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how to create a configuration that supresses a feature?

dave_franchinodave_franchino Member Posts: 5
Hey folks, Sorry - Solidworks user here and Configurations are really befuddling me.  I would like to simply create two configurations for a part (that's one part in a multi-part studio if that makes a difference). One configuration would have a couple of features supressed.  In this way I could show a drawing that featured two versions (think of an as-cast version of a part and then a part that has machined surfaces). Is there a video or a tutorial on configs that would address this? I'm sure I just have a conceptual block because I'm trying to think like Solidworks and it appears that configs are using a different strategy in Onshape. Perhaps it will have unique advantages but right now Onshape configs are just confusing me. Thanks for the help!

Comments

  • Axel_KollmenterAxel_Kollmenter Member Posts: 159 PRO
    edited May 20
    Hi Dave welcome to Onshape.

    first you have to generate a configuration


    Than you can right click on your feature and click Configure suppression.

    You will nor get the option to supress or unsupress the feature in your configs

    You can check the onshape learning center: https://learn.onshape.com/catalog?labels=["Learning Pathways"]&values=["Onshape Fundamentals"] there  your will find a lot of tutorials.
    Best regards,

    Axel Kollmenter
  • Axel_KollmenterAxel_Kollmenter Member Posts: 159 PRO
    It doesnt make a difference if it´s a multi-part studio

    Best regards,

    Axel Kollmenter
  • john_mcclaryjohn_mcclary Member, Developers Posts: 3,671 PRO
    edited May 21
    If you create a single 'list' configuration

    Then it is exactly like solidworks.



    Where Onshape differs is the ability to add multiple independent configurations (layers of configs if you want to think of it that way)

    They also offer 3 different types


    List is what you're used to.
    Checkbox is just a binary option (probably perfect for your current situation) name the config "machined" then set suppression that way.

    then there is Variable, which allows you to create parts on-the-fly in an assembly or another document whether or not the part config was made or not.
    Perfect for something like a bolt library, where you enter the length of the bolt in the variable.
    Or in a recent case I did, where all of the yellow hand rail was modeled only once and a length was chosen at the assembly level
    same with the toe-kick plates and the angle iron support structure weldments.



    The weldment was also configured to allow for adding / removing spacers evenly as well.


    Then it all came together at the drawing level to auto-generate where-used tables and cut-lists


    So, it would be worth your while to study all you can on Onshape's configuration system. It's very powerful and will make SolidWorks' configs look like a baby's toy.


  • chadstoltzfuschadstoltzfus Member, Developers Posts: 77 PRO
    The cool part about configuration variables is that you can use them the same way you would use any other variable, meaning you can put the configuration variable into a formula, or a conditional statement, or a custom feature, etc. We have built some fairly powerful configurations by combining the basics of configuration parameters with other aspects of Onshape. 
  • john_mcclaryjohn_mcclary Member, Developers Posts: 3,671 PRO
    The only real challenge to Config variables, and Configurations in general is the difficulty of capturing all of your configurations on drawings.

    When there are just a list of options, or booleans, you can find what you need.
    But when you have a variable config, you need to know every entry you made throughout the design.
    You can't just attach a part number as a configured property, since the Insert command only searches the default config, It's up to the detailer to fill in the configured variable precisely.
    If that variable is changed at the assembly, then the detail's config needs to be changed also.

    That's why I ended up using a chart drawing, to capture all of the random sizes spread across multiple weldments/assemblies.

    That won't always work, but in this case I "got away with it"
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