Import Kurt DX6 CAD file into Solidworks as an assembly file vs part file
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    Default Import Kurt DX6 CAD file into Solidworks as an assembly file vs part file

    Hey all.

    I'm new to using the Solidworks CAM portion of Solidworks. I am looking at importing a model of my DX6 vise to use in assembly layouts and simulations in CAM. I can only seem to find part files and not assembly files to download. I have tried downloading as a step file and saved the individual solid bodies. But I get an error when clicking "Create Assembly / browse button" in the window that opens to save the solid bodies.

    Kinda beating my head against the wall here. Can anyone offer any assistance?

    Thank you....

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    I seem to recall you can save a multi-body SLDPRT file as a SLDASM file. There won't be any mates between the parts, but you can then add them.

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    Depending upon the version of SW you're using STEP files can come in as an import and without a feature tree even when saved as a Solidworks part file. Try adding reference geometry (axis, planes, points, etc.) at the component level that you'll need and save the file. This may allow you to create an assembly. Don't know what you'll be doing with this but I'd have the assembly as only 2 parts, the base/back jaw, and the moving jaw. Keeps it simple and a smaller file size. Hope this helped someone.

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    Thanks to those who chimed in.

    It seems I was able to get it to work with a combination of things suggested.

    I downloaded it again as a part file then saved the solid bodies. Once saved as solid bodies I created an assembly from the part file. In the assembly screen I "floated" the moveable jaw and associated parts. Then I created new mates for these components as well as a distance mate for the movable jaw assembly.

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    Quote Originally Posted by motofish84 View Post
    Thanks to those who chimed in.

    It seems I was able to get it to work with a combination of things suggested.

    I downloaded it again as a part file then saved the solid bodies. Once saved as solid bodies I created an assembly from the part file. In the assembly screen I "floated" the moveable jaw and associated parts. Then I created new mates for these components as well as a distance mate for the movable jaw assembly.
    If you mate the jaws to the part, then modify the part, your vise assembly will change with it automatically. This can be especially valuable if you are collision checking against vises, fixtures, vise stops, or whatever. In essence this is how the reuse library works in NX and can be used standalone or with a machine simulation.

    Let the software do the work for you.

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    You can Import(open) STP files as an assembly into your assembly template file.

    Go to System Options -> Import -> File Format and change it to STEP/IGES/ACIS

    Then under the Options section on the same dialogue, set Import Multiple Bodies as Parts. This will pull it in as and assembly using your assembly file template. If you have the Import assembly as multi-body part, then it will pull it in a part file template which I believe is the default setting. I also check the Auto Import Diagnostics to help heal gaps and whatnot that seem to be common with STEP files and SW.

    Now just file open(or drag and drop into SW empty screen) your part and the new assembly file will be populated with all the parts as individual components.

    Now, you can choose to save each part individually as a part file external to the main assembly file. This is nice for a typical SW assembly workflow. I usually save the parts internal, that way there is only a single file for the whole assembly. You still get the same functionality.

    Also, be sure to Break the External links on your imported step file. It can keep you from making modifications to the new assembly.

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