Failing mates

[Uncle_Hairball]

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]

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.

Hello Uncle Hairball (great name!)

1 - Any imported geometry?
2 - Relative small/large features (.001mm and 1000mm)
3 - VOR (verification on rebuild) On/Off?
4 - Configs?
5 - rebuilding via Incontext relations or CRC's?

[mike miller]

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.

[SPerman]

Too many mates in a single assembly/sub-assembly is another possibility. The solidworks mate solver runs out of fingers and toes rather quickly. After that, it becomes inconsistent.

Parallel mates also tend to cause lots of problems.

[Roasted By John]

Multiple mates doing the same thing, how many times have I forgotten that I mated those parts before??

First off, I would delete all the mates and start over, I can't stand assemblies that act like that, drives me nuts, good when you save and then forest fire when you open, definitely a "Delete The Mates" candidate.

You really don't need to delete all of them, I normally start from the bottom and go up, delete a section, close and re-open the file.

To reduce the amount of mates, look for perpendicular possibilities, two mates instead of three is a plus by subtraction

[MJuric]

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.

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.

[Uncle_Hairball]

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?

[Uncle_Hairball]

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.

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]

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.

Maybe I should clarify a little: The assembly was good last night (it's not just one assembly, it's a recurring problem with many assemblies), today it is not. I am the only SW user unless China is hacking my files. Nothing has been done to the parts or assemblies. All I did was go home, have dinner, sleep a little, come back, and open the file. Kaboom!

[mike miller]

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.

Do they go away with a Ctrl+Shift+Q?

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.

[matt]

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]

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.

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]

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]

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.

[Uncle_Hairball]

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.

Interesting... I am very careful not to overconstrain, but your explanation has made me realize that my typical method has too many rotation constraints. I'll have to reconsider.

[Uncle_Hairball]

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

Yes, I've seen that, too.

[Uncle_Hairball]

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.

Understood and I agree. That's the way I usually do things.

[DennisD]

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.

These are good tips. Subassemblies in particular are good, especially if you can put as many things in the subs as possible.

Also, sometimes if the subassembly is a purchased group of parts or otherwise can be static then you can locate them with mates and then Fix everything and then suppress the mates. THIS really helps!

Assembly patterns are also very good. Keep in mind that the pattern instances can reference different configurations of the subassemblies.

[Roasted By John]

sleep a little, come back, and open the file. Kaboom!

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

[TRKemp]

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.

Likely not your issue, but the only time i have issued with this occurring is when my assembly opens in Large Assembly Mode. Usually i can correct it by resolving everything.. etc.. but instead I mostly just close it and open it resolved.

Also, if I have a part or sub-assembly that was working just fine but then gives me mate errors, I always try just suppressing and unsuppressing it before messing with any mates. More often then not it right's itself, albeit inexplicably ... but that's SW for you.

[MJuric]

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.

Absolutely agree that the least complex you can make an assembly the better. I try to make S/A's simple, if possible and mate them in their parent by the base level planes and origins. This kind of sucks because it requires that all the S/A be designing in machine position. This also can't be done when you have moving S/A so they have to be mated the way they are built or to the item they are not moving in relationship to.

[Damo]

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.

I'll second this.. and add that Tangent mates also have frequently caused me no end of grief until finally throwing my arms in the air and deleting them and creating other reference geometry to enable a more stable coincident mate instead.
And, YES..! It can literally take only one "flipped mate" to throw up a swathe of errors across the entire mate folder

[Glenn Schroeder]

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.

[Uncle_Hairball]

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

Thanks! Hairball was given to me by my fraternity brothers and Uncle was given by my sister when she made me an uncle.

[Roasted By John]

Thanks! Hairball was given to me by my fraternity brothers

That's enough on the Hairball comment, seems to be a lot more then we wanna know behind that nickname, oh boy

[Ry-guy]

Crap. I thought this thread was about Failing dates. I've had a lot of those in the past. Not nearly as many failed mates though!

[Damo]

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.

Oh YES..!! This too. In actual fact, that is my "Go-to" method of dealing with any sudden and inexplicable forest fires in the feature tree.
Find the first RED broken mate and supress and unsurpress. Presto, fire is out.. I guess SW just gets overwhelmed or confused sometimes..
It took me a while to work this out too. The number of times I've wasted time chasing down conflicting mates to find nothing wrong and it all just suddenly works again.

[matt]

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.

[Glenn Schroeder]

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]

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.

I've had that too! Did you ever find a remedy? SolidSometimesWorks!

[Glenn Schroeder]

I've had that too! Did you ever find a remedy? SolidSometimesWorks!

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.

[Jaylin Hochstetler]

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.

I also use it for hardware. I have a macro for it w/ a button for it on one of my mouse gestures. It locks the rotation, and enters 0" for the distance. The only problem is it won't always get the alignment right. The macro is in the downloads under Mike Miller's macros.

[mattpeneguy]

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

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?

[matt]

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?

I only made a 2 cylinder engine in SE, and I don't think I had the same kind of problems. The mate solving is not a Parasolid function, and I do think they use different components to solve mates.

[DanPihlaja]

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?

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.

[Tom G]

To reduce the amount of mates, look for perpendicular possibilities, two mates instead of three is a plus by subtraction

Yuck!
Sorry to join this topic after it's been eviscerated clean.
I only wanted to chime in that Perpendicular mates cannot flip when you want them to. I prefer the extra control that Parallel allows.

That said, I also have begun making a redundant alternate (Front-like) Plane, for example, and I call it Accessible Plane. This way, I can orient my ball valve stems (and handles) to that plane, and if I wanted to flip which side is more accessible, I flip the reference plane and they all follow.

[mattpeneguy]

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.

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?

[DanPihlaja]

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?

I have seen the issue (to a lesser extent) in CATIA V5.

I know that I saw the issue in I-DEAS.

[SPerman]

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?

I don't recall every having this problem in NX.