Mate(s) Problem... Again!

Does it clear up when you do a Ctrl Q?

I am not sure why SolidWorks does this. I have seen this happen also on rare occasion. Usually a Ctrl Q clears it up. It is like the mate solver gets stuck and doesn't cycle through all the mates.

If you just need the bolt for a screen capture, you could check the option box at the bottom of the mate screen to "Use For Postioning Only" so the mates are not actually added to your assembly.

Regards,

Anna Wood

Ar> Hi,

Aron,

Do you have the bolt heads constrained so they can't rotate ???? Like maybe using a parallel mate with a flat ???

I tend to leave bolts free to rotate. The assemblies seem to solve faster too.

One of the guys here can't stand to have any minus signs next to any parts. He was getting lots of mate errors with parallel. He started using perpendicular instead, and doesn't have this issue.

Mark

Hi,

It does not clear up upon control Q, and I also do not have the bolt "parallel" constrained. I usually leave the bolts mated as they come from the toolbox - i.e. concentric and coincident... that's all.

I will try the position only.. I do use this, but, really SW should be able to do this... are you listening SW.

I also do not mind "minus" signs in my assemblies. I am very methodical when I put an assembly together, just because of what is happening right now - an over constrained "something - somewhere". I will be loading 2007 in the next few weeks or so to try out the new "SWIFT" technology (I believe it handles problems with mates).

It certainly is difficult finding the problem mate...

Thanks for you solutions to my issue(s),

Aron

A lot of times, for me is the solution to suppres the last added mate(s), then the red flags disappear. Un-supress the supressed mates and all works fine! Strange, but it works for me.

Wim

You can try the old trick: suppressing _all_ faulty mates in one go and then 'Undo'. This used to help with earlier versions. Unfortunately it is usual that they wrack the mating system in the new version again... although it used to happen with SP 4.0 rather than with SP

Do you have any sub assemblies in the major assembly?

One time I had an assembly with some sub assemblies. Then the client requested some additonal parts. Without paying much attention the new parts were contrained onto the sub-assembly but in reality the parts were placed at the assembly level. This is actually very easy to do and SW should really pop up a warning when the user does something like this. But, until then we just need to be aware of such a sequence.

Even this confussion did not create any problems until a certain number of the parts were constrained. Then, all of a sudden there were all kinds strange errors and reaction.

When the new parts were moved up to the assembly and reconstrained the problems all disappeared.

But, if you don't have any assemblies this isn't your problem.

Hope this helps.

Ed

Ed (& everyone else),

That may be it... I have the "Major Assembly" made of some "Sub-Assemblies", and then the hardware (from the toolbox), and a few brackets, etc., to hold it together - i.e. like you would build it in reality.

I had a "width mate" (which can be handy at times) especially in this case since these "panels" that get installed are movable, then you drill and rivet on site. Anyway, once I got ride of that width mate things cleared up...almost.

I did notice something strange (and I will mention an "artifact" later), I had a part that seemed to have been mated to itself??? I do not know how it happened - you cannot do it, SW won't let you - but it was an edge mated to a nearby radius on the same part - a sheetmetal part. After I deleted that mate, the part changed orientation and all was well again, and the assembly is living happily (it loads faster) ever after!

Now for that artifact I mentioned earlier... a few parts in these assemblies in question kept loosing their leaders of notes on the drawing sheets. I always check the PDFs I send via email and twice I have had to go back into the drawing and re-enable the leaders! I noticed this when I control-c copied a note from one page to another in the same drawing, then saved the drawing in PDF format. Under review of the pending/to-be-sent email, I saw the problem... just thought I would mention this for added confusion :^}

All seems quiet in the land of oz for the moment - I've made it to "Munchkin Land"... all parts, assemblies, and drawings are working, and the "Lollipop League" is happy. See: