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IndustryArena Forum > CAD Software > Solidworks > Save Assy as solid
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  1. #1
    Join Date
    Feb 2007
    Posts
    40

    Save Assy as solid

    I need to send an assy to a customer but I don't want them to have all the models. Can I save the assy as a solid or something that will merge all the parts into one?

  2. #2
    Join Date
    Feb 2007
    Posts
    162
    Yes, the 'join' command works very well for this.

    I've used it many times for creating fixtures and nesting muliple single parts into a piece of stock.

    Use and follow the help file in Solidworks, it walks you through it step by step.


    Scott

  3. #3
    Join Date
    Aug 2006
    Posts
    231

    assembly as solid

    Are you talking about SolidWorks?

    If so do you mean saving as a part file? Solids and surfaces are "body" or entity types within the part enviroment. A part is a collection of bodies(solid and or surface). Assemblies are collections of part files.

    You cannot save anything as a "solid" You can however save things as parts which containg solids and or surfaces.

    Now to answer your question:

    You can save an assemble "as part" which will take all of the assembly files and create a part file with imported bodies.

    Now if you want to "merge all the parts to one":

    once you save an assmbly as a part file and you have all the parts now as solid bodies in one part file. Use the combine command under the feature manager to take all the seperate bodies and merge them to one. However.....and I will cover what I am about to say in the next paragraphs. If you send them that file they can still roll the feature tree back and "uncombine" the bodies and regain access to the sepertae bodies unless you.....after combining all of the bodies, save it as a parasolid or similar "dumb solid" file type which will whipe out any history in the feature tree thus becoming a "dumb solid".


    Reccomendations:
    I personally would not send a native SW to a customer unless thats what they were paying for. And never to a vendor. They have no need to know how I made something and have that much control over one of my designs. When I say native I mean something with the history. Like I said unless it is what was contracted or they absolutely need access to the history in the feature tree I do not send native. Otherwise I do one of two things:





    1) if they need an actual model I save as parasolid(there are other formats but SW platform and most other prefer this format). it is readable by alot of softwares fairly stable and is manipulatable as a "dumb solid" meaning that the geometry is there to manipulate but they do not have access to how you created it origionally to that point anyway. Plus this avoids issues with version conflicts. SW and similar parametric modellers are not backwards compatable. You can merge your bodies and save it as a parasolid and it will stay merged without the history there to break it back apart.

    2) if I am just having a rapid prototype I send and STL file. It is all they need and they have no way to manipulate the geometry. I heard, however, there are programs out ther to extract it out of STL but it will never be the same as the virgin goemetry before STL facets it all up.

    3)If the vendor or customer just needs to see the part and take some general dimensions I use edrawings which is part odf SW. This allows the your parts or assemblies to be viewed, measured and for them to make mark ups for requested chenges etc. without them ever hactually having accesss to a geometrically manipulatable file of any sort. This may be what you want to do as it seems you have a concern over theem seeing what the core parts are. You can combine and save in this manner as well.

  4. #4
    Join Date
    Feb 2007
    Posts
    162
    right...

    ...and I should have added if you decide to use the join feature to create a part file from an assembly file, you should save the newly created part file as a iges, parasolid, step, or whatever file. Otherwise Soildworks will complain that it can't locate the orginal part files and assembly when it tries to rebuild the joined parts/models.

    enat

  5. #5
    Join Date
    Jan 2004
    Posts
    3154
    AFAIK
    You don't want to join or merge your assembly just to send them something to look at.

    Option 1 (my preferred method)
    Send them an EDRAWING.

    Option 2 If they really need native SW file.
    With the assembly open click save as.
    Change the file type type to SLDPRT
    select other necessary options.
    Now your assembly is a simple part with no innards.
    sweet.
    www.integratedmechanical.ca

  6. #6
    Join Date
    Dec 2007
    Posts
    617
    You cann save an assembly as a part. File, save as .prt.
    Voila, works very well.

    regards

  7. #7
    Join Date
    Feb 2007
    Posts
    162
    Thanks DareBee, I don't think I've used that before, I've always used Edrawings. I saved the assembly I was currently working on and it crashed SWX 2007, but it saved the assembly as a part file okay. The cause could have been because one of my parts had 3 configurations and I was only using one of them. ....doesn't matter, it worked well.

    I do use the join command in assemblies whenever I need to position an odd shaped part onto a fixture or a group of fixtures, very handy.

    The combine command, AFAIK, is used in a part file for combining bodys.

    (rhetorical question) Why send a client an assemby with some of the parts missing? ....search me. I send everything, saves me the trouble of looking for models requested later. Now if it's a proprietary part or if it's an issue of security, then the user needs to contact the correct person for info and not a public forum.

    Scott

  8. #8
    Join Date
    Jan 2004
    Posts
    3154
    Quote Originally Posted by pixburghenat View Post
    (rhetorical question) Why send a client an assemby with some of the parts missing? ....search me. I send everything, saves me the trouble of looking for models requested later. Now if it's a proprietary part or if it's an issue of security, then the user needs to contact the correct person for info and not a public forum.

    Scott
    That's not rhetorical (especially on this forum) :wave:
    When you are working on designing equipment for a customer, it can take a lot of back-and-forth to tweak a design to suit manufacturing/kaizen requirements.
    Usually inside unseen components are not relative in this case. Emailing 40Mb files doesn't work. And a part of the same assemble would be, maybe, 1mb.
    www.integratedmechanical.ca

  9. #9
    Join Date
    Feb 2007
    Posts
    40
    I have tried the save as part and don't like it. I still haven't done the join yet.

    I am a machine builder. We are just getting started with Solidworks. One of our customers is asking for Solidworks drawings to use in the plant layout. All they really need is overall stuff but they asked for the model. I don't want to give them everything about my machine. But if I could save everything as a solid part with no features then maybe that would be fine. I just don't want to send out the model and find a copy of my machine coming back from China in a year.

  10. #10
    Join Date
    Jan 2004
    Posts
    3154
    I have had good experiences saving assemblies as parts for your exact application, but it has been years since I did it last.
    Another option is to export and then import.
    Export the assembly as parasolid or step or....
    Then import it again.
    You will have featureless (dumb) part assembly (depending on your settings (again, been awhile since I have done this).
    www.integratedmechanical.ca

  11. #11
    Join Date
    Dec 2007
    Posts
    617
    CharlesM479
    Specifically what don't you like about saving as part?

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