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Broken references from master part file

Question asked by Jim Bourque on Apr 21, 2014
Latest reply on May 12, 2014 by Terry Thom

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Hello,

I created a master part file with many seperate bodies and then right clicked on the solid bodies and clicked "insert in to new part".

Somehow a few of my parts now have broken references and are unable able to update when I change the master part file, and there is no sketch in the part because it was created from the master so I'm unable to modify it at all.

Is there a way to get those references back? The only way I could figure how to do it was to recreate the part again and overwrite the existing broken part. This is not the ideal method because most parts have many other features done to them once created as a part.

Thanks - Jim

SW2013 SP4.0

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Dwight Livingston Apr 21, 2014 12:55 PM
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Jim

One approach would be to roll back to first feature and insert your master part there using Insert / Part. Delete the unwanted bodies, then shift all the references to the new body. Major work, but maybe better than nothing.

I find that SolidWorks easily loses track of body identity. I don't know if that is what happened in your case, but it might be. I prefer to insert the entire master part and delete bodies for just that reason. It allows me to reselect the bodies.

Dwight
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- Jim Bourque @ Dwight Livingston on Apr 21, 2014 1:16 PM
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  Dwight,
  
  I know I didn't delete any references so I'm assuming it was SolidWorks losing track of the body identity. It's too bad they can't make this function more robust because I think this is a great concept. It makes building the assembly so much easier because you avoid mates....less mates, less errors. The real kicker is, I was showing my boss what a great way to create models and this happened. needless to say, he's not sold on the idea.
  
  I've worked with other companies who have inserted the entire master in a part and deleted, or surpressed...not sure which, the unwanted bodies. Now I understand why.
  Doesn't that make for huge files tho?
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  - Dwight Livingston @ Jim Bourque on Apr 21, 2014 3:33 PM
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    Jim
    
    I don't think it makes a larger file, as that is more dependent on the final geometry. I could be wrong.
    
    Dwight
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- Terry Thom @ Dwight Livingston on May 12, 2014 9:16 AM
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  It does make for much larger files. Did it both ways on my part on the one file is 3,600 KB and the other is 540KB.
  
  I am using both methods now and the "insert into new part" seems to be more stable. At least I dont have to continously delete bodies out of all 10 parts. I still have a couple parts that I am going to leave with the delete bodies method just to see which gives me more headaches as I go.
  
  BTW i submitted a enhancement request on this issue and they said they would work on it so lets hope. SPR's reference number is: 784140
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Denny Peter Apr 22, 2014 7:00 AM
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Hi Jim

After creating the new part, are you saving it seperatly? if so references may go. Also if you create a part in an asembly and deleting the assembly, but using the new part in some other assembly will not help to retain the references.
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- Jim Bourque @ Denny Peter on Apr 22, 2014 9:43 AM
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  Denny,
  
  I create a part with seperate "Solid bodies" and RMB on each body to save the parts seperatley and then add them all to an assembly.
  I'm not creating a part in an assembly.
  See attached example
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Denny Peter Apr 23, 2014 3:03 AM
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Hi Jim

For me its working fine, You may have to uplaod the files here
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- Jim Bourque @ Denny Peter on Apr 23, 2014 9:08 AM
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  Denny,
  
  It was working fine for several weeks until one day it just decided to break references on it's own on a couple of parts.
  
  I've already gone thru and deleted the broken parts and recreated them. Luckily I hadn't done a detail drawing of them yet, or else I would be redoing those as well.
  
  I was just curious if there was a way to get the broken references to link back to the master?
  It doesn't sound like there is.......
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  - Matt Gortner @ Jim Bourque on Apr 23, 2014 9:34 AM
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    Did you rename any parts or move any files? What symbol is next your "stock" part -->? (reference not open) or -->x (reference lost)?
    
    I recently lost a reference through a part created in this manner and I think it was due to name change. I don't think there is a way to fix it.
    
    You may find the "save bodies" feature more robust and safer to use. You could also try creating in-context references in an assembly. It's not ideal because you'll have extra parts (a "master" assembly and a "functional" assembly).
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Glenn Schroeder Apr 23, 2014 9:46 AM
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I agree with Dwight about SW often losing references on parts (or bodies from parts) when inserted into other parts. I don't often use the procedure; usually only if inserting a hex nut into a multi-body part that will be welded to structural steel, and then I'm fully prepared for and expecting the reference to get lost.

And I don't know that I agree with you about the "less mates, less errors" theory of this being a better workflow than assemblies. Mate errors get less frequent the more I work with SolidWorks, and they're usually pretty easy to fix. That may not be the case with your broken reference.
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- Jim Bourque @ Glenn Schroeder on Apr 23, 2014 10:34 AM
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  Matt,
  
  it was the ->x symbol. Now that you mention it, SolidWorks crashed and the autorecovery made me save my file as a different name after I had worked on it for a while....that must have been it.
  
  Next project I do, I will try what Dwight suggest and insert the "master" part into a part and delete unwanted bodies.
  
  Why is the save bodies any better? It seems like it makes an extra step. Will that allow me to rename parts after they are created?
  If I do as Dwight suggests, I believe I can rename parts and still retain referneces as well.....
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  - Matt Gortner @ Jim Bourque on Apr 23, 2014 1:27 PM
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    You can always rename parts, but make sure to use Solidworks Explorer. You do this by right clicking the file in Windows explorer, and under "solidoworks", pick rename. It will find all the parts that reference it and update them. Very powerful.
    
    Save bodies is a nice reminder in the master file that you have exported bodies to other parts. Other benefits:
    -You can export a body at a less than final state, ie. you can export and then make subsequent changes to the body for other purposes.
    -You can edit the stock feature. I think you may be able to fix a lost reference but I haven't had to test it yet. You can't do this with "insert into new part"
    I don't know for sure if it is any more stable than other methods. There may be other benefits I'm missing.
    
    One note on insert part - beware that the inserted part can jump around for no reason. I've run into multiple instances (SW 2013) where my inserted part loses its mates. I have to delete the mates and re-assemble it. It's fairly random and I was never able to nail down the cause. I try to avoid using it for this reason.
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