..."?
You're my new BFF. This trick/tip just saved me 8 hours work!!