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Add body to "Insert to New Part"

Question asked by Vald Mand on Dec 28, 2020
Latest reply on Dec 29, 2020 by Tim Rosendal Halvorsen

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I have this Layout, with 5 Bodies.

I have done "Insert Into New Part", and Inserted all arcs into another part:

I need to add Triangle to Arcs (not overwrite, only add as a body to existing Part File). I can't figure out how to do it. Because, when I do Insert into new part, Solidworks overwrites the previous file instead of adding additional bodies.

This is an easy example of course, I am referring to more complicated Weldment assemblies, where drawings had been made. And in times when you need to add one or two more bodies to exported Weldment (Saved Externally with Insert Into Part) , I don't really know the way to add them, without overwriting the previous file and loosing all connections to drawings.

Please help!

P.S. in case anyone wonders, sign is from Harry Potter, Deathly Hallows.

Tim Rosendal Halvorsen Dec 29, 2020 4:01 AM

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Hi Vald

Not entirely sure why you are not making assemblies, or assemblies with virtual parts - but the way I'd go about something like this, would be by using the Insert Part feature.

I made a video showing this on your files, so this might help you or confuse you

Here it is: 2912202001 - YouTube

Tim

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Arcs.SLDPRT.zip109.3 KB
Layout_Decoration.SLDPRT.zip134.3 KB

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Maha Nadarasa Dec 28, 2020 7:02 AM
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File?
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Deep Shukla Dec 28, 2020 7:10 AM
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Hey,

I think you save your triangle as a part (externally) and after that insert into arcs,
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- Vald Mand @ Deep Shukla on Dec 28, 2020 7:41 AM
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  Yep, agree with this method.
  Although, I hope there is another way. Much more easier. Like Add bodies of layout directly to the sub assembly (SubWeldment for example)
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Maha Nadarasa Dec 28, 2020 7:32 AM
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- Part7.SLDPRT.zip116.5 KB
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- Vald Mand @ Maha Nadarasa on Dec 28, 2020 7:47 AM
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  I don't know, which version of Solidworks you are using, but I can't open your file.
  and 2nd, I think from the image you've posted, you did not understand the topic of this thread well.
  I try to be more precise:
  I am looking for a way to export bodies (weldments, sheets, simple bodies) to parts.
  Like making a sub-weldment.
  When you insert bodeis into parts, you get a part file with bodeis from layout. The problem is, I need to g oto layout, and add additional bodies to already exported ones.
  Problem that solidworks instead of adding bodies, can only overwrite the file.
  Maybe there is a way to do that normally?
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Maha Nadarasa Dec 28, 2020 8:36 AM
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- Part & Assembly.zip400.9 KB
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- Vald Mand @ Maha Nadarasa on Dec 28, 2020 8:53 AM
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  Thank you for your answer. I wan't to avoid assemblies, because it saves all parts as a separate file. Problem comes when you have same parts (pipes, sheets, etc.) and they are all saved as separate parts. There are some tutorials on that too. In the end method is a mess.
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Elmar Klammer Dec 28, 2020 8:38 AM
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See multi-body parts and rename - a warning! | SOLIDWORKS Forums for a way to achieve it with save-body feature
See Rename base part and keep external references | SOLIDWORKS Forums for a good explaination between save-body and insert-into-new-part feature
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- Vald Mand @ Elmar Klammer on Dec 28, 2020 9:01 AM
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  I tried first method. Saving bodies over the top. as I mention before, it overwrote the files and drawing connection dissapeared.
  Honestly, solidworks have some frustrating drawing/part management ever... anyway. it is not the point
  Somehow I believe there must be a way to add derived bodies to part..
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  - Elmar Klammer @ Vald Mand on Dec 28, 2020 9:07 AM
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    Hi Vald,
    
    You don't have to make the assembly. Save Body inserts an editable feature that you can modified in the new part.
    Along the line as in your example. Similiar but not the same.
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    - Vald Mand @ Elmar Klammer on Dec 29, 2020 2:01 AM
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      Hello, Elmar,
      what I want to explain is in this example:
      I am saving a "Triangle" and a "Mark":
      
      It saves them separately:
      I want them both to be in the same Part.
      Using Insert Part again to insert all separate parts into one, looses its meaning.
      I want All exported body relationships to stay purely between the Single Layout ant the Single Derived Part.
      Single Derived Part has bodies from Single Layout, which can be added or deleted at any moment.
      I know this feature work in Autodesk Inventor simply. I am sure Solidworks somehow thought of this as well.
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      - Elmar Klammer @ Vald Mand on Dec 29, 2020 3:56 AM
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        Well there are several ways to do this...any of those can be used...all depends what works best for your workflow.
        
        Option0: Insert the complete master file into a new part. Use delete body feature with "keep option" and select the bodies you want to keep. Now you have exactly what you want. And after the fact added bodies in your master file won't show up in your derived ones. Since your delete body feature remembers the keep selection and deletes the rest.
        You will need to test it out. See if SW model updates throw a wrench.
        
        Option1: Well use configurations in your master file. Create a configuration for a given body composition or for each body. Then use insert part and specify the configuration. Now you can bring in as many bodies as you want.
        
        2018 SOLIDWORKS Help - Inserting a Part into Another Part
        change the configuration of the inserted part:
        Right-click the part and select List External Refs.
        Select a configuration in Configuration Name, and click OK.
        You can also control the configuration with a design table. See Base Parts in Configurations.
        
        Option2: Combine the bodies you want to export into a single body with some dummy geometry first. Make the feature simple so you can easily remove it in the derived part. Thin Extrude would work well in your given example.
        
        Option3: Use the save body command and add missing bodies with using option 1.
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Tim Rosendal Halvorsen Dec 29, 2020 4:01 AM
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Hi Vald

Not entirely sure why you are not making assemblies, or assemblies with virtual parts - but the way I'd go about something like this, would be by using the Insert Part feature.
I made a video showing this on your files, so this might help you or confuse you
Here it is: 2912202001 - YouTube

Tim
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Add body to "Insert to New Part"

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