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How to use mates in Part Studio?

robert_arminrobert_armin Member Posts: 10
edited August 2015 in Community Support

I'm trying to drill e.g. holes through multiple parts in assemblies. From reading the forum I have learnt that this is not possible for now. The recommendation I found was using PartStudios instead of Assemblies. 
Now, how to use Mates in PartStudios? I just found how to set mate connectors.


How do I connect the mates in part studios?  - or more general how to connect parts in PartStudios?



  • navnav Member Posts: 258 ✭✭✭✭
    edited August 2015
    Hi @robert_armin you can`t connect mates in Parts Studio (https://forum.onshape.com/discussion/1392/do-mate-connectors-serve-a-purpose-in-parts-studio-other-than#latest) there are two workflows at the moment, use the derive parts feature recently introduced by OS

    Or build all parts from the ground up in one part studio using constraints/Use command.
    Nicolas Ariza V.
    Indaer -- Aircraft Lifecycle Solutions
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    If parts don't need to move relative to each other, then Mates are actually a very inefficient workflow compared to what @nav is suggesting in his last sentence. This is true in other packages too, but they don't have all the extra enabling functionality offered by Onshape's Part Studios, most notably the "Group" mate, which permits bringing a bunch of parts into an assembly, maintaining (and in future, updating) their relative positions as defined in the PS.

    In Onshape, Mates are specialised for controlling parts which need relative motion, and this makes them extremely efficient compared to other modelling packages.
  • shashank_aaryashashank_aarya Member Posts: 265 ✭✭✭
    Many parts have complex geometry and they cannot be assembled with the help of their default mate connectors. Also many parts need to assemble at the reference outside their geometry such as planes, co-ordinate systems in other CAD tools. But we do not have datum planes, co-ordinates in assembly. For that reason there is a provision of mate connector creation in part studio where you an create the mate connectors at any position even with the help of sketch point. Same you can further use to assemble the part.
  • robert_arminrobert_armin Member Posts: 10

    Many thanks for the great hints. I'm impressed on how fast I get responses. :-)

    Indeed those parts do not need to move. So I looked up constraints as recommended. I used them already in my sketches. However, I did not find a way to apply constraints between multiple sketches within a PartStudio. As soon as I edit a sketch I cannot click the other parts for constraining.

    How can I apply constraints across multiple parts in a part studio?

  • Narayan_KNarayan_K Member Posts: 379 ✭✭✭
    You can't apply any assembly constraints in part studio..mate constraints are available only in assembly studio.
    To make assembly quick and eassy you can create mate connector in part studio.
    Any have there is no relative motions in part studio..so no need to apply constrain in part studio.if you have some parts not having any relative motion then you can constrain them in assembly studio.
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    edited August 2015
    @robert_armin asked:
    How can I apply constraints across multiple parts in a part studio?
    You can apply a constraint between a point or other entity in a sketch which you are editing, and any other sketch entity (provided the other sketch is toggled to "Show") by selecting the two entities in the display area, and choosing the constraint you want from the menu.
    The "other sketch entity" can be in any part within the same Studio.

    This is a great way to build parts in context with each other in Onshape.
  • robert_arminrobert_armin Member Posts: 10
    thanks your help. for simple sketches this works indeed. But as soon as I use extrudes and want to constraint the extruded part with something else it does not work anymore. I'm sure I'm missing something really basic here.

    A simple repro would be:
    1) I create 2 sketches, ich each sketch I create one rectangle.
    2) Now I extrude both rectangles to a cuboid. 
    3) Now I want to make sure the cubioids are constraint together at their extruded end. I do not get this working, it always throws an errror.

    How can I constraint the extruded part of sketch with another part/sketch/extrude in the same partstudio?

  • robert_arminrobert_armin Member Posts: 10
  • robert_arminrobert_armin Member Posts: 10
    in my case I want to connect the blue part and the grey part. The blue Part is and extrude from the left grey part. the right grey part is a copy. It would work with a transfrom but the parts would not be connected?
  • shashank_aaryashashank_aarya Member Posts: 265 ✭✭✭
    @robert_armin If you want to connect those parts with transform feature, you have to make sure about the correct distance between the two parts, then you can select "translate by XYZ" from transform tool. According to the view cube direction put that distance either in X, Y or Z. There are other options such as translate by distance, translate by line in which you can provide any direction or line other than the directions on view cube.
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    The concepts I think you are looking for are "end conditions" for an extrude, and "merge" or "boolean addition" to connect (If by connect you mean for two parts to join to become one).
    If you want the blue part to bridge between the grey parts, it's simply a matter of choosing "up to next" or "up to part" as the end condition for the blue extrude, and you can choose whether or not to Merge it with the adjacent part or parts.
  • viruviru Member, Developers Posts: 619 ✭✭✭✭
    @robert_armin , Refer below video to connect the parts in part studios with the help of transform by mate connector option.

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