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Why is the ability to use and mate to the planes used in part construction missing in Assemblies?

Machines from the small to the gigantic use planes for assembly.  "The Datum Reference Frame / Planes"  Yet in Onshape there are no planes that are usable for mating in Assemblies.  You would think that the Assembly would have planes similar to a Part Studio.  You would think that the construction planes used in a Part Studio would be able to be used in an Assembly.  Is this an oversight or is there some new paradigm that is hidden, or is this functionality going to shortly appear?

Thanks!  I switched back to Freemium from Pro because of this deficiency.

Answers

  • brian_bradybrian_brady Member, Developers Posts: 498 EDU
    I initially missed planes after switching from Creo, but have warmed to the use of Mate Connectors. You can add one, two, or three Mate Connectors to the origin and orient them such that the "local z-axis" of the connector points the direction you desire. Then you can mate any of you parts to these connectors and apply offsets if desired. I have found that I like to add Mate Connectors to parts in Part Studios at key points to make assembly cleaner and faster. These could coincide with the local origin and planes in the part or any other points on the part.

    I hope that helps.
  • bradley_saulnbradley_sauln Moderator, Onshape Employees, Developers Posts: 375
    Welcome to the world of Onshape and the advancements we've made to traditional CAD. As @brian_brady said you can now utilize higher order mate connectors. Here is some information on them: https://cad.onshape.com/help/#mateconnector.htm?Highlight=mate connectors
    Engineer | Adventurer | Tinkerer
    Twitter: @bradleysauln


  • rick_gibson_deerick_gibson_dee Member Posts: 3
    More info:  So you are in an assembly and you "Turn Section View On".  The pop up is... wait for it..." Select a Plane, Planar Face or Mate Connector".

    Where are the planes in Assemblies?  Why are they NOT there?  Why can't we use them along with all of the Mate Connectors?  Imagine the beauty of that scenario!  This is a very serious need for this software!  Let us not evade the question!
  • brian_bradybrian_brady Member, Developers Posts: 498 EDU
    I agree that it would be nice to add planes in an assembly for sectioning if nothing else. An "Add Plane" button like that in a Part Studio would be nice, with options to add standard planes (XY, YZ, ZX) or offset, point-plane, etc.
  • Gerard_at_RexGerard_at_Rex Member Posts: 1 PRO
    I vote to introduce plane options in Onshape assemblies. Engineers work with datum planes, which are missing in Onshape. Where to find a tutorial to show what has replaced using datum planes? I suggest to at least provide the option for designers to use planes in assemblies.
  • dirk_van_der_vaartdirk_van_der_vaart Member Posts: 150 ✭✭✭
    edited January 10
    Take a look at this simple document how to use a sketch and a mate connector in an Assembly to place an object in a wanted position.
    https://cad.onshape.com/documents/a75232e47655976955ac7b3d/w/ea82bd68fdfbadf588cd8123/e/7ba2f5c5952d15ab76f5e75c

  • john_mcclaryjohn_mcclary Member, Developers Posts: 3,415 PRO
    edited January 10
    Onshape does not compute the orgin of each assembly when you have sub assemblies. 

    That being said, if you keep that in mind, you can add a mate connector to the origin. A mate connector is a plane/axis/point all rolled into one. 

    If you want a traditional plane, create three surfaces or square sketches in a part studio, then derive that into any assembly and fix it. Mate everything of that.

    But honestly you should focus on practicing the 'proper Onshape techniques' rather than sticking to and out of date concept like 'three mates per part' or 'assembly planes' 

    In the end, it's the parts you're mating, not the assembly. Since all Onshape parts are free floating in higher assemblies, where other cad locks them down. Unless you check the 'flexable' option which even 1 intstace of can tank your model's performance in SW... 
  • S1monS1mon Member Posts: 348 PRO
    @john_mcclary

    I've been trying to unlearn my past experience and learn more of the Onshape way.

    There are some places where the avoidance of assembly planes at locking stuff to the origin gets you trouble:
    1. When you import/export assembly CAD it's relative to the origin. If this isn't locked down and understood, it will cause problems.
    2. Creating assembly cross-sections of organic shaped exterior parts is impossible without adding mate connectors or sketches. I've had stuff where there was literally nothing to pick until I added stuff.
    3. Inserting things (either from part studios or imports) at the default location doesn't lock anything down. You need to lock at least one part, and group the rest. To me floating by default when I import an assembly is one of the most shoot-yourself-in-the-foot stupid things that both Onshape and Solidworks do.

  • john_mcclaryjohn_mcclary Member, Developers Posts: 3,415 PRO
    Those are valid points. I have encountered some, even with cross sections of odd parts. 

    But i suppose I haven't seen it enough to be a problem, i can see that being an issue with organic designers on a daily basis. 
  • eric_pestyeric_pesty Member Posts: 23 PRO
    I was also unsettled by the lack of ref geometry (origins, planes, sketches) in assemblies but it does keep things neat and clean. My personal take on this is that it is worth simplifying and decluttering things, even if it needs a couple extra clicks once in a while. In the odd case where you have organic shapes with nothing to pick, it seems easy enough to create reference mate connector(s) in the part(s), or directly on the assembly origin (think of all the extra clicks and scrolling you save by not having to navigate the expanded tree to show hide planes and sketches!)

    I've had many times in SW when you open someone else's assy and there are random sketches and planes visible all over the place from various sub-components (because they had plane and sketches display off when they saved it and I didn't realize). I you are using PDM and these are read-only you are stuck having to individually show/hide stuff every time you open up that part/assy, I don't miss that!

    Mate connectors (compared to multiple low level mates) are another example of what I think are smart tradeoffs made in Onshape: they are significantly better 94% of the time, require a few extra steps 5% of the time and a pain in 1% of cases but definitely better overall.
  • S1monS1mon Member Posts: 348 PRO
    @eric_pesty

    I would largely agree with all of your points.

    I've spent a lot of time cleaning up other people's Solidworks models over the years so that planes and sketches are not all shown in assemblies. It's especially painful with master model driven work when someone adds a new sketch or plane to the master and forgets to hide it. Then all the driven parts would suddenly have extra clutter showing up. In drawings it doesn't matter if you have the top-level visibility of sketches turned off, if the individual sketches are shown, they screw up the bounding box which would often lead to views which were overlapping and impossible to manage. You've triggered my PTSD from this BS.

    The one thing that kills me in Onshape is the idea that if I lock down the location of parts in a subassembly with group mates, and the top level assembly can override that. It's so counter-intuitive, and I had a very hard time figuring it out in the first place, let alone the pain of dealing with it on an ongoing basis.
  • eric_pestyeric_pesty Member Posts: 23 PRO
    S1mon said:

    The one thing that kills me in Onshape is the idea that if I lock down the location of parts in a subassembly with group mates, and the top level assembly can override that. It's so counter-intuitive, and I had a very hard time figuring it out in the first place, let alone the pain of dealing with it on an ongoing basis.
    Yeah that takes some getting used to for sure... Although I find it is "logical" behavior considering the origin and planes are not part of the sub-assy.
    In this case Onshape doesn't try to assume what you want until you explicitly define some sort of relation between your sub-assemblies. I guess it might be nice to have the option to "propagate" any fixed relations upward when inserting (like an optional checkbox or something), but I can also see how that could backfire... 
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