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Split a multi-suface body part into multiple parts

Question asked by 1-CKLISI on May 29, 2008
Latest reply on Jun 2, 2008 by Mark Matthews

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I have a multi-(suface body) part that I want to use as a 'master model' to produce seperate parts for each surface. The "Split" feature does exactly what I want except it only works with a multi-(solid body) part. Any help would be appreciated. Thanks.

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Charles Culp May 29, 2008 6:34 PM
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This functionality does not exist. It has been discussed on a thread earlier this year. It would make a GREAT enhancement request.

One thing you can do, and I believe it was the consensus of that earlier thread, was to use "offset surface" with an offset of 0 (copy surface). This will create a copy of the surfaces to use as your child bodies. If you want them to be in separate part files, simply create an assembly, and create the child parts in-context with that assembly.

I found that thread, and Matt Lombard's suggestion was to copy the body, and then trim off everything that "isn't".
https://forum.solidworks.com/f...catid=20&threadid=8994
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- 1-CKLISI @ Charles Culp on May 29, 2008 8:21 PM
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  Charles, Thanks for the help. I made my first enhancement request today! Hopefully that'll be in 2009; it seems like a quick fix improvement but I could be wrong. I've got several thousand surface bodies inside a part that I need to turn into seperate parts. The only way I've known how to do this was to select each individual surface 'on-at-a-time' and 'save-as' -->'selected faces' and name my file. But then, that file is not associated with the master model and it becomes a bookkeeping chore to keep track of the changes made and remeber to resave each individual part.
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  - Dwight Livingston @ 1-CKLISI on May 30, 2008 11:54 AM
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    Jon
    
    I'm not sure what you're after here, but I'll make a stab. Sounds like you have a part file with no solid bodies and thousands of surface bodies. You want to have a thousand part files each with one surface body linked back to your original part file.
    
    What to might do is make a new part file and insert the original part into that. Then select all the surface bodies and delete them. Make a thousand copies of this new file. Go into each one and edit the delete feature, removing one of the surface bodies.
    
    It may be a lot easier to just make configurations using a design table in your original file. Unfortunately, you can't specifiy which surface bodies get deleted in a design table. You have to delete each surface body in its own delete feature, and then suppress or unsuppress all those delete features in the design table.
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    - 1-CKLISI @ Dwight Livingston on May 30, 2008 1:34 PM
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      Dwight Livingston wrote:
      
      I'm not sure what you're after here, but I'll make a stab. Sounds like you have a part file with no solid bodies and thousands of surface bodies. You want to have a thousand part files each with one surface body linked back to your original part file.
      
      Yep, exactly what I want to do. Here's a further detail of what I'm doing. Perhaps there is something else I could consider:
      1. I've got one part file with many solid bodies that I'm starting with.
      2. I want to turn these solid bodies into surface bodies so when I'm done building this part I select all of the faces that I want and export only these faces into a new part file (In my case it is far easier for me to export only the desired faces rather than to delete the unwanted faces). -->(If I could simply export these faces into an assembly my problem would be solved)
      3. Now I've got the new part file, after I import it, that contains all of the surface bodies and zero solid bodies.
      4. From here I need to split these surfaces up into multiple parts and construct a new assembly with all of the new parts.
      5. So now I have an assembly consisting of individual surface body parts that geometrically match my original surface part file of 'Step 3'.
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      - Mark Matthews @ 1-CKLISI on May 30, 2008 5:18 PM
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        Can we ask why you want the parts to be surface bodies and not the solid bodies you're starting with?
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        1-CKLISI @ Mark Matthews on May 30, 2008 5:30 PM
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        I'm not using SolidWorks to produce any drawings for anything that will physically produced or analized with FEA. However the model will be used for a physics based simlation that requires only surfaces to be defined without any volumes (fully enclosed surfaces). It will only remain is a digital 3d model and coverted into another format where the thickness for each surface is applied
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        Mark Matthews @ Mark Matthews on Jun 2, 2008 5:04 PM
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        Sounds like you want a way to export all your surface bodies so that the program you're going into will interpret them as seperate entities? Have you tried exporting as IGS? If you make all the surface bodies a unique color, some programs will interpret that as being seperate elements and may put them on different layers in whatever program your importing to.
        
        Hypershot does this.
        
        Do the bodies share boundaries? If not, then they might be interpreted as seperate elements. It all depends on how your software interprets the IGS file. I know that when I've imported IGS into Rhino, all the surface patches come in as unique surfaces, but all bodies, solid and surface, end up on their own layer.
        
        Sounds like you want to blow up your model (physics simulation).
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      - Jerry Steiger @ 1-CKLISI on May 30, 2008 6:52 PM
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        Jon,
        
        If I understand you correctly, it seems like the easiest solution for you is to split your original multi-body part file, making a new assembly with all of the solid parts that you need for your surfaces. Then edit each part and Knit or Offset 0 the faces that you want. Delete or suppress the solid body in each part. Now you have an assembly all all the surface parts.
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  - Charles Culp @ 1-CKLISI on May 30, 2008 12:48 PM
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    Since this has come up before a few times, I have attached an example of how to create a "surface master model". This method uses in-context parts, that use the "copy surface" command based on a master part.
    
    Thank you to Mike Wilson for the Roman Surface model.
    
    Note that there is another method discussed in this thread: https://forum.solidworks.com/f...catid=20&threadid=8994
    Which uses one part file, that you then use the "copy body" command, along with "trim surface" to create multiple bodies in a single part file.
    
    What's the difference between the two methods?
    With the method attached you get parts in separate part files. The surfaces lose their history, but will automatically update with the master model. If you add/subtract surfaces from the master, you will have to recreate the "copy surface".
    
    The other method only uses one part file, which you may not want. It may also take longer to rebuild. However, it will have the history, and if you add/remove surfaces, you will only (possibly) have to recreate the trim feature.
    Attachments
    SurfaceMasterModelExample.zip3.8 MB
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Split a multi-suface body part into multiple parts

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