Planes in Assembly

dan_schwartz

Hello
Is it possible to show the planes in assembly?
I want to make mate between planes, like in Solidworks.
Regards

owen_sparks

Hi, no planes in OS assemblies, we tend to mate on or between entities.

Shout if it doesn't make sense.

Cheers,

Owen S.

MBartlett21

dan_schwartz said:

Hello
Is it possible to show the planes in assembly?
I want to make mate between planes, like in Solidworks.
Regards

@dan_schwartz

You can mate to the origin, if that is what you're wanting

philip_thomas

I will be doing a webinar on this in a couple of weeks - hasn't been announced yet, but watch your email

billy2

Be careful mating to the origin in the assembly. What's not obvious, when moving this assembly into a higher assembly, mates to the origin don't transfer up and everything becomes unstable. There's no red flags. Once an assembly is in the higher level, check to make sure mates transferred properly. Look in the mate features folder, watch for mates to origin which can only be detected by editing the mate feature and looking for 'mate to origin'. 'mate to origin' will be in lower assembly but is missing in the higher assembly.

What would be nice is to have a chart of those things that move up to the next assembly and those that don't.

move up:
groups
mate connectors
mates

don't move up:
mates to origins
fixes (thanks @brucebartlett )

I don't have a good listing, Philip seems to have it all worked out in his head and has been repeating them to me.

Assembling by coordinates is a standard design pattern in use with all other parametric modelers. I think we all use them, but they're not in OS. There are other ways to put things together. 

One pattern that seems to be working well, and Philip showed me, is to use mate connectors defined in part studios. A mate connector can be anywhere yet owned by any solid body. These seem to move up the assy structure nicely. My problem was that I needed to assemble to something that wasn't selectable. Using a mate connector at the part level allowed the selection needed. This might be a substitution for assembly by coordinates. I think this is @owen_sparks suggestion and it's working for me.


It's hard to explain and some good examples are needed badly, looking forward to the webcast.

brucebartlett

Dan, to mate a part between 2 faces you can use create a mate connector in your assembly with the between option. A little more complicated to start with than using planes but once you get the hang of Onshape mate they are heaps more efficient. 


@billy2 fixes also don't move up.

My general rule for stable assemblies is only ever use 1 fix or 1 mate to origin per assembly. I will generally use fixes rather that mate to origin as the fixes are easy to visually see and alarm bells go off for me if an assembly has multiple fixes. 

Also, I try only ever use group mates in the first level of the assembly. If you use group mates over multiple levels conflicts can arise causing the assembly to have parts out of position. 

larry_hawes

philip_thomas said:

I will be doing a webinar on this in a couple of weeks - hasn't been announced yet, but watch your email

Really curious as to what "this" you are referring to? Showing planes in assemblies? Mates to the origin? Mates in general? The webinars are very long and tedious and really would like to know what topics/features will be covered.

Thanks

philip_thomas

Dan - in the meantime, please checkout this Technical Briefing (its really good ) . . . 

https://learn.onshape.com/learn/article/mating-basics

One point about things 'floating away in space' - I only hear this about 10 times a day.
Here is the reason - "A 'fix' only applies to the level of assembly in which the fix is applied".
This means that if you insert this (now) sub-assembly into a parent one, those parts that were 'fixed' in the sub-assembly are now floating.
As a general rule - there should only be ONE fix in any level of assembly - usually this holds a main component on the origin.
EVERYTHING ELSE RELATED TO ITS POSITION IN SPACE (but not to another component) should be a GROUP mate.

Workflow for an imported assembly with multiple parts in a single part studio.

1) insert part studio into assembly.
2) apply group mate to all inserted parts
3) apply fix to ONE part

That's it - you're done and it always works - 3 simple steps. You may now insert this assembly into a parent one with impunity - none of the parts will move relative to one another. The entire assembly can float around (because the 'fix' only applies at the level of assembly to which it was applied) - you can now mate the assembly with ONE mate or fix ONE part.  

I hope this helps

Webinar will be announced soon

philip_thomas

Larry  - the title of the webinar will be 'Onshape assemblies for SolidWorks users' and will cover the scenarios that users of traditional cad are running into when trying to learn Onshape. We left SolidWorks to build a better cad system - we've just done a 'less than awesome' job of making those new and more efficient workflows discoverable. We are working on it

robert_morris

@brucebartlett
Those are my general assembly rules as well. One 'Fix' or origin mate per assembly level, and only use Group mates where absolutely necessary. Everything else gets properly mated.

I've had assemblies not update correctly to part changes because a Group mate was used somewhere which caused some confusion for awhile, so I stay away from them as much as possible.

philip_thomas

@robert_morris - just to be clear, i am advocating using group as being preferable to individual mates for multiple parts being inserted into an assembly that do not move relative to one another.
When you say 'not update correctly', is there any example you can describe or point me to? (just trying to understand perspectives and use-cases).
Thank you.

billy2

@brucebartlett I tend to define groups: fixed, move1, move2 in almost every assy and then mate these groups together. Are you saying this can become disjointed?




How do you handle hardware? I'm dragging them into their own assembly to keep'm out of the tree. If I need to reposition them, I'll drag'm from the assy, move'm, and then put'm back. For things that aren't stable, I'll mate those to holes so when the design changes they update. But, when things are stable, I'll drag'm back to the assy. You can see the 2 bolts that are outside my assy. These are changing position as my design changes.


One thing I use all the time is the 'move to origin' after bringing in 1st component:


Once at the origin, I fix it. This is how I deal with first component in. Then it's moving things in/out of groups after that. I use a fastener mate to position components. Then when adding to group, it throws an error, I then delete the mate. I have fairly simple assemblies with hardly any mates.

To prevent having to use a mate and then deleting it, I've asked if 'move to origin' get upgraded to position any component to any other, and then all I have to do is add it to a group. Possibly the concept of mates is just a bad idea. Yeah, maybe we need a few.

I'm thinking an assembly is mostly groups and a few mates.




Can you post your tree and show me your structure?

robert_morris

@philip_thomas
I can't share the document that I had the issues in, and I've deleted the group mate after that anyway, but I'll see if I can make an example document later.

I'll try and describe what I saw.
I had a subassembly that consisted of a couple of manifold blocks with custom shaped seals between them and a long brass fitting attached to one block with an O-Ring on the end of the fitting. Everything was mated with fasten mates except for the custom seals. I used a group mate for the seals and one of the blocks since they were brought in from a single part studio. This subassembly was then added into a larger main assembly.

At a later date, I changed the length of the brass fitting. When I switched back to the main assembly, the O-Ring on the end of the fitting was no longer in the correct location even though it was mated with a fasten mate (it was still in its original position from before the length change). The only way to get the O-Ring to reset to the correct location was to suppress and usuppress the group mate. To be clear, the O-Ring and the brass fitting were not a part of the Group mate, but were in the same subassembly.

Also, if I remember right, the O-Ring was correctly located in the subassembly, but not in the main assembly. So I had:
Part studio 1 ( with blocks and seals )
Manifold Subassembly (with the group mated block and seals) <-- This one had the O-Ring in the correct position
Main Assembly <-- This one had the O-Ring in the wrong position.

It took a support ticket with Lou Gallo to help me figure out what the problem was.
After that, I've pretty much stopped using group mates and just taken a little extra time to mate things properly.

brucebartlett

@billy2 I rarely use the move to the origin or mate to the origin. I normally get stuff in position in my assembly based off the original part studio position and adding a fix.  

I personally think the mate to origin should follow up into higher assemblies, like a plane mate would in Solidworks but I am very happy that fixes don't move up this creates very nice workflows for floating assemblies and using the fixes as local controls after initial mating is done. 

You bring up a very good point, I am constantly using mates to position parts then deleting and adding a group mate. I think it would be really nice if you could position the ball on the triad on your geometry then invoke a way to drag and snap to position parts without having to add and delete mates. Is there an IR for this?

brucebartlett

@philip_thomas I am trying to recreate my group mate problem to prove why I try and keep my group mate to the lower level assemblies.  But I can't make it fail, this is either because this problem I have only seen after a couple 100hrs work but also they may have been further improved to stop the problems I was seeing from happing. 

Here's my test assemblies that seems to work fine with groups on groups. 

https://cad.onshape.com/documents/479fb6167f8c97471312996e/w/2736ced464ca56f21255a93f/e/d66f83905cae572f36a5717e

brucebartlett

Ahh..   I worked out my issue with to many group mate see the link in my last post. Problems arise in the group mates of upper-level assemblies when new parts are added in the group mates on the lower level. 

Group mates are awesome and I love using them but if you overuse them you get in trouble. My general rule is to keep them minimal and on the lower level assemblies, always look to edit an existing group mate rather than add a new one. However, if used carefully looks like they can be used on the upper levels successfully too.  

philip_thomas

BRUCE - you just gave me a good tip - group mate should only be used on parts in THIS assembly. 
I will go through your other scenarios in depth tomorrow (I am at a restaurant currently). 
This is all very timely as we are looking closely at the workflows with a view to improving them. 

billy2

@brucebartlett I think you're right and I'm fixated on the origin/planes and possibly this shouldn't matter. I need to abandon the old ways.

I'll try letting the part stay put and see where I end up.

As far as groups go, I tend to have a part assigned to a group, A part either moves or it doesn't. I'm not cross pollinating my groups with other groups. They seem to stay intact and maybe it's my simplistic usage of groups allowing it to work for me. My assemblies aren't that deep which might also help in my use case.


Thanks

brucebartlett

@billy2 we'll see what @philip_thomas comes up for best practices with group mates.

On the positioning of parts in assemblies, I find if I can lock/fixe the position to be the same as the part studio where possible and also model parts in the part studio's in position where possible, this makes it very easy to add new parts to the assemblies and the group mates.

Ideally, however if Onshape are looking at these workflows , it would be nice to somehow get the group of parts (subassemblies) automatically from the part studio with instances from the part studio without having to drop the parts in assemblies and modify group mates. 

robert_morris

@philip_thomas

I just tried to recreate my problem, and couldn't get the simple example to fail. I'm not sure if that's due to updates in Onshape or what.

I did look back at my support ticket, and was slightly wrong in my previous message. The assembly with the group mate (the main assembly) was the one that would not update part positions that were mated in the subassembly until the group was suppressed/unsuppressed.

I can message you the support ticket number that has all the details and screenshot if that helps you.

brucebartlett

I have replicated that exact problem in this assembly.  It happens when a out of original position part is added to the lower level group mate, and the upper level wants to hold the position it initially saw the part in, a simple suppress and un-suppress fixes this but can be dangerous if it goes unnoticed. 

https://cad.onshape.com/documents/479fb6167f8c97471312996e/w/2736ced464ca56f21255a93f/e/d66f83905cae572f36a5717e

robert_morris

@brucebartlett
Yes, that is what was happening to me except I only had a single group mate at the top level. I was told that the group mate was preventing downstream mates (in lower subassemblies) from updating at the top level. Suppressing/Unsuppressing fixed it.

robert_morris

Ok, I got it to fail.
https://cad.onshape.com/documents/70f3cbb4d5530e20ad68516b/w/08522aa5dce52f34914e687e/e/2f2889d0a18f9e7ab7976ac0

I have a subassembly and a main assembly. There is a group mate in the main assembly between the seal and the subassembly. When I changed the length of the fitting and added a plug to the subassembly, it is not updated in the main assembly. Suppressing/Unsuppressing the group will fix it.

billy2

@brucebartlett

Understanding the relationship between the partstudio & assembly is more complicated than in the past. I'm trying to keep it simple and the assembly moves things and instances things (make many copies). Most partstudios have assemblies that end up in the top assembly. Once this become stable, I'll move it to it's own document. I will establish a top document that pulls in the other documents. Right now my top is a folder (the project) containing multiple documents. I have established a few global documents.

My projects are fairly simple and not that deep so this easy approach is working.

The idea that newly added parts in a partstudio will appear in the correct position in the assembly, well, I gave up on that idea a long time ago.

billy2

I'm trying to recreate your grouping error. Can't say I've seen it.

Kevin_Snyder

The documentation isn't terribly clear but the group function (you'll notice it isn't actually called a mate and is separated from the mates in the toolbar) applies not only at the level that you create it but all sub-assembly levels for items in the group as well. It essentially overrides every sub-assembly mate at the level that you create the group. This is why sub-assemblies will update properly in their own tab but won't update at the top level. This is also why suppressing the group and allowing the sub-assembly mates to become active and unsuppressing it fixes the problem.

robert_morris

Yes, that is correct, and the way it was explained to me by Lou. It's essentially a "saved state" of where the parts are located at the moment in time you created the group and those positions are not updated until you suppress the group.

To me personally, that is a flaw or deficiency. It's just a group of "things", it shouldn't matter if that thing is a single part, a subassembly, or another group.
I shouldn't need to think about where those "things" come from first before grouping them together just because of how the software works under the hood.

In other programs, I can just group things and move on without worrying about it. That's what I want to do in Onshape.
Alternatively, the software shouldn't allow me to group things that could cause breakage later that might not be noticed.

brucebartlett

robert_morris said:

In other programs, I can just group things and move on without worrying about it. That's what I want to do in Onshape.
Alternatively, the software shouldn't allow me to group things that could cause breakage later that might not be noticed.

Or, if there is a problem with parts being out of position to the lower sub assy's an error should show. 

philip_thomas

@billy2 - We are still working on making this better for everyone, but hopefully i can demystify some stuff for you.

• Part Studios are where you make A PART.
• If a second part is directly geometrically related to the first, then its ok to build in the same part studio
• Part studios are not assemblies;
•        There is no motion
•        There is no instancing
•        They are not a 'sub assembly' (inserting the contents of a part studio into an assembly is not parametric (adding a part to a part studio will not cause it to appear in the assembly - being able to add the contents of entire part studio is a convenience)

@Kevin_Snyder is totally right

@brucebartlett - that is an excellent enhancement request - in fact, please submit it as a bug!

This is an excellent thread and you are all giving me excellent material for the upcoming webinar
"Onshape assemblies for SolidWorks users"

billy2

@philip_thomas I remember your demystification tip from our last conversation.

I'm just trying to figure out how to use OS to design products. I'm not sure it's clear how to structure a project in OS that'll handle all the requirements for developing a great product.

Possibly after your "Onshape assemblies for SolidWorks users", you can share with us one of your successful projects and detail out your structures you used to create a great product using OS?

philip_thomas

billy2 (Sort of begs the question, 'what fate befell Billy1?') - I want to help you.
Would you spend an hour with me over a GoToMeeting so that you can show me what you feel is the natural, discoverable path in Onshape?
Clearly we are doing something 'sub optimal' if users are not getting the optimized workflows that we believe exist ("its us, not you")

my email is pthomas@onshape - just let me know when works for you.