CAD Forum

Uncle_Hairball wrote: ↑Wed Apr 28, 2021 12:22 pm Over and over again, I have a stable assembly model with no red or yellow mates. I save and close and the next time I open the model, it turns red. Any thoughts as to why this would be happening? I'm on SW 2019.

Uncle_Hairball wrote: ↑Wed Apr 28, 2021 12:22 pm Over and over again, I have a stable assembly model with no red or yellow mates. I save and close and the next time I open the model, it turns red. Any thoughts as to why this would be happening? I'm on SW 2019.

zxys001 wrote: ↑Wed Apr 28, 2021 12:39 pm Hello Uncle Hairball (great name!)

1 - Any imported geometry?
None
2 - Relative small/large features (.001mm and 1000mm)
No
3 - VOR (verification on rebuild) On/Off?
On
4 - Configs?
Sometimes
5 - rebuilding via Incontext relations or CRC's?
No in context relations. What's a CRC?

mike miller wrote: ↑Wed Apr 28, 2021 1:02 pm Where are the errors and what do they say? I haven't used my crystal ball for awhile.
Is it a lost mate reference, an overdefined condition, or a failed external reference...or...???? It's an absolute shot in the dark without knowing more details.

Uncle_Hairball wrote: ↑Wed Apr 28, 2021 2:23 pm The problem I'm trying to resolve is not the errors; rather, I'm trying to figure out why the assembly goes from resolved to corrupt just because it took a nap overnight. The errors are conflicting mates or over constrained assemblies.

Uncle_Hairball wrote: ↑Wed Apr 28, 2021 2:23 pm The problem I'm trying to resolve is not the errors; rather, I'm trying to figure out why the assembly goes from resolved to corrupt just because it took a nap overnight. The errors are conflicting mates or over constrained assemblies.

Uncle_Hairball wrote: ↑Wed Apr 28, 2021 2:23 pm The problem I'm trying to resolve is not the errors; rather, I'm trying to figure out why the assembly goes from resolved to corrupt just because it took a nap overnight. The errors are conflicting mates or over constrained assemblies.

mike miller wrote: ↑Wed Apr 28, 2021 2:35 pm Do they go away with a Ctrl+Shift+Q?
I wish, but no.

Are there mates to Sheet Metal parts? I've had face IDs switch randomly after a bad night's sleep(?). This will cause conflicting mate conditions that can be difficult to find. The What's Wrong dialog is your best friend in a case like this.
No sheetmetal in this case.

matt wrote: ↑Wed Apr 28, 2021 2:42 pm SolidWorks plays fast and loose with a lot of things. One way you might normally think of a "fully defined part" as having 3 plane-to-plane coincident relations, and SW lets you do that, and trains people to do that.

Degree of Freedom analysis

- 1 X to X plane coincident mates locks down 1 translation (in X - translation in Y and Z are open) and 2 rotation (about Y and Z - rotation about X is open)

- 2nd plane Y to Y plane locks down translation in Y, Z still open), rotation in X and Z are locked, Z is double locked, no rotation open)

- 3rd Z to Z plane locks down translation in Z, all closed. Locks rotation in X and Y, both double locked.

So your standard 3 plane coincident scheme leaves you with 3 overdefined degrees of freedom, but SW somehow allows it... sometimes. And then suddenly it doesn't.

Instead of 3 coincident plane mates, you could use 2 line-to-line mates, which locks everything down, but still has 1 overdefined dof.

If you think of mates as constraining degrees of freedom, you are less likely to overdefine your mates, and can stop relying on SW to to allow some and not others as it sees fit.

AlexLachance wrote: ↑Wed Apr 28, 2021 2:46 pm Oh, I know I know!

You use flexible assemblies. Remove the flexible and put it back. For some reason when you restart SolidWorks, it doesn't remember the flexibility of the assembly and therefor throws those error. Removing it and putting it back on refreshes it's memory. SolidDoofy

SPerman wrote: ↑Wed Apr 28, 2021 2:52 pm My problems weren't really about over-defining the mates, but more about overwhelming the system.

Old way
1 assembly with 100 parts

New way
1 assembly with 10 sub assemblies, each with their own sub assemblies as needed.

Old way
100 fasteners

New way
1 fastener and component patterns

Old way
Mate as the machine would be built

New way
Use ordinate geometry as much as possible.


Solidworks has to simultaneously solve all mates in a given assembly. It has a much higher chance of success of solving 10 individual assemblies with 10 mates vs 1 assembly with 100 mates. (Even if all of those smaller assemblies come together in the main assembly, they are solved one at a time.) Hopefully I've done a decent job of explaining this.

SPerman wrote: ↑Wed Apr 28, 2021 2:52 pm My problems weren't really about over-defining the mates, but more about overwhelming the system.

Old way
1 assembly with 100 parts

New way
1 assembly with 10 sub assemblies, each with their own sub assemblies as needed.

Old way
100 fasteners

New way
1 fastener and component patterns

Old way
Mate as the machine would be built

New way
Use ordinate geometry as much as possible.


Solidworks has to simultaneously solve all mates in a given assembly. It has a much higher chance of success of solving 10 individual assemblies with 10 mates vs 1 assembly with 100 mates. (Even if all of those smaller assemblies come together in the main assembly, they are solved one at a time.) Hopefully I've done a decent job of explaining this.

Uncle_Hairball wrote: ↑Wed Apr 28, 2021 2:29 pm sleep a little, come back, and open the file. Kaboom!

Uncle_Hairball wrote: ↑Wed Apr 28, 2021 12:22 pm Over and over again, I have a stable assembly model with no red or yellow mates. I save and close and the next time I open the model, it turns red. Any thoughts as to why this would be happening? I'm on SW 2019.

SPerman wrote: ↑Wed Apr 28, 2021 2:52 pm My problems weren't really about over-defining the mates, but more about overwhelming the system.

Old way
1 assembly with 100 parts

New way
1 assembly with 10 sub assemblies, each with their own sub assemblies as needed.

Old way
100 fasteners

New way
1 fastener and component patterns

Old way
Mate as the machine would be built

New way
Use ordinate geometry as much as possible.


Solidworks has to simultaneously solve all mates in a given assembly. It has a much higher chance of success of solving 10 individual assemblies with 10 mates vs 1 assembly with 100 mates. (Even if all of those smaller assemblies come together in the main assembly, they are solved one at a time.) Hopefully I've done a decent job of explaining this.

MJuric wrote: ↑Wed Apr 28, 2021 1:45 pm One of the things I absolutely abhor about SW. It seems to randomly decide which mates are higher up in the hierarchy and thus causing, randomly, mate errors. Then to make matters worse rather than having any ability to narrow down where the problem is it simply throws up it's hands and proclaims "EVERYTHING IS BROKEN!".

I had an assembly that would randomly flip the direction of a shaft once. No errors no yellow, red...shaft going one way, then the next time you looked, shaft is going the other way. It was maddening.

As others have noted the culprits are often times conflicting mates, duplicate mates and the worst offender is angle mates.

Roasted By John wrote: ↑Wed Apr 28, 2021 3:20 pm It's the loss of sleep, which could be directly related to overseeing anything till it's way too late, using SW sometimes give us "Day Mares" which reduces the ability's for the 2:00 snooze we all need, dream on, yep that don't happen in Fusion 360, neither does anything else,

BTW - Best Forum Name Ever :0

Uncle_Hairball wrote: ↑Thu Apr 29, 2021 1:12 pm Thanks! Hairball was given to me by my fraternity brothers

Glenn Schroeder wrote: ↑Thu Apr 29, 2021 7:05 am It's not particularly uncommon that I get mate errors on an Assembly that previously didn't have any, so I suppress one of the mates. The errors go away. I un-suppress the same mate. No errors.

Glenn Schroeder wrote: ↑Fri Apr 30, 2021 10:56 am I had a profile mate between two rectangular faces that would randomly rotate one of the components 90° when I wasn't looking. That was fun.

Jaylin Hochstetler wrote: ↑Tue May 04, 2021 8:22 am I've had that too! Did you ever find a remedy? SolidSometimesWorks!

Glenn Schroeder wrote: ↑Tue May 04, 2021 8:31 am No, but I don't believe I've used a profile mate on rectangular surfaces since then either. I typically use them for mating hardware in holes.

matt wrote: ↑Fri Apr 30, 2021 10:17 am I had a run in with not failing mates, but flipping mates. This may be an old story for some of you, but when I was working on an engine assembly for some training materials, I absolutely could not get the Cam mates to stay where I put them. I assembled an 8 cylinder engine with all of the moving parts for overhead cams and valve lifters, and as it would go through the motion, one or two of the followers would just instantly flip.

This gif shows what's going on. The assembly was built originally in 2012, and then updated in 2018, and now checked in 2020, and it's still doing the same thing. You may have to click the image to get it to play. Larger gifs get a thumbnail which isn't animated.

To me its kind of remarkable that the software can handle the 281 top level mates and 272 flexible subassembly mates it takes to make this go, but why it always has to flip some of them after they've been working just blows me away.

zzz.gif

mattpeneguy wrote: ↑Tue May 04, 2021 9:30 am So @matt,
There was a whole thread about flipping mates over in the old forum. Just out of curiosity does this type of thing happen with SE? If not, how do they handle it that the SW people can't figure out?

mattpeneguy wrote: ↑Tue May 04, 2021 9:30 am So @matt,
There was a whole thread about flipping mates over in the old forum. Just out of curiosity does this type of thing happen with SE? If not, how do they handle it that the SW people can't figure out?

Roasted By John wrote: ↑Wed Apr 28, 2021 1:29 pm To reduce the amount of mates, look for perpendicular possibilities, two mates instead of three is a plus by subtraction

dpihlaja wrote: ↑Tue May 04, 2021 11:54 am The problem is, when a mate has 2 (or more) possible solutions, when Solidworks is rebuilding, it can "jump" to one of the possible solutions, which may or may not be the solution you wanted.

I understand it......but not necessarily like it.

The only solution is to make sure that there is only 1 solution.

Example: Tangent mates are notorious for flipping to the other side of the circle because, mathematically, it is a valid solution.
The solution is to eliminate all other possibilities. Like use some sketch geometry to create a line with an end point where you want your tangency. Now make your tangent line coincident with the end of the line.

mattpeneguy wrote: ↑Tue May 04, 2021 12:43 pm I get it too Dan. But, what does SE and IV do to prevent this or, do both of them have the same problems?
Do SE and IV "know" proximity to where the initial mate is made and not make the mistake?
I wonder if SW didn't create the situation with their choices and whether the other guys were smarter and understood and planned to avoid this situation?

mattpeneguy wrote: ↑Tue May 04, 2021 12:43 pm I get it too Dan. But, what does SE and IV do to prevent this or, do both of them have the same problems?
Do SE and IV "know" proximity to where the initial mate is made and not make the mistake?
I wonder if SW didn't create the situation with their choices and whether the other guys were smarter and understood and planned to avoid this situation?