Info on Mates and Relations

[MikeInSoCalif]

As a user group leader, I figured I would try and put together a technical presentation that I could give to our group. I choose mates and relations for two reasons. First, when I first started using SW, this is an area that took me a while to understand. Second, there looks to be numerous new mate and relation features comming in SW2007.

So what I would like to get from people here, is their hints, tips, quirks, and observations of how mates and relations work for them. Basically just the little things you know about them. I can then complile all of them into a presentation. Thanks for the input.



Mike Puckett
Group Leader
Los Angeles/Orange County
Solidworks User Group

 

[Nella95]

I don't do this much anymore, but I had a problem with 'over'-mating my assemblies. It doesn't happen so much anymore, and I'm not terribly sure how it happened in the first place. (I just know, that if I am the sole creator of the parts and assembly from the word 'go' then - I rarely, if ever, have those 'over'-mating problems)

And there are some 'rules' I live by:

*mate to planes or faces if at all possible
*mate - how you would put it together, if you were building the piece (SolidWorks is one of the best 3D modelers at this - and performs features on the part, in a way that would happen in real life)
*(it's just me, I think) - but I, personally like to fully constrain my parts in assembly -(even my fasteners) -- unless I'm using COSMOS Motion

 

[dezignstuff]

I find the SW interface for mating to be pretty clumsy. You're always clicking extra things to close the dialog, and editing mates is worse yet.

To get around the clumsy creation, I prefer to use mate macros. Click face, ctrl click face, hit hotkey. Way faster unless you're doing distance or angle mates or some complex mate.

Also, you should demo the Width mate and Symmetry mates. I think these are underused, and can save you a lot of time. The width mate makes it easier to center components that weren't created symmetrically.

SW a few releases ago became very error-phobic when it comes to mates, so there are many times when you have broken mates that don't show up as errors on the top level mate folder, so you have to keep your eye on them.

Mates are more stable when they are made to things that can't fail, or at least can't disapear due to failure, such as planes, axes, sketches. Faces disapear when features fail, when split lines are used or when consumed by other features. Edges can change internal ID if either face changes, and of course vertices can change if any of the edges that come together change. These entities are listed in order of stability.

Motion of complex mechanisms (a gripper at the end of a robotic arm) can be difficult if there are too many degrees of freedom open. Sometimes adding more mates will make it easier to move a part at the end of a long chain of moving parts. Sometimes fixing one part (living temporarily with the associated over-defined errors) will allow you to move a part which might not have moved smoothly when the entire mechanism was free. If there is more than one possibility for the positions of other parts, the part you are trying to move may be difficult.

 

[CorBlimeyLimey]

Definitely do a demo to explain Cam, Gear & Limit mates. For some reason they seem to confuse many people.

The Use for positioning only option could also be explained.

Using folders within the mategroups can help to quickly locate sets of mates for particular parts.

Naming, or rather renaming, mates is also a good practice in some cases where some manipulation may be in order. (eg. "Fascia Open Angle" is much easier to understand than "Angle53")

The benefits of using Mate References could also be explained.




Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[MikeInSoCalif]

This is all great information so far. This is what I was looking for. Any and all info is appreciated.

Mike Puckett
Group Leader
Los Angeles/Orange County
Solidworks User Group

 

[CorBlimeyLimey]

The use of Sketch Relations can be a blessing & a curse. They can be extremely powerful when used correctly. (eg. the symmetry used in the sketch profile of the Spoon example at Matt's site), but they can be a real PITA to fathom out what is related to what. Especially if the relation symbols are turned off.

I prefer to use actual geometry to force the relations/constraints. (a hangover from the "golden" days manual drafting) eg. a horizontal construction line (chord) to constrain the endpoints of an arc, rather than just making the endpoints horizontal. The chord is an instant visual relation. The two "floating" endpoints may not be so obvious.


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[ctopher]

Maybe on auto-mates, cntrl-drag a part to an assy and auto-mate. A lot of users do not understand it.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 05
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[mncad]

Along the lines of what CBL said about renaming, I used to rename all of the mates which was rather time consuming. Now as soon as I have the mates for a particular part done I add them to a folder and name the folder something meaningful. The mate will still be named "Angle53", but at least it is in a folder that makes it easier to find. Also for relations, the Display Relations is a handy thing if you have an overdefined sketch.

mncad