Understanding how an assembly was created 1

[acciardi]

Hi again...

OK, so I've been using SW for an entire week now (not really true, I did go thru all the tutorials a while back).

Wonderful tool, but a quite a bit different in one aspect from my old Pro/E in regards to how assembly constraints are created.

In Pro/E the way you examine how a part is assembled is to right-click on it and select 'edit definition'. The part comes up in a small window, and the assembly rolls back to the point in time where it was mated in the assembly. You can then click on each constraint and see the associated surfaces on both parts. Pretty straightforward.

In SW, I see that each part's constraints are listed in a folder called 'Mates' that appears under each component. The problem with this view is that if the part has contact with many components, each set of constraints is listed.

The way I've been approaching this is to suppress all the components below the part I am interested in. This suppresses all the associated mates on subsequent parts and gets you to the three constraints you are interested in.

Am I missing a better way to understand the assembly construction? I found the 'View Mates' icon, but the view presented is still very confusing to me.

I might add that I am working on assemblies that were created by another engineer and I have no idea how the actual, real parts go together. I only have the SW assembly to work from.

I've opened each subassembly and exploded it to understand how they work, but this is taking a lot of time.

Any tips or suggestion appreciated.

Ed

 

[ArtemTat]

Another useful tool is "Isolate" one. RMB on component and use "Isolate".

BTW. You should't suppress all the components to leave mates belonging to this one. In the Feature Manager tree expand the component's structure and see the folder "Mates in <Assembly Name>". Here you can find all the mates added to this component only.

Artem Taturevich, CSWP
Software and Design Engineer
AMCBridge LLC

http://www.amcbridge.com

 

[brengine]

The way I've been approaching this is to suppress all the components below the part I am interested in. This suppresses all the associated mates on subsequent parts and gets you to the three constraints you are interested in.

-->This is the same method I use.

I haven't used "Isolate". I will check into that one myself.

 

[Simon205]

It may not help you totally deconstruct how your assy is mated together, but did you know if you select two components and then click on the 'ProperyManager' tab, all the common mates between the two components appear in bold?

 

[acciardi]

Ding! Thanks Simon, that is exactly what I was looking for.

Much obliged.

Ed

 

[EEnd]

I do not know if it is still the case, but when I last used ProE, it wanted the location of a component to be defined by constraints to components that were inserted earlier. SolidWorks is quite flexible in this respect. A user can throw a bunch of parts in, move them around with the mouse and then start adding mates without regard to the order of insertion. The software then tries to make it all work out. It is slick when it works and a PITA when it does not. I have found that I get more robust assemblies when I constrain each part as I go as opposed to mating them piecemeal.

Eric

 

[acciardi]

Yes, you cannot assemble a part to a part that comes later in the assy in Pro/e.

They are still 100% in pure history mode. I always build my assys like they are to be manufactured anway, as I expect most people do.

SW works a lot like NX in this regard. Siemens claimed that the simultaneous solution avoided circular references, but I don't seem to remember getting any of those in Pro.

Ed