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Mate connectors in Part Studio stay behind when I transform their owner part

chris_8chris_8 OS Professional Posts: 101 PRO
Am I missing a way to bind the part to the mate connector?

thanks,
Chris



Example:
https://cad.onshape.com/documents/6b714e18e39e7a82c583e9db/w/1b919740fcf6075f60128924/e/3e3023a32957b2f261920b77




Best Answers

  • philip_thomasphilip_thomas Posts: 1,056
    Accepted Answer
    Ok, so i had a go at this, and it is a perfect storm.

    Normally, a user would have at least one of the following;
    1) Access to the part feature history - this would enable you to put the mate connector at the center of the bottom face before cutting away the cylindrical opening.
    2) Two vertical faces that would allow you to use the 'between entities' option in the mate connector dialog.
    3) The ability to derive in a mate connector attached to a part

    In the absence of these, a sketch is the way to go.


    Philip Thomas - Onshape
  • chris_8chris_8 Posts: 101 PRO
    Accepted Answer
    I believe that if you hide the transform feature in your feature tree then that will hide the mate connector. 

    Owen S.
    I didn't even remotely consider that, but it works!
  • philip_thomasphilip_thomas Posts: 1,056
    Accepted Answer
    @chris_8 - YES, you are correct.

    'Between' enables you to position and orient a Mate Connector and then say 'but half way between this face and this one' :)
    (this is straight from the help - https://cad.onshape.com/help/Content/mateconnector.htm)


    Philip Thomas - Onshape

Answers

  • chris_8chris_8 OS Professional Posts: 101 PRO
    edited May 13
    Mate connectors don't bind to the part in the part studio but if you select the mate connector in the move feature it will move as well. 
    Thanks Bruce.  That works.   I realized there is an extra layer in my issue.  My example blocks were designed without all the features of the part studio that had sparked my question.  There was a sketch involved in my design, and the mate connector was attached to a midpoint on the sketch.  I had tried clicking on the sketch to have it moved as well, but it wouldn't get selected.   I didn't ever click on the mate connector itself until you mentioned it,  I think I had tunnel vision focusing on that sketch (see below). 

    Now I know how to move the mate connector.  Is it possible to move the sketch as well?

    https://cad.onshape.com/documents/6b714e18e39e7a82c583e9db/w/1b919740fcf6075f60128924/e/7fe629eee1ac35df8f394160


     


  • chris_8chris_8 OS Professional Posts: 101 PRO
    Now that I've cleaned up my Part Studio by including the mate connectors in the transform commands, those mate connectors can no longer be hidden.  Mate connectors that remained static can be hidden, but the ones that relocated are permanently visible it seems.
  • chris_8chris_8 OS Professional Posts: 101 PRO
    That's a bug, they should be able to be hidden. I'd report it with you feedback tool "?" top right.
    Done.  Have a great week
  • owen_sparksowen_sparks Member, Developers Posts: 1,468 PRO
    I believe that if you hide the transform feature in your feature tree then that will hide the mate connector. 

    Owen S.
    Production Engineer
    HWM-Water Ltd
  • philip_thomasphilip_thomas Member, Onshape Employees, Developers Posts: 1,056
    Accepted Answer
    Ok, so i had a go at this, and it is a perfect storm.

    Normally, a user would have at least one of the following;
    1) Access to the part feature history - this would enable you to put the mate connector at the center of the bottom face before cutting away the cylindrical opening.
    2) Two vertical faces that would allow you to use the 'between entities' option in the mate connector dialog.
    3) The ability to derive in a mate connector attached to a part

    In the absence of these, a sketch is the way to go.


    Philip Thomas - Onshape
  • chris_8chris_8 OS Professional Posts: 101 PRO
    Accepted Answer
    I believe that if you hide the transform feature in your feature tree then that will hide the mate connector. 

    Owen S.
    I didn't even remotely consider that, but it works!
  • chris_8chris_8 OS Professional Posts: 101 PRO
    Ok, so i had a go at this, and it is a perfect storm.

    Normally, a user would have at least one of the following;
    1) Access to the part feature history - this would enable you to put the mate connector at the center of the bottom face before cutting away the cylindrical opening.
    2) Two vertical faces that would allow you to use the 'between entities' option in the mate connector dialog.
    3) The ability to derive in a mate connector attached to a part

    In the absence of these, a sketch is the way to go.


    1) This was a Mcmaster part import, so you're right: there was no access to a feature tree.

    2) Honestly I didn't understand "Between entities" then.  I thought of entity as a body, but it can indicate 2 different faces from the same body?   That's good to know!
  • philip_thomasphilip_thomas Member, Onshape Employees, Developers Posts: 1,056
    Accepted Answer
    @chris_8 - YES, you are correct.

    'Between' enables you to position and orient a Mate Connector and then say 'but half way between this face and this one' :)
    (this is straight from the help - https://cad.onshape.com/help/Content/mateconnector.htm)


    Philip Thomas - Onshape
  • chris_8chris_8 OS Professional Posts: 101 PRO
    @chris_8 - YES, you are correct.

    'Between' enables you to position and orient a Mate Connector and then say 'but half way between this face and this one' :)
    (this is straight from the help - https://cad.onshape.com/help/Content/mateconnector.htm)


    I've been through that help before and I skirted around it because it didn't seem to work as I expected.  I didn't have a need for "between entities" at the time so I shrugged and moved on. 

    After working with it this evening I realize my issue was misinterpreting the "between entity" box.  I expected to be able to specify 2 things in the "origin entity" box, and then expected the mate connector to appear in between the two.  But I could only choose 1 entity.  I saw the "between entity" box and thought I don't need to click there because I already chose Between entities.   

    If entity 1 is an origin, I'd expect entity 2 to be a terminal or something.  Between is what I expect to happen between entity 1 and entity 2.  How does entity 2 get defined as between entity?

    I get easily tripped up be wording in OS sometimes.  I went off on a rant about 'derived' years ago once I finally figured out what it's really for.  I'd been searching through help for Copy part, or Insert Copied Part, or Duplicate Part to no avail.  It Derived me crazy :) 

    Now I know.  Thanks
  • owen_sparksowen_sparks Member, Developers Posts: 1,468 PRO
    I agree the between entities feature input dialogue is slightly counter-intuitive.  I was expecting to pick two points not a point an a face, however once understood I like it a lot. 

    In the example It's especially useful if you have some tolerance (slop from side to side) in the pin, so you don't want to mate a surface on one end of the pin to one side of the bracket.

    Cheers,

    Owen S.
    Production Engineer
    HWM-Water Ltd
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