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How to Mate motor to mounting plate (compounded mates?)?

florian_fordflorian_ford Member Posts: 54 ✭✭
edited July 2016 in Community Support
Hello, I have some difficulty getting along with mates and with the Triad in assemblies.

For one I can't seem to use the Triad to rotate by exact angle so I couldn't rotate the motor 45 degrees with respect to some face (a mate that locks relative angle would help)

Second I am trying to Mate the holes of the motor face with the mounting plate and rotating the motor 45deg as a consequence of this mating:
 - I tried a Revolute mate between one of the 4 mounting holes and its corresponding hole on the mounting place. This worked as expected and now I can rotate the motor around that revolute mate.
 - next I tried adding one more mate (I think I have tried all) so that I could mate another hole of the motor or its shaft with its corresponding hole on the mounting plate to no avail. It always resets the Revolute mate and snaps the whole motor in another place.

How can I mate 2 holes of one Part with two holes of a mounting plate and have both mates work? I find it logical that if I have a Revolute mate on one hole I could do a fastened mate between the other two holes and it will rotate around the first mate until it satisfies the second condition.

How can this be done in OnShape?

Thanks. 

Answers

  • florian_fordflorian_ford Member Posts: 54 ✭✭
    Ok, here I am again answering my own question. Partially at least.

    So I was able to create a fastened mate and then expand the Mate Feature and right click > Edit to edit the Mate Connector. In that dialog I have a Realign and a Move options. The Move option permits me to rotate by an angle around the original position the motor was fastened to the plate. I had to eyeball and then adjust from top view until the other holes were concentric.
  • malay_kumarmalay_kumar Onshape Employees, Developers Posts: 84
    I am not sure what your model is like but I think you can create all of them as revolute mates and all holes will be aligned. You effectively will have a fastened mate between those two parts. Also while you are adding mates you will have to hit solve button to get all mates solved and see final solved positions.
  • florian_fordflorian_ford Member Posts: 54 ✭✭
    It didn't work for me. The part always reset its position to accommodate the new revolute mate as if it was the first mate to be applied. I don't have a lot of experience with mates so I gave up pretty easily in search for a workaround.
  • malay_kumarmalay_kumar Onshape Employees, Developers Posts: 84
    While in mate dialog we only solve one mate being edited but you can press 'Solve' button to see final solved positions. It will also do full solve when you accept the mate edits. Did you try pressing 'Solve' button. If it doesn't work then please make the model/example public if you can and share the model link and one of community member can help. You can also contact support through feedback tool.
  • florian_fordflorian_ford Member Posts: 54 ✭✭
    I tried again wasn't sure if I did it before but yes, I remember doing it. So it's like I say:
    1) create revolute mate motor mounting hole to mounting plate hole; test rotation;
    2) create revolute mate between another motor mounting hole to another (its corresponding) mounting plate hole;

    Motor Part used in the mating jumps to accommodate the last revolute mate and position resets for the first Revolute mate (it jumps to an 90 degree angle from the way it was before); I press solve => all other motor parts follow the new position. First Revolute mate is left hanging and I get complain about over constraining ("overdefined")

    My Onshape evaluation project is at: https://goo.gl/piW6rh 
  • colemancoleman OS Professional Posts: 244 PRO
    edited February 2016
    @malay_kumar
    I will agree there is confusion with instances like the one mentioned above.  
    While I use two revolute mates to solve the problem....it seems there should be a better way.  After all, a revolute mate is designed for revolving motion.  It seems counter-intuitive to add two revolute mates that constrain each other to solve the issue of fixing objects that are outside of 90, 180, 270 & 0 degrees of rotation. 

    Maybe I am missing something but I think that is how it works.  
    Would one revolute mate + 1 fastened mate work?  If I remember correctly it doesn't.  

    In what ways can this common mating condition be improved?  Should the fastened mate be limited to 90 degree increments of rotation? 
  • florian_fordflorian_ford Member Posts: 54 ✭✭
    It's quite logical to me if it was permitted. It's using a feature that already exists (mates) and it works just like in real life. I would first fasten one corner of the motor and then rotate it with the screw in place until it grabs so that I fasten the second motor corner to its plate, and so on.

    If only this mate would work as expected, compounding mates and resolving all prior mates before the next ones. If I create a revolute mate on one corner, all subsequent mates should search for a position that is permitted by the first revolute mate, that is, they are on the circumference circle defined by the centerpoint at first revolute mate that I've created.
  • florian_fordflorian_ford Member Posts: 54 ✭✭
    edited February 2016
    Ok, first I want to appologize for this long post that will follow.

    I managed to do it the following way:

    1) created the revolute mate between one hole on the motor front plate and one of the mounting bracket holes in the CoffeCore tab=> motor is placed accordingly and its position is reset from the arbitrary angle I turned it to a parallel position to some axis (or to its original position, I don't have any idea what is this position)

    2) Measured on the Sketch of the mounting bracket the angle of one of the holes (that i want to rotate to) to the horizontal axis:


    3) Expand the Revolute Mate Connector and Edit the Motor side connector (Right Click > Edit);

    I measured the diagonally opposed hole to the revolute-mated one so I will try 45+14.343 ...


    Spot on.

    Note: I get the red complain because I did the Reset while still in the Edit Mate dialog (it somehow looses Origin in the process). The correct OS procedure would be to click the green check and then do the Right Click > Reset. But it would be better to be able to do this with the dialog open, as long as there is no Solve button in this one.

    I did undo and did it the expected way and now i get it right:


    ------------------------------------------------------------------------------------------------------------------------------------

    Several observations IMHO:

    1) I would like to be able to "Rotate about Z" right in the viewport and have the X deg appear dynamically in the "Rotate about Z" field.

    2) I am able to select another possible mate from the ones that appear under the cursor and rotate the Part around the revolute mate previously created. It would be awesome if the Mate i've selected would snap, on it's trajectory constrained by the first revolute, to other mate points it finds on its way, thus making the rotation a powerful direct editing feature, so I don't have to know the exact angle by which to rotate:

     

  • malay_kumarmalay_kumar Onshape Employees, Developers Posts: 84

    Maybe I am missing something but I think that is how it works.  
    Would one revolute mate + 1 fastened mate work?  If I remember correctly it doesn't.  

    In what ways can this common mating condition be improved?  Should the fastened mate be limited to 90 degree increments of rotation? 
    One revolute mate + 1 fastened mate would work if the mate connector line up. The problem is that the implicit mate connector that one create may not align from two holes. We understand the pain point here and we are looking into making this workflow better. For now I think two revolute is the best solution or creating exact mate connector and have just one fastened that aligns both/all holes.  We could also solve all mates of two involved parts even when we are not doing full solve (doing mate edit). 

    We could also come up with workflows that lets a user align multiple holes and then create one fastened mate at the end. Another feature that could help is to convert a revolute to fastened at current mate value.

    Please keep the feedback coming. It is very helpful to know pain points. This is one area we can surly improve experience.
  • malay_kumarmalay_kumar Onshape Employees, Developers Posts: 84
    It's quite logical to me if it was permitted. It's using a feature that already exists (mates) and it works just like in real life. I would first fasten one corner of the motor and then rotate it with the screw in place until it grabs so that I fasten the second motor corner to its plate, and so on.
    If we create one real fastened (weld) then we won't be able to rotate so I think you meant revolute. We can call it anything but for onshape mating scheme it will be a revolute mate.

    If only this mate would work as expected, compounding mates and resolving all prior mates before the next ones. If I create a revolute mate on one corner, all subsequent mates should search for a position that is permitted by the first revolute mate, that is, they are on the circumference circle defined by the centerpoint at first revolute mate that I've created.
    Thanks for providing the example. Two revolute should work. My guess is those two holes may not be perfectly aligned. We will look into that. We can also look into tolerating issue if any. If they are perfectly aligned  (within our constraint solver tolerance) then I would expect them to work with multiple revolutes. We also need to work on more feedback as what is solved and why it is not working.  Again thanks for detailed description and example.



     

  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 3,356
    edited February 2016
    This type of mate has always been a problem for 3D CAD and it's usually a tolerance issue related to the distance between the holes. SolidWorks 2017, out in October this year, will be able to do this type of mate. That's release #25 of a 21 year old, $4000 CAD system.

    Best way to get this to work is to create the mate connector in the part studio. Create a sketch on the face of the plate and add a line constrained to the centers of two of the side holes (not diagonal holes). Then create a mate connector at the center of one of the holes, aligning the secondary axis to the line. Now you have something to mate to. 
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