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Completly lost with assemblies....
paul_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.
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.
0
This discussion has been closed.
Answers
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.
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.
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.
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."
UX/PD/Community Support
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.
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.
UX/PD/Community Support
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.
UX/PD/Community Support
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.
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)
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.