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Hard time figuring out how to use assemblies
nyholku
Member Posts: 58 PRO
I've checked some of the tutorials and experimented but I cannot really get my head around how use the assemblies.
I have a hard time even describe my difficulties!
Here is my current/specific problem.
I've modeled a group of parts in a part studio in correct relation to each other.
Now when I insert this into an assembly want to treat them as a one part.
So how should I go about this?
Should I just group them in the assembly?
That seems to work to some extent but then I need to create a linear pattern out of that one part (group) and this I cannot do.
To me it would make more sense to bring all the parts from that part studio into an assembly which I would then insert into
and other assembly making the first assembly a sub assembly in the second assembly where I could then move that whole subassembly as a whole.
But that does not seem to work, if I grab part that is part of the sub assembly, then only that part moves.
If I multiple select parts and try to move them in a group then weird movements happen when I rotate them and sometimes the rotate does not work at all (nothing happens).
I guess that a lot problems stem from the fact that in the subassembly the parts are not 'mated' together.
Ok, so I want to mate them with the 'fastened' mate ... but that requires specifying mate connectors for each of dozens of components ... why can't I just tell the system that fasten them (all six degrees of freedom) together, why does it matter which mate connector is used so why should I need to specify it.
Getting close to ranting now, sorry, trying to get back to the problem.
My problem is that when I design I want to sketch some group of parts.
By sketch I mean that I will later want to come back to that group of part and refine it by adding /removing parts or refining parts as my design evolves.
Then I want to create an other group of parts.
Next I want create a group of groups, creating a sort of logical hierarchical model of the system I'm building. Sometimes I want to create those groups of groups as linear patterns, sometimes I want to just drag them in place. Sometimes I need to add one group multiple times into an other group.
At this stage in the design I usually don't know the exact relationship (position/orientation) of different groups of parts (or group of groups) and I just want to drag them around because that is what I'm actually looking for ... how to best fit things together.
I realise above is incoherent and hard to follow but nevertheless I'm hoping for some kind of wisdom from the crowd.
To make this concrete (this is not my design case but something that illustrates the process).
Say you are designing a tank (of the armoured vehicle kind).
You do a quick extrusion to mock up a wheel.
Then you mock up swinging arm for a pair of wheels.
You assemble those together.
Then you assemble ten of those arm+2 x wheel combos into two rows to form the tank track support system.
Next you mock up the body.
Assemble the body and the track support system together.
And so on and so on.
You move things around to see what is best.
Then you want to go back to the wheel and start to add details there.
As your knowledge and understanding of the design grows you start adding mates and exact dimensions and so on.
And I can't figure out the correct approach in Onshape how to go about this....
I have a hard time even describe my difficulties!
Here is my current/specific problem.
I've modeled a group of parts in a part studio in correct relation to each other.
Now when I insert this into an assembly want to treat them as a one part.
So how should I go about this?
Should I just group them in the assembly?
That seems to work to some extent but then I need to create a linear pattern out of that one part (group) and this I cannot do.
To me it would make more sense to bring all the parts from that part studio into an assembly which I would then insert into
and other assembly making the first assembly a sub assembly in the second assembly where I could then move that whole subassembly as a whole.
But that does not seem to work, if I grab part that is part of the sub assembly, then only that part moves.
If I multiple select parts and try to move them in a group then weird movements happen when I rotate them and sometimes the rotate does not work at all (nothing happens).
I guess that a lot problems stem from the fact that in the subassembly the parts are not 'mated' together.
Ok, so I want to mate them with the 'fastened' mate ... but that requires specifying mate connectors for each of dozens of components ... why can't I just tell the system that fasten them (all six degrees of freedom) together, why does it matter which mate connector is used so why should I need to specify it.
Getting close to ranting now, sorry, trying to get back to the problem.
My problem is that when I design I want to sketch some group of parts.
By sketch I mean that I will later want to come back to that group of part and refine it by adding /removing parts or refining parts as my design evolves.
Then I want to create an other group of parts.
Next I want create a group of groups, creating a sort of logical hierarchical model of the system I'm building. Sometimes I want to create those groups of groups as linear patterns, sometimes I want to just drag them in place. Sometimes I need to add one group multiple times into an other group.
At this stage in the design I usually don't know the exact relationship (position/orientation) of different groups of parts (or group of groups) and I just want to drag them around because that is what I'm actually looking for ... how to best fit things together.
I realise above is incoherent and hard to follow but nevertheless I'm hoping for some kind of wisdom from the crowd.
To make this concrete (this is not my design case but something that illustrates the process).
Say you are designing a tank (of the armoured vehicle kind).
You do a quick extrusion to mock up a wheel.
Then you mock up swinging arm for a pair of wheels.
You assemble those together.
Then you assemble ten of those arm+2 x wheel combos into two rows to form the tank track support system.
Next you mock up the body.
Assemble the body and the track support system together.
And so on and so on.
You move things around to see what is best.
Then you want to go back to the wheel and start to add details there.
As your knowledge and understanding of the design grows you start adding mates and exact dimensions and so on.
And I can't figure out the correct approach in Onshape how to go about this....
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MBartlett21
Member, OS Professional, Developers Posts: 2,034 EDU
@kustaa_2
Try using group mat, rather than fastening all your parts, then insert into another assembly. It should work then5
Answers
Try using group mat, rather than fastening all your parts, then insert into another assembly. It should work then
IR for AS/NZS 1100
Thanks! That seems to work just the way I wanted it to!
HWM-Water Ltd
I created a minimal example.
It is here:
https://cad.onshape.com/documents/ef5fa2be0955b7d9fe6f5868/w/e8037923abd2bbfdf6a26439/e/669ceeaa4746ab22fbbbcc20
Basically I created a part and did assy 1 where I placed the part twice:
I then did assy 2 where I inserted assy 1 twice:
and the created assy 3 where I inserted assy 2 twice:
I then went back to assy 1 and dragged one of the components to change assy 1 to this:
but assy 2 and assy 3 do not reflect these changes, how can I update the assy 2 and assy 3 to reflect the changes I 've made?
If I change the parts in parts studio the changes are visible in assemblies just fine.
New parts created in part studio are not visible in the assemblies.
I guess I'm using this wrong and not as intended. I sort of get that
new parts are not in the assemblies cause I've not added them.
But this is not the way I want to work and the way my mind works
and I think I'm not alone so I guess I'm just missing something.
Think about car design. There is going to be four wheels, engine
and a body. You start with the engine. You know there is going
to be the block and intake and exhaust manifold but you don't
know the details.
So you mock them up with some boxes.
Then you create an engine assembly of those mockups so that you
can move them around.
Next you mockup a body and to be able to move the engine around
in the body you create an assembly in which you insert the engine
assembly and the body.
As the design progresses you know more about then engine
so you want to go back to the engine work for example on
the exhaust manifold that now comes in two parts.
So you make delete the mock up of exhaust manifold from the
the engine assembly and insert two new parts there and expect
that the all the assemblies that contain the engine assembly
directly or indirectly as a sub assembly of an assembly will
reflect that.
Would that not be a very natural work flow?
Surely Onshape supports something like this and
I'm just not getting it how to do it....
Hmmm ... after more experimenting it *almost' works as I would
expect. Part modifications and new parts are reflect in the
hierarchy of assemblies as I would expect. However, and this
is crucial, positions of inserted parts and assemblies are not
handled hierarchically, if I drag them around in a sub assembly
that is not reflected in the containing assembly.
Maybe this would work if I had everything mated but as in the
early design stages I have no idea (besides I'm working with
mockups or place holders) how the parts mate using them seems
like a drag. And when I replace the mockups with real parts
more work with the mates.
Please note, again I'm not trying to complain as I'm sure there
has to be a way to do something like what I've described.
AND there should be a tutorial video to explain this.
https://cad.onshape.com/documents/b3d9316bfae18de9a5749c0d/w/5cb104626a51ec8dfecaa71c/e/a040dd51c7c2d2524e9b7d07
I create four wheel, engine and a body.
I create a wheel assembly that inserted four times to an assembly with body and engine and used some mates and dragging to locate them as I wanted.
I then went back to wheel part studio a created a 'rim' for the wheel.
Problem 1:
When I went to wheel assembly and inserted it there I could not find a way to insert it automatically in the 'correct' place even though it was designed in the part studio 'in place' i.e. in correct position relative to the wheel.
Problems 2:
If you look at the four instances of the rim in the main assembly they are all over the place.
Not getting this....
HWM-Water Ltd
Try Using Fastened mate, rather than Planar.
Edit the planar mate and choose fastened in the dropdown
IR for AS/NZS 1100
Thanks, sounds like it might work.
But how do I do that? When I insert a part (wheel) to the wheel (any) assembly the system allows (forces) me to place it with the mouse so it ends up anywhere ... how do I just insert part to an assembly at the position it is in the part studio?
That would work (if I could just 'not move' them as insert them (see above) comment), but... what you suggest is bottoms up design, works fine when you are building a model that you more or less know what you are going to do.
However in a real design process I (and I think most everyone) work from top down AND bottom up alternately. So I need to be able to do some high level conceptual thinking then go add nitty gritty detail and then back to moving things around at higher level. Not to mention that at some point your realise that the wheel assembly is going to need subassemblies of its own (bearing assembly, brake calibers etc) and this I just can't get to work for me.
Ok, so I tried this. I removed all the mates from Wheel assembly and applied group mate.
So, the rims in relation to the wheels are ok, great, but the wheels are now all over the place.
So I go to the main assembly remove all mates, drag the wheels in the right place and apply a group mate to all.
That should the approach eh?
And I get:
Looks good.
Now back to wheel assembly to reposition the rim, I suppress the group mate, drag the rim to correct position, and the un-suppress the group mate:
But when I get back to Main assembly the rims have not moved to the new positions ....
HWM-Water Ltd
Thanks!
Ok, I see, great tip on how to keep parts in place. Essential stuff, how did I not see that!
I get the point about the mates ... how ever at early stages creating all those mates gets in the way of just sketching everything together so dragging would be preferable at that stage.
But I guess I could live with that if I could just get the changes propagated to all higher level assemblies.
However, Onshape assemblies are a total dumpsterfire, in my opinion.
- No assembly planes
- No assembly level sketches
- No import of subassembly planes
- Imported mate connectors not locked to geometry
- Reliance of mating components to other components (generally a bad practice to begin with)
No. Dragging components around and reorienting them in assemblies is incredibly useful for concepting and design, not having the ability to do this is a shortcoming.
Honestly, in their current state, I would say Onshape assemblies are borderline unusable.
At the end of this message, i am going to offer you a one-on-one session with myself (and probably the Assembly lead), to understand better the workflows that you would like to have as well as show you how other users are successfully using Onshape.
In the meantime, here are some short responses to your statements . . .
- No assembly planes
This was intentional - the universal mechanism for mating is the mate connector.
The main benefit being that 99% of the time only a single mate is needed between any two parts or sub-assemblies.
Did you know that you can snap Mate Connectors to the assembly origin in any of three default orientations (mimicking the default planes that you are looking for)?
- No assembly level sketches
I use assembly level sketches (with Mate Connectors!) all the time!
Select the 'Insert' dialog and switch the type to 'sketches' (the other options are parts and surfaces).
The sketches are completely associative to their Part Studio.
- No import of subassembly planes
If you are referring to imported data (such as Parasolid/Step), I don't think that most systems even output them.
Try round-tripping a part with planes from and back into SolidWorks, I don't believe that i have seen planes come back in.
If i have mis-interpreted your statement, I apologize.
- Imported mate connectors not locked to geometry
Not true -
Mate Connectors attached to parts, move with the parts.
Mate Connectors attached to sketches, move with the sketch.
Mate Connectors attached to the origin, well, they stay stuck to the origin.
Its not possible for Mate Connectors to become 'detached'
- Reliance of mating components to other components (generally a bad practice to begin with)
Usually when i see a comment like this, i ask if the poster has ever used a 'group mate' - 99% of the time this is what they are looking for.
Whenever a user wants to insert a number of components into an assembly and they do not move relative to one another (eg an imported stepper motor), then a single group mate is all that is needed.
Ben - my apologies if i have mis-interpreted any aspect of your statements. I would like you invite you to email me (pthomas@Onshape.com) with some suggested days/times, for us to spend an hour on a gotomeeting answering any questions you have and to hear about your desired workflows. My only ask is that you would post a followup here to give others insight into your 'new ninja-ness'
Parts from different studios, drawn at silly locations / orientations mated to a separate unrelated layout sketch not to each other:-
Owen S.
HWM-Water Ltd
Rather than in-line answer your in-line comments to my in-line answers, i am just going to throw a couple of things up here that might help you.
PLEASE DO TAKE ME UP ON MY OFFER!
You are a paying customer - let me help you
Ok, I have learnt a few things from your followup that will help form my answers.
- What if you want to mate, say, the origins of two subassemblies relative to each other with no parts touching?
Easy - drop both into the parent assembly, their origins are by default coincident.
At that point you can either;
'Fix' one part from each sub assembly or,
Fix one part and put a group mate around one part from each sub-assembly now they cannot go anywhere
- I'm talking about a sketch created within the assembly itself to be used for controlling the layout of inserted parts and subassemblies
Yes, our support for layout sketches in an assembly comes from our ability to insert Part Studio sketches in any assembly.
What most people do is open two browser tabs - one with the sketch being edited in the part studio and the other showing the assembly.
When the sketch is updated in one browser tab, the assembly automatically updates in the other. I am happy to show you this working.
- I inserted a mate connector to the origin of an assembly, then dumped that assembly into another assembly. When attempting to use that sub-assembly's mate connector to mate to the origin of the master assembly, the mate connector moved, the sub-assembly did not. The reason I did this to begin with was because when dumping the sub-assembly into the master assembly, there was no way at all to set its position (not even "fix") unless I wanted to mate some random part of the sub-assembly to the origin of the master assembly, which of course I did not.
There are some fundamental differences between SolidWorks assemblies and Onshape assemblies.
One of those differences is that ours are always 'flexible', in SolidWorks, you aren't nearly so lucky - BUT, it does mean that parts that are not 'fixed' (or otherwise constrained) cannot float away. If you set a SolidWorks assembly to 'flexible' and drop it into a higher level assembly, it would behave just as Onshape does.
The reason the mate connector moved and the parts did not (in your example) is that there was nothing defining the location of any one part relative to the origin (and mate connector).
An hour has passed since i started writing this and you have sparked 'vigorous debate' here in the office.
Two leading solutions have emerged that would enable you to work the way you want to.
1) The ability to include a mate connector in a group mate
2) The ability to allow an assembly mate connector to be owned by an arbitrary part
We need to run these (and the problem by UX to see what we can do.
The leading 'available now' solution is to add a sketch (eg a circle) to the assembly with the center mated (or fixed) to the origin. That sketch can now be included in the group mate. I will make an example for you and post the link here in a little bit.
- Only on very rare occasions have I used group mates, like when mating dozens of chassis stringers to the same plane (in SW). The reason I state that mating components to other components is bad practice because if your geometry changes, your assembly changes, which is often not desirable. Or what happens if you delete some of your geometry, where does your mate go? You also run the risk of "stack up" issues with multiple mates across multiple components where one mistake or change may have a drastic effect on the remainder of an assembly.
I am imagining that this problem exists in every cad system. If the size of the parts changes and you want the others to move to accommodate that change, then they need to be mated to one another. The benefit of Mate Connectors really shines here as you only need one mate between each pair of parts.
BEN _ PLEASE TAKE ME UP ON MY OFFER!!!
Happy to spend time with you after hours if need be.
Philip
Good stuff gents, love this kind of debate.
@andy_morris and @philip_thomas
(1) One thing that has become clear from this thread is that people are often unaware that you can drop things into an assembly in their native position / orientation by not clicking in the screen and instead just accepting the insert as soon as the part is selected from the list.
I only learned this indirectly (watching a webinar on something else and banging head on desk as this was demonstrated).
Please forgive me if this is now plastered all over the training / help files but I believe there could be a UI improvement to make this more obvious.
(2) Please could these 'vigorous debates' be shown as pay per view for pro-subscribers? I imagine it's a bit like the UFC (Mixed Martial Arts) crossed with a University debating club. Sounds entertaining.
Cheers,
Owen S.
HWM-Water Ltd
Twitter: @onshapetricks & @babart1977
Interesting, I like the concept of return to native position.
(i) Today we could do this by returning to the part studio and creating an explicit mate for each part plonked on the origin. We'd then be free to fasten this in our assembly to the assembly origin if we'd moved the part but later wanted to get back to default.
(ii) Going forward I'd like to see an origin mate (created for every part automatically behind the scenes) that we can toggle on or off in an assy.
(iii) A right click context sensitive option in the assembly "Return to native position" a bit like the existing "Move to origin" option might be good too.
Thoughts?
@kustaa_2 We seem to have hijacked your thread, sorry about that.
Cheers all,
Owen S.
HWM-Water Ltd
Twitter: @onshapetricks & @babart1977
@philip_thomas I'm a paying customer too
Yes - if you’re a pro (or standard - paying is what matters
I like this approach too. As this topic has devolved into a "wouldn't it be nice to have x/y/z" discussion I'd like to build on that.
Dummy parts can be really useful in assemblies. Especially for things like bounding boxes, mating points or even as surfaces for tangent mates to follow.
One thing that bugs me at the moment is the "show all / hide all" property. If you hide stuff to say set up a mate and then return to "show/all" then of course everything turns back on, including your dummy/helper parts.
I'd love a be able to nominate parts (via meta-data property) to be a helper/dummy parts or surfaces and be able to show/hide them as a group.
Does that make any sense?
Cheers,
Owen S.
HWM-Water Ltd
OK, was feeling a bit guilty about walking all over your thread so here is an example of how I would go about this task.
https://cad.onshape.com/documents/a885a7ce308602785bdae0fa/w/671ab048f6b854a8aceaa4e5/e/978140440a32dd91a221c21f
(1) First Up I've added some mates in the individual part studios so we can use them to place things precisely later. This is overkill for round parts as OS will infer the centre of circles all by itself, but I like explicit named mates, you'll see why later.
(2) I've added some variables to control where they are placed. Again, overkill, we could dimension within the sketch or use offsets in the mates but I like this method better. It's easier to see the values at a glance and easier to find them to make modifications later.
(3) Next we make a wheel sub assembly. We'll need the same thing four times so no point reinventing the wheel each time.
(4) Next we start our main assembly, by dropping in the parts, un-mated at this stage.
It's a good idea to fix the first part in place (right click > fix) so when we mate parts together OS knows which bit we want to move.
Next up we add some mates to join it all together.
I've used revolutes for the wheels as I want them to spin round, and a fixed "fastened" mate for the engine block.
Note the nice tidy feature tree as we've taken the time to name features and mate points.
Now if we modify say the wheel:
It'll carry through automatically to the sub assembly
And the main assembly:-
Hope some of that is of interest.
BTW if the mate connectors are getting in the way then the "k" key cycles them on and off and the "j" key does the same for the mate indicators.
Cheers,
Owen S
HWM-Water Ltd