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Mates and assembly solving

andy_morrisandy_morris Moderator, Onshape Employees Posts: 87
edited December 2014 in Using Onshape
We want to make the process of mating parts in assemblies in Onshape as simple and efficient as possible. That led us to implement the mate connectors in assemblies and give you the ability to change mate types very easily.

I'd like to get your feedback on mate solving when adding new mates: After you have selected two mate connectors for a mate we move the parts so their relative positions are solved, but we don't solve the whole assembly until you click 'OK' or the 'Solve' button.

How do you feel about this partial solve of assembly mates?
In your experience does this help you get your parts mated faster and more reliably?
Andy Morris / Head of Product Design / Onshape, Inc.
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Comments

  • fastwayjimfastwayjim Member, OS Professional, Mentor Posts: 219 PRO
    These questions deserved to be answered...

    I like the partial solve because it satisfies the "non-committal" side of my brain, but it could be a bit better. If part 1 and part 2 are being mated, and part 2 already belongs to a mated assembly, OS consistently moves part 2 during the partial solve. I would rather have OS move part 1 (which is typically floating out in space), so the partial solve would be a bit more like a final preview.

    It is more reliable for sure, as the mate connector concept is new, and I find myself toggling between revolute/cylinder a lot as I am trying to get the proper DOF's. The partial solve allows for that, and it is nice. The "animate DOF's" is an EXCELLENT feature. Really helpful!

    Like I've mentioned before, this mate connector concept is on it's way to becoming one of the most innovative new CAD things I've seen in a long time. Well, you know, except for the whole "cloud" thing of course.
  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,934 PRO
    edited December 2014
    Double click on mate connector to bring up dialogue. It would be good if you could do this from the assembly for part studio part connectors but defiantly in the part studio.

    I find i position a part, then want to offset it, only way to do this is with the mate connector. I would then right click on the part, switch to part studio, click on the connector to find it in the tree, then right click edit to bring up dialogue, then click on the move and type the offset. Long winded to get a simple offset. 

    Happy to use the connector for the offset just need better access to edit it. Initially was frustrated there was no offset mate but think I am over that now.
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,934 PRO
    I want to be able to have mate connectors auto snap, . Check out my fastners Doc, I made it public. I want to be able to insert a bolt,nut washer and snap the the mate connectors together by dragging and hovering. I also find I insert a part, click in the work space and forget to tick it off then move to the mate connectors to mate and the part disappears,  you lean to tick it off on insert after a couple goes. I love the mate connectors so quick once you get your head around them. I have alway struggled to complete a full bolt and washer arrangement in SW as you need some many mates, Onshape is heaps quicker. Also the search function on the part insert is awesome makes for a great toolbox .  
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • traveler_hauptmantraveler_hauptman Member, OS Professional, Mentor, Developers Posts: 419 PRO
    babart77 said:
    I want to be able to have mate connectors auto snap, . Check out my fastners Doc, I made it public. I want to be able to insert a bolt,nut washer and snap the the mate connectors together by dragging and hovering.
    I second this... I have to assume though that this has already been on the todo list and they just haven't gotten to it yet.
    babart77 said:
    I also find I insert a part, click in the work space and forget to tick it off then move to the mate connectors to mate and the part disappears,  you lean to tick it off on insert after a couple goes.
    I've gotten bitten by this as well. I while ago I filed a feature request for them to not start a new action (create feature/insert mate/etc) until the current dialog has been either ok'd or canceled. I don't remember the outcome.
    babart77 said:
    I love the mate connectors so quick once you get your head around them. I have alway struggled to complete a full bolt and washer arrangement in SW as you need some many mates, Onshape is heaps quicker. Also the search function on the part insert is awesome makes for a great toolbox .  
    SW has mate connectors. (Called mate references.... ). They autosnap and work great for screws and other parts with repetitive ways of mating. (In a solidworks part you can add them with Insert->Reference Geometry->Mate Reference. Try them out next time you are in SW!)
  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,934 PRO
    I do use the mate references in SW's but only really for bolts etc, dragging parts out of the toolbox and find they don't fully define parts, that might be me. I have set up a couple of parts but don't use them very often, had trouble getting them to work and did not persist with them.
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • raj_Onshaperaj_Onshape Onshape Employees Posts: 79
    These questions deserved to be answered...

    I like the partial solve because it satisfies the "non-committal" side of my brain, but it could be a bit better. If part 1 and part 2 are being mated, and part 2 already belongs to a mated assembly, OS consistently moves part 2 during the partial solve. I would rather have OS move part 1 (which is typically floating out in space), so the partial solve would be a bit more like a final preview.

    It is more reliable for sure, as the mate connector concept is new, and I find myself toggling between revolute/cylinder a lot as I am trying to get the proper DOF's. The partial solve allows for that, and it is nice. The "animate DOF's" is an EXCELLENT feature. Really helpful!

    Like I've mentioned before, this mate connector concept is on it's way to becoming one of the most innovative new CAD things I've seen in a long time. Well, you know, except for the whole "cloud" thing of course.

  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,313 PRO
    I've been using OS assemblies lately and I don't think you'll want to assemble that bolt stack up using mate connectors. If you look at a top level OS assembly and count the DOF's of your device, that's how many mate connectors you'll use. 

    Positioning sub-assemblies requires a mate connector if you want to control it's position with offsets. Therefore add to the DOF the number of sub-assy's and you'll have the total mate connector count.

    total mate connectors= assy DOF + sub assy's

    I really think what is gone is the mate hell that we all experienced in past parametric systems. A top level assembly shouldn't have more than 20 - 30 mate connectors which is totally manageable. I think building OS assy's using old parametric techniques is a wrong idea.




  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,934 PRO
    @bill I like the mate connectors for Bolt washer stacks. Checkout my public doc. https://cad.onshape.com/documents/516b1784884d4facbc4c0d74/w/8e947edb43904354bb16b3f2

    Only problem I have is there is no way to replace a bolt and pick up existing mate, however mate is that quick to do you don't need to worry too much.
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,313 PRO
    edited February 2015
    Bruce, if it doesn't move, why mate it? Try grouping and leave the mates for moving components.

    I'm positioning components, deleting the mate, then adding to a group. The bolt stack up should probably be grouped with the part it's fastening. At the end of the day, you'll have very few mate connectors.

    My assembly is going really well, it's clean, very easy to understand. I think it's the way forward. Much better than anything I've seen in the past.

    Having transformations between each component is crazy, who ever came up with such a wild idea?




  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,934 PRO
    edited February 2015
    Can't see any reason not to group a stack of bolt and washers. Two mates and done if they drop in the right locations, upto10 for the same thing in SW's. 
    In SW's I do built dummy sub assy's, drop in and explode to save mating time. But this is better.
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,313 PRO
    edited February 2015
    I wish I could share my assembly, I need to get permission. I would like to share some of my ideas with you on putting together a top level assembly. I've been working on it for the last couple of weeks and I think I have something that's working well. 

    I'm really trying to reduce mate count and come up with a strategy that minimizes the confusion. Mates in SW are crazy and difficult to follow.

    You're example, 4 bar linkage, I think I could do with 6 mate connectors and have the same motion you have using ~25 mates. Most assemblies motions are simpler than your example and really take advantage of grouping. 

    Your dummy SW assy is similar to the group idea if you fixed all components in that dummy assy. I've never seen this strategy used in SW. The grouping workflow in OS is painless and easy to manage. Not sure how your dummy SW assy stacks up to OS grouping, I'll have to give that some thought.  



  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,934 PRO
    @bill, all I was doing with this assy was trying to work out how best to mate hardware. In my mind the plates were not really a working linkage, just holes for mating various examples of fasteners I might use in my daily work. You are right in trying to reduce the mates, very hard to manage at the moment, hopefully onshape will improve mate management soon.

    Normally I would try to build parts up with complete set of fasteners attached in the top assy, this is useful for getting clearances/sizing, makes the assembly look visually finished off and needed to build the BOM on the drawings/parts manual's. Normally it time consuming and annoying in SW's I would quite often just do a concentric and face to face mate under the bolt head but you still have a loose parts have to come back later and lock down with a plane to plane parallel mate. I think some of these mating methods are much quicker and more robust.
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,313 PRO
    Well, if nothing moves, I'd do it with no mates. I'd probably position everything, group them, then delete all the mates. 

    That's my design intent, which is different than yours. I'm on a mission to omit all mates except the ones that really matter.

    FYI-grouping mated items throws an error with the mate connectors. As well, fixing mated items throws an error. In SW fixing items doesn't throw an error with mated items (I submitted that one and they fixed it). I submitted an OS fix-it ticket to stop throwing mate errors for fixed items. I'm wondering if grouped items should also be excluded from mate errors. I think so. Mates should error with other mates and not fixing or grouping.

    You can't nest groups (add a group to another group). Only components can be added to groups. Not sure if this is a bug.

    I still can't design in an assembly and have to dance around sub-assemblies & part studios. All this makes my head spin. I find having multiple OS sessions open in the browser is faster than dancing between document tabs.

    You can't merge 2 part studios which really makes working with downloaded geometry a real pain. I'm trying to consolidate tabs but can't.
  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,934 PRO
    bill said:
    Well, if nothing moves, I'd do it with no mates. I'd probably position everything, group them, then delete all the mates. 

    Why not just us a part studio ?

    bill said:

    You can't merge 2 part studios which really makes working with downloaded geometry a real pain. I'm trying to consolidate tabs but can't.
    Suppose this is a reason. Hopefully fixed soon.
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,313 PRO
    edited February 2015
    Why not just us a part studio ?
    Because you can't merge a downloaded bolt into a part studio.

    Suppose this is a reason. Hopefully fixed soon.
    Yeap it's turning out to be a real issue.


    Moving components in a part studio requires a transform which can only handle translations or rotations. Typically you need 2 since you can't mix rotations & translations. You have to know the distances & angles. SW allowed constraints when moving bodies inside a part file, not so in OS. Also OS remembers everything so your tree has all these transformations locked up in perpetuity. I was hoping for a delete transform but leave geometry option. Positioning bodies in a part studio is a real drag.

    Or, on second thought, why not have an option in the transformation dialog that logs the transaction to the feature tree or doesn't, maybe a "position only" option. I think most people won't want to log transformations into the feature tree.





  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,934 PRO
    Why use groups and not sub assy's?
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,313 PRO
    I struggled with that. Seems groups are easier and less tabs. I do have an extra sub assy to keep names contained. Try putting part studios into a top level assembly and watch how bad it gets, fast.



    -I think everyone agrees the part studio trees are un-manageable.

    -Put a part studio in an assy and it's tree is f'd-up.

    -Go up one more level and now we have something manageable.




    Bruce, I really think I could have done a better job at putting this together.

    Do you have a strategy for large assembly management? 



  • clem_1clem_1 Member Posts: 8
    I tell you what, I really miss the feature/sketch driven patterns in SW because of this.  Efficient and editable.
  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,313 PRO
    I agree Clem, for handling hardware, that's a real time saver.
  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,934 PRO
    bill said:

    Bruce, I really think I could have done a better job at putting this together.

    Do you have a strategy for large assembly management? 



    Not yet @bill, I still have to figure best way to tackle assemblies, I've got a lot of question marks in my head at the moment. I am kind of waiting for more improvements before launching to far into a major project on Onshape. I really want to see how the drawing package is going to work with BOM's, rightly or wrongly this will determine how I build my assemblies. I am also waiting for exploded view's, this may also have a impact on structure and mates used, eg. will explodes work on group mates? Onshape still has lots of detail/features missing from the assembly section but it's off too a great start, looking forward to things to come.

    Sounds like your on the right track with reducing mates and keeping things clean. Hopefully this will make it easier when coming back into a model to work out how it was created, less maintenance and problems. Although I am expecting Onshape to come up with good methods/features to manage mates rather than the user getting rid of them altogether because they are unmanageable.

    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
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