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Boolean subtract problem with a Catia step file.

Discussion in 'Using Alibre Design' started by JohnRitson, Jan 29, 2020.

  1. JohnRitson

    JohnRitson Member

    I am receiving models from my customer that will not allow me to boolean subtract or cut a face to put in a tapped hole. I'm assured they are proper solids created in Catia but when I cut the part I can see through it as if it is only a skin. I have included on of the models I received. Is this a Alibre problem. Thanks in advance. John
     

    Attached Files:

  2. NateLiqGrav

    NateLiqGrav Alibre Super User

    Here is what I get when I do a Check of the part. Lots of duplicate Verticies.
    Try importing with Import Advisor and Check Part to see what Alibre suggests.
    Then import again with those settings.
    upload_2020-1-29_19-46-52.png
     
  3. Lew_Merrick

    Lew_Merrick Alibre Super User

    Hi John -- Make sure that your customer saved the Catia file as a solid rather than as series of Surface Elements -- that is something I run into with fair regularity. -- Lew
     
  4. W01FM4N

    W01FM4N Member

    It appears that the STEP file is a SHELL or a SOLID that had features that resulted in a NON-WATER-TIGHT entity. I've STEP files of SOLID PARTS created with CATIA import as a SHELL in CREO due to small features were the accuracy was insufficient to generate a solid at import, and vice-versa. Or, it was exported as surfaces, which is possible. Being a STEP file doesn't necessarily mean that it is a SOLID BODY.

    Applied an EXTRUDE CUT, but it appears to be a SHELL. A bit strange...
    upload_2020-1-29_19-9-53.png
     
  5. JohnRitson

    JohnRitson Member

    The suggestion to vary the import methods led me to changing some settings. The part was only one small part of a larger assembly and as I have had no problems with smaller imports I assumed the settings were good. Thanks for your help, I think I am OK now and will close the thread. Thanks again for your help this is a large weight off my shoulders. John
     
  6. bigseb

    bigseb Alibre Super User

    Catia is notorious for poor quality exports. As already mentioned you can do a 'check part' to see what's wrong but don't expect much beyond that.

    I ultimately imported stp's from Catia into Moi first and cleaned it up first. Then imported that into AD.
     
  7. idslk

    idslk Alibre Super User

    Hallo colleagues,
    you can make it with Alibre only...maybe not perfect, but...
    - I made a "raw material" block (bigger than the part) and saved it as Block1.
    - Then made a boolean subtract (Block1 - Part). (Result is a "hollow" block)
    - Saved that as eg. Block2.
    - Than made a Boolean subtract (Block1 - Block2) and then you get a solid of the Part.
    - Save it and work with it...
    Btw.: Doing only an intersect of Block1 and Part will result in only a surface of the Part...
    upload_2020-1-30_23-25-38.png
    Regards
    Stefan
     
    Last edited: Jan 30, 2020
    simonb65, bigseb and sz0k30 like this.
  8. sz0k30

    sz0k30 Senior Member

    Hey idslk,

    That's pretty slick!
     

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