Mating issue 4

[joec230]

Hello,

I'm making a sub-assembly of some piping for a larger assembly.

When i try to mate a 90 degree bent pipe to a straight one it it throws out about 20 over defining mate errors. These errors are all with parts that have nothing to do with what i am mating now. I cann't seem to figure out why it is doing this.

I am using solidworks 2001plus.

Joe Conklin
joeconklin@gmail.com

 

[Theophilus]

That's not an issue I've found before. (Sounds like the assembly is large if it has that many overdefined mates.)

You might try rebuilding the sub-assembly from scratch to see if you can avoid the problem. Try reassembling things differently than the first time. Maybe there is something you've overlooked.


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.

 

[MElam]

Need more info.

What mates are you adding to the pipe and elbow?
Are you mating with faces? edges? reference geometry? origins? sketches? other?
Does the elbow have any straight, cylindrical faces on the ends or is it just a curve?

Mate errors can often follow throughout an assembly, since everything is usually connected in some way (foot bone's connected to the ankle bone, etc.)

 

[drawoh]

joec230,

Welcome to debugging! :O

I have problems like this all the time on complex assemblies. Part_A is assembled to part_B, which is assembled to part_C which is assembled to part_D...

Probably, something is not parallel to its mating surface. You can minimize this weirdnes by systematically mating six degrees of freedom, only. This is a good assembly strategy if your parts tend to not be orthogonal.

If your parts are supposed to be orthognal, then redundant assembly constraints will help you verify this, albeit at the cost of the hassle you are now describing.

Try suppressing and unspressing each messed up assembly constraint, one at a time. Usually, this will tell you which other dimension is causing your problem.

Your problem is probably that some piece of model geometry is not doing what it supposed to, or what you think it is doing. You need to find this and fix it.

JHG

 

[Dennyd]

There are several aspects to assembly mates that I've learned to pay attention to:
1. Use subassemblies in the files. Build up subassembly models as you would actually put the parts together. This speeds things up a lot, reduces file size and complexity (the mates are MUCH easier to navigate!), creates reusable subassembly files, and makes other mating options available.
2. Mate surfaces/faces as they would actually touch each other rather than using a coincidental surface. For instance, mate the OD of a bearing to the ID of a bore rather than to the concentric OD of the part with the bore.
3. Features that mate, such as holes, should be created in the same way. If you are mating a 3-hole pattern in two parts by using a concentric mate on one hole pair and another concentric mate on another pair then those hole patterns should be defined in the same way. I had one part where the three holes were equally spaced on a bolt circle and it would not mate to the other part where the holes were defined with cartesian dimensions. The locations were identical as far as I could tell (as far as I bothered to look which was 4 decimal places), however, they weren't exactly the same. This was a bit frustrating, but has proven to be a well-learned lesson.
4. When encountering mates that conflict and you don't think they should, try suppressing the last mate and measureing the angles or distances of the features you have just picked. Sometimes you'll find they are off ever so slightly and they shouldn't be. (If you try make this a defining dimension it becomes a mate unless that would cause an over-defining condition.)
5. Sometimes when a mate chokes and pukes it is because you have constrained more begrees of freedom than necessary. Try moving one of the parts involved in the failed mate. This will help you see where it still has a degree of freedom. From this you can use a different mate that is more appropriate. A good example of this is making two cones coincident. This creates a concentric constraint and an axial constraint, leaving only a rotational freedom. If that is what you want then all the better, but if you have already constrained the cones axially then this could be a problem.
6. Use component patterns whenever you can. This is MUCH faster than having to insert a subassembly and applying several mates. This is beautiful too because the components in the pattern can be different configurations from each other and the original. I have a part with 16 configurations. I located the first one in an assembly and created a component pattern in 2 directions with 4 instances each. I then went to each instance and selected the configuration to use. Now I had a nice overview of all the parts without creating a ton of mates.

joec230, as I read your original posted problem I would suggest moving the parts to see where they still have some freedom and then making sure to apply an appropriate mate (#5, #4, #2). The other concern would be to make sure the geometry is defined the same (#3, #4).

- - -Dennyd

 

[hisrik]

Sometimes when I had this problem, I could get past by just supressing the mates and unsuppressing them one by one instead of all at once and it worked!!!!

I know this sounds silly buy hey...it worked!

I do not know if it does on urs.try it though!

 

[macPT]

I have the opposit strategy of drawoh and similar to hisrik.

When there are several mates conflicting, I suppress all of them (not one by one) and unsuppress one by one untill reach the conflict.

Why I do this? Normally the solution is simple to find and, like hisrik sayd, sometimes SW complaints about mates that should be possible to make. By some reason SW gets stuck warning about conflicts (maybe, during the rebuilding sequence, SW find more than one possible solution for DOF constraints and can't decide what to do). But suppressing all these problematic mates and unsuppressing one by one, I drive SW to the correct solution. Once found, SW does not complaint again.

And one more thing joec230. As you make several mates between several parts, creating dependencies between those mates, you should expect that one single mate can make impossible the solution for a bunch of other mates. So your's 20 overdefined mates can be caused by the error on only one of them.

Regards

 

[Theophilus]

A coincident mate and a parallel mate referring to the same surfaces is redundant--and therefore overdefined by nature. They can both be true, but it's similar to dimensioning a feature twice in a drawing--bad practice.

This gets very important with larger assemblies. Given the problem heading this thread, debugging becomes difficult with sloppy redundancies like this. Don't allow yourself to do it or you will find yourself going bald trying to solve the problem.

A part can be constrained in three axes to lock down a part completely. Any more, and you're asking for trouble. The maximum number of mates to constrain a given part, therefore, is three. Stick to some good practices like these, follow Dennyd's guidelines above, and you'll have trouble-free assemblies (from a mate perspective).


Jeff Mowry

http://www.industrialdesignhaus.com

Reality is no respecter of good intentions.