Solidworks 2017 Pro SP0.0 ... When I insert a part to create a derived part, the only thing that will insert is the planes/axis. No solid bodies will come in even though the yellow "shadow" is there before I click "okay" on the command. I've tried rebooting Solidworks as well as my PC. Nothing seems to help.
Can you upload the files?
Unfortunately not. These are protected files. I was hoping that this was a quick fix.
I have not personally experienced this but I suggest checking that there are no errors in the either of the files. If either have imported bodies (like from a STEP translation, etc.), I'd run import diagnostics on them (even if they don't show any errors).
Good luck!
Just thought of something... Expand the Solid Bodies folder in the tree and make sure that none are hidden.
All bodies shown. I replied to another comment with my "process" of how our parts are made. I do this process a lot and this problem seems to pop up from time to time. I haven't really found a fix for it.
Andrew Raison wrote:
Unfortunately not. These are protected files. I was hoping that this was a quick fix.
Can you reproduce the issue with simple "dummy" files?
I tried this idea to see if I could, and turns out that I could insert the "dummy" part into a new part. So I guess that it would have to be a problem with my source file. Thank you for this idea.
I'm in SW2015 but are you selecting "solid bodies" from the screen after you've selected the part file to be inserted?
Steve C
Yes, solid bodies is actually the only thing that's usually selected. I do this process a lot, and this seems to pop up from time to time when making my derived parts.
Snapshot of my process:
Receive customer STEP/IGES --> Save that as a part in PDM --> Open that part --> Do all my designing in that file --> Create my part numbers and insert the customer part now with my design in the newly created part --> delete body to remove customer geometry from my model --> make drawing.
From the start with this file, the insert body command looks good. Everything is checked that is supposed to be (in this case solid bodies is all that I need), the part shows in the yellow-tinted "shadow" in the model space, but as soon as I click okay it vanishes and nothing has been added to the feature tree. It is very strange.
Is it possibly hidden in the solid bodies folder?
Steve C
No sir. Nothing gets added to the feature tree after I click "okay". Here are screenshots of before and after clicking okay:
hmm,...can you check the box "Locate part with Move/Copy feature".. and see if it comes in?
I've tried many combinations of checks and nothing seems to work. My source file has 0 errors in it which is why I think this is so odd. I even try simply breaking the link and that doesn't work either.
Andrew.. glad you figured it out and yeah,.. what you concluded by deleting a body.. sounds familiar...
I think I also have gone through this as well... remove/reinsert a imported body...I just can not find the files to reference/share.
Insert Part has had it's hiccups over the years.. but, it's the way to model (ala copygeom in pro/e or creo.. my fav!)
Andrew... very curious... does this thread sound similar?
If not.. the first thing which came to mind was somehow the size/scale of the part.. that is, the 1 kilometer bounding limits are effecting this?
Next.. do a ctrl-q... and also check to see if you have VOR on or off?
Okay, I figured out a way around this. It's not the best, but it still got me the result I wanted without breaking anything!
I just decided to try a "delete body" on the customer part (in the customer part file where all my geometry is), and that seemed to work. Now when I insert the customer part into a new part, all the bodies come with it. I tried this since someone in this thread mentioned there may be something wrong with an inserted .STEP or .IGES.
Thank you everyone for racking your heads!
I am seeing the exact same behavior using SW2014 SP5. I can attach the file since it was downloaded from the internet.
Changes I made to the file:
The download was in STEP format.
The assembly consisted of two parts.
One of the parts has import diagnostic errors that will not correct. (these are due to threads)
I saved the assembly out as a part file with two bodies.
I performed a series of repair surface features to get rid of the threads.
When I place this part into a new part, as described by the OP, I get the yellow ghost preview but only the planes come through.
I have attached both the part version and the assembly version.
The step file can easily be downloaded from the Hoffman website.
Daen
Daen,.. I tested in 2014sp5 and don't see that but after I repaired the thread, I can also see there are many ZTG errors on the bottom housings bosses so, I removed them and one last error on a corner.. then, the top also had a error on the corner. (files attached)
Paul,
Thank you for taking a look at this. Your version inserts into a part file without issue.
I am not very strong with surfacing techniques. I would love to hover over your shoulder and learn your general approach to conquering troublesome imports like this.
As is usually the case, I downloaded to "SAVE" time... and spent the better part of the afternoon. It was no easy thing to raise the white flag and admit defeat!
Thanks, Daen
I had the same problem. I had the same problem. It is necessary to check the part file using the command:
"CHECK" and repair the invalid faces.
Okay, I figured out a way around this. It's not the best, but it still got me the result I wanted without breaking anything!
I just decided to try a "delete body" on the customer part (in the customer part file where all my geometry is), and that seemed to work. Now when I insert the customer part into a new part, all the bodies come with it. I tried this since someone in this thread mentioned there may be something wrong with an inserted .STEP or .IGES.
Thank you everyone for racking your heads!