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SolidWorks - Body-Delete/Keep featuremanager

motion guru

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Dec 8, 2003
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I imported a step file of an Electrical component that is overly detailed and the part file is 21MB . . . I thought I could just select the exterior surfaces of the parts I wanted to keep and delete the rest of the bodies, but the bodies appear to be retained in the FeatureManager.

So while the bodies / surfaces are no longer showing in the model, they appear to remain in the file as the file is still huge. I was hoping to get it down to a Meg or less.

Is there an easy way to delete all of the "Body-Dlete/Keep" items out of the feature tree? If you select them and delete them, the bodies just show back up in the model and the file size stays the same.

Is there an easier way to do this and I am missing something? How do I get rid of the items circled in red below?

featuretree.JPG
 
I'm confused, are you clicking the delete/keep body button? Because that will generate those deletions as a feature like you're showing. Try just highlighting the parts you want to delete in the tree and hitting the delete key on your keyboard.
 
Try saving it as a STEP file again, then save as a SolidWorks Part,

That was the first thing that I did . . . made no difference.

I'm confused, are you clicking the delete/keep body button? Because that will generate those deletions as a feature like you're showing. Try just highlighting the parts you want to delete in the tree and hitting the delete key on your keyboard.

when I highlight the parts in the tree and press delete - SolidWorks 2020 creates the "Body-Delete/Keep" item in the feature tree, the parts disappear from the model and I thought I was happy until I checked the file size and it remained the same. I then deleted the "Body-Delete/Keep" items in the feature tree, and the feature was deleted from the FeatureManager, but the parts all showed back up in the model. . . obviously not what I wanted.

The model had 2500+ bodies in it, after combing through it, only 28 remain that define what is important for my assembly.
 
I'm confused, are you clicking the delete/keep body button? Because that will generate those deletions as a feature like you're showing. Try just highlighting the parts you want to delete in the tree and hitting the delete key on your keyboard.

Yes, or right click on the M75X_fr01_wo_acc.stp feature and select "Dissolve Feature".
You should just be able to click on a body and hit the delete key.
 
That was the first thing that I did . . . made no difference.



when I highlight the parts in the tree and press delete - SolidWorks 2020 creates the "Body-Delete/Keep" item in the feature tree, the parts disappear from the model and I thought I was happy until I checked the file size and it remained the same. I then deleted the "Body-Delete/Keep" items in the feature tree, and the feature was deleted from the FeatureManager, but the parts all showed back up in the model. . . obviously not what I wanted.

The model had 2500+ bodies in it, after combing through it, only 28 remain that define what is important for my assembly.

That is really strange. I have done this a million times and never had solidworks generate a feature of the deletion. The only way I've created those is by clicking the delete/keep button in the feature toolbar. I just tried this again with an assembly and it just deleted the items, although I'm still running 2019 so I'm not sure if anything has changed.
 
I believe that it is a 2020 feature.
Has something to do with keeping a link to the original step file.
 
yes - dissolving the step file broke the link and disassociated the Body-Delete/Keep features from the model. Now when I delete the bodies, they simply go away.

The little bit of searching I have done on this indicates that this is a change for 2020.

Thanks for pointing me in the right direction.
 
I believe you can turn off 3d Interconnect in the options if you want it to behave as it used to. When enabled you are not actually opening the step file but rather linking to it. It has some advantages. The way it is supposed to work is that say your customer sends you a file you open it with interconnect then you add some chamfers or fillets for machining. If you customer sends you a new version you replace the one you had and the link updates and you keep your chamfers and fillets.

I think all CAD has a version now. I think they license the technology. Autodesk calls it AnyCAD.

Screenshot 2020-10-02 172126.jpg
 
My favorite way of reducing purchased part size is opening it in Rhino 3D which doesn't give a crap about how the surfaces were created and then I delete not only all the internal components but even the internal surfaces of the external part. For motors and blowers with all kind of cooling fins I replace them with plain cylinders. Rhino is the Swiss Army Knife of 3D modelers and at about $800 a really worthwhile investment in my book. I am current and have been using it for about 20 years. Only as a repair tool now but I did complex assemblies with it years ago.
 
My favorite way of reducing purchased part size is opening it in Rhino 3D which doesn't give a crap about how the surfaces were created and then I delete not only all the internal components but even the internal surfaces of the external part. For motors and blowers with all kind of cooling fins I replace them with plain cylinders. Rhino is the Swiss Army Knife of 3D modelers and at about $800 a really worthwhile investment in my book. I am current and have been using it for about 20 years. Only as a repair tool now but I did complex assemblies with it years ago.

Agreed, Rhino is a great tool to supplement SW.
There are some things Rhino can do that SW can't (easily).
 








 
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