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Completly lost with assemblies....

paul_breedpaul_breed Member Posts: 16
I've shared a drawing Tank end cap assembly.
It has an assembly drawing with some parts... they are all supposed to fit together in a cylindrical assembly.
All of these parts were made elsewhere and imported.
I'm trying to assemble them.


Go to tab Assembly 1 you will see the 5 parts....   


In the same document there is a tab (the very last one) called Complete Dome parts....
This has all the parts in the correct location...

When I click the mating selector it cant seem to find the center of any of the obviously round parts?

If Assembling by hand I'd put the oring on theTank Dome
Then I'd slide the  outer sealing ring over the  Tank Dome crushing the oring.
Then I'd slide this into the end of the carbon tube dome facing out.
Then I'd bond in the bond ring wide part facing the come.
Then I'd slide the whole thing so the bonding end is aligned with the end of the carbon tube.





Answers

  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    edited May 2015
    Paul

    The "obviously round" parts are imported from another modelling environment, rather than created natively in Onshape, so it's possible they may look perfectly round, but in fact not be. You could submit this model to Onshape Support for their diagnosis.

    I tried sketching a line on the Top plane of that Complete Dome parts model to represent the axis of the part, then making a second sketch to "Use" the edge of the chamfer surface. I then revolved this second sketch 180 degrees so that it was a representation of the imported surface. When you select the "Mate Connector" tool, this geometrically perfect surface lets you select the centrepoint of the outer arc, the inner arc, or the conical face (all of which lie on the same axis, but the resulting connector is slightly displaced along it, according to which entity you pick, due to the conical geometry).

    I had to select one of the existing parts to act as the "Owner Part" - I selected your Part 2.

    You can see the modified model in the Public folder, with the suffix "AT copy".

    I have to say that the graphics make it look as if the surface I created lies exactly superimposed on the imported surface of your Part 2, so I'm at a loss to explain your inability to assign a mate connector to the imported geometry. The error (if there is one- perhaps the scaling in X and Y is slightly different?) might be too small to see, though.
  • traveler_hauptmantraveler_hauptman Member, OS Professional, Mentor, Developers Posts: 419 PRO
    A link to make it easy to find: https://cad.onshape.com/documents/245758b5c5d64c0e8a694dca/w/7907f20bb37b495b8b5a76b1

    This is a great example for the Onshape guys to use to improve their mateconnector system.

    The import brought everything relative to the same origin so you could use that fact, but since 'complete dome parts' is assembled that way I'm assuming you are testing something else.

    Onshape does not recognize the curves as circlular so you'll have to add manual mate connectors to each part, perhaps also using sketches to help position the mate connector as you want.

  • paul_breedpaul_breed Member Posts: 16
    The parts were all drawn in Rhino. 
    I started by importing each part individually (as a parasolid) and trying to assemble them to understand assemblies in onshape.
    I failed to make a functional assembly so I then exported the the complete pre-assembled set so I had a put together correctly example to show what I was looking for.

  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    Is it possible the entities which look circular are actually defined in Rhino as B-splines? (apologies if this is an ignorant suggestion, I'm not familiar "under the hood" of Rhino)
  • paul_breedpaul_breed Member Posts: 16
    The parts were created as revolved solids so they should be round, under the hood I have no idea how they are represented. I'd really like to use OnShape for a new project, alas I find the drawing process almost impossible and was hoping to do my parts in rhino (a UI and process I understand) then do assemblies to share in on-shape. This was the first trivial test of that process.....

  • abefeldmanabefeldman Member Posts: 166 ✭✭✭
    @paul_breed - can you share this document with Onshape Support?  And can you please include the original Parasolid files you exported from Rhino?

    To share with support, select or open the Document in Onshape, click Share, and click the **Share with Onshape support** link in the bottom left of with window. Remember, you may revoke access at anytime by clicking "Unshare with Onshape support."
    Abe Feldman
    UX/PD/Community Support
  • paul_breedpaul_breed Member Posts: 16
    When you make the document public (as I did with this one) it seems to gray out the share with support button.
  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,763 PRO
    edited May 2015
    One needs to understand the differences between an analytical face and a parametric face. Looks like rhino prefers to make everything parametric faces which look flat but doesn't have what's needed to work in any other modeler. I would say it's best to stop using rhino for analytical shapes. It's a great surface modeler, so use it for that.

    Pick on the end face and try to create a sketch. Nope. You can create a sketch on a plane or an analytic face but not a parametric face. In your rhino model, the end faces aren't what you think they are. 

    OS could display the entity type that's selected and the you'll know what kind of face that's been selected. OS, also add sketch entity types. Many times I pick a straight curve thinking it's line when it's not.



    Some times you think you have an arc when it's a spline. Slicing a cylinder with an oblique plane use to create a spline but now it computes a conic. Its hard keeping up with these cad systems.


    OS please tell me what I've selected.



  • paul_breedpaul_breed Member Posts: 16
    I've tried to remake the same parts in OS directly and thats is now in the parts sheet of the included document...
    I did the parts in Rhino in less than 10 minutes, it took me 3 hours to battle the sketch tool into submission in OS.
    It wanted to help me with automatic snaps that were wrong 99.9% of the time.





  • emmett_weeksemmett_weeks Onshape Employees Posts: 26
    The inferences while sketching in Onshape are a bit on the thick side, so it can be hard to sketch in a cluttered area without picking up a snap to something. The shift key disables sketch inferencing which should help with densely packed sketches.
  • abefeldmanabefeldman Member Posts: 166 ✭✭✭
    edited May 2015
    @paul_breed  - if you own the document, you should always be able to click share and toggle the 'Share with Support' button.  You can also create a new document and upload the file again.
    Abe Feldman
    UX/PD/Community Support
  • paul_breedpaul_breed Member Posts: 16
    Abe, its a minor nit, but if you make the document public so anyone anywhere can see it the UI grays out the share with support.... button, ie support can see it because everyone can see it, so turnign on share with support would be redundant. 
  • jakeramsleyjakeramsley Member, Moderator, Onshape Employees, Developers Posts: 642
    Abe, its a minor nit, but if you make the document public so anyone anywhere can see it the UI grays out the share with support.... button, ie support can see it because everyone can see it, so turnign on share with support would be redundant. 
    Hi paul_breed,

    Can you post a screen shot of the share with support being grayed out?  I just looked at it on one of my documents and the share with support worked after making the document public.  
    Jake Ramsley

    Director of Quality Engineering & Release Manager              onshape.com
  • paul_breedpaul_breed Member Posts: 16
    I'm an idiot... the switch is gray and when I first tried to click on it nothing happened... I went and retried it and it does toggle even with  document public. My error...

  • abefeldmanabefeldman Member Posts: 166 ✭✭✭
    edited May 2015
    @paul_breed - Not a problem - glad to see you figured it out.  When a document is made public, it's view only, which means a user has to copy the workspace to make any changes or view the feature details in any of the part studios.  This also purges the workspace history, which is what the Support team is interested in seeing in your document.  With that, we can go back to where you first uploaded the models to determine if it's an Onshape issue you're running into.
    Abe Feldman
    UX/PD/Community Support
  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,763 PRO
    edited May 2015
    paul_breed- 

    It took me 10 hours to orient my first part inside Onshape. I still like it though.

    It's a good system and worth putting the time in to learn.

    I cut your cylinders creating new end faces hoping the parasolids kernel would substitute analytic faces for your parametric faces, didn't work though.


  • julian_lelandjulian_leland Member, OS Professional, Mentor Posts: 59 PRO
    +1 for some way of figuring out whether a given piece of geometry is a parametric/analytic face, line/curve/spline, etc.
  • andrew_troupandrew_troup Member, Mentor Posts: 1,584 ✭✭✭✭
    edited May 2015
    I don't know if Onshape Support have waved some magical fairy dust over my copy of  @paul_breed's ;;model, but I now find I *can* add a mate connector relative to the centre of the imported geometry. 

    Refer my model https://cad.onshape.com/documents/b0e53069f02f4e1a8965fd28/w/987cfcd365954908a3a94153/e/fc7319d98beb432088087dd9

    Under the tab "CompletedDome Parts", one mate connector is called "Mate connector wrt surface" and the other is called "Mate connector wrt imported ring"
    The former is created by hiding all parts except the 180 deg conical revolved surface, added by me as a workaround when the imported geometry was seeming not to "play nice"; the latter by hiding all parts except (imported) Part 2.
    Don't be misled by the fact that the owner part for both connectors is Part 2: this is a separate question from the geometry to which the mate connector acts as a reference.  (A surface cannot act as an owner part)

    It might simply be that the method for adding connectors is currently rather fussy, so that neither @paul_breed nor I succeeded first time round. I do find it much easier to attach connectors by resorting to RMB "Hide other parts" (equivalent to Solidworks "Isolate"): the connectors will reference only geometry which is visible.

    As far as a way of figuring out what is analytic geometry and what is not: I would expect to be able to attach a connector to the centrepoint of any curved geometry which, when selected, reported a radius or diameter in the measurement field at bottom right of the window (as Part 2 does)
  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 1,763 PRO
    edited May 2015
    Not sure what they did, but you can pick on flat faces and create sketches.

    It's interesting rhino uses half sections for cylinders. Typically this is the sign of an old geometric kernel. I'm not sure what rhino uses. Pro/e did this also and was based on the idea that an edge is made up of 2 surfaces. A cylinder with one edge would share the same surface which violates the idea that an edge is the intersection between 2 surfaces. This is why pro/e geometry creates 2 surfaces for their holes. If you've ever detailed pro/e geometry, holes were 2 arcs. This is the sign of an old kernel. I wonder if SW will begin showing this artifact now that they are switching to the catia kernel. 

    Creating sketches on flat faces is a SW trick. It's a fast way to determine what type of surface you're dealing with. I didn't come up with it, the guy who did curvy 101 at SW world brought this to my attention. I still use it as a technique to determine which surface type I'm dealing with.

    Yesterday I was filling in a trimmed boundary on a manifold which subsequently wouldn't allow a sketch features and created real problems down stream in my design. Redefining the trimming boundaries and fitting a planar surface in roughly the same place allowed a face that I could create sketch features and now the rest of the design will be easier. It is relevant and it does occur.

    I work with a lot of rhino geometry, especially t-spline geometry but can't remember if I've run into this problem before. I must say that the geometry I get from rhino isn't flat, far from flat.

    There are 2 surface types. They both look the same. But they are different. It's hard to tell which is which. Please beware it'll bite you.

    Andrew, the intersection of a cylinder (analytic surface) with a parametric face isn't a circle, therefore there is no center. It's interesting that most the stuff we do is prismatic with well behaving geometry. You know centers, normals and clean geometry, but it's not hard to step into the world of crazy geometry. Two cylinders intersecting, cylinder/cylinder intersect, whats the resulting edge? And then what can you do with it? What happens when you start importing and exporting this stuff. How come I can detail a pro/e part inside a SW drawing? I find this fascinating.

    One of these days I'm going to type up a post about "how stupid is a dumb solid". You'd be surprised at how much geometry is contained in a dumb solid. In fact, adding parametrics to a dumb solid is trivial.


This discussion has been closed.