Disappearing Relations

[nitan]

Hi,

Question here. I have SW 2005, make realatively large assemblies, and subs, subs within subs,etc. Problem is, I will get a complex assy together and working properly, IE front suspension/steering, I save it, and the next time, or several times later, I will open the file,and all of the relations have been disconnected, and I did nothing to the file.

Is there a setting that I am forgetting?

 

[ctopher]

Does it happen with the same assy, all of them during a session, or varies? If you close the assy (or SW) then reopen, is it fixed?

Chris
SolidWorks 06 5.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 01-18-07)

 

[CorBlimeyLimey]

Which SP?

Do you have configurations of the assemblies?

Are you opening the assy in the Large Assembly mode?

What happens if the Large Assembly mode is not used?

 

[debodine]

We had exactly the same thing happen when our IT department decided to mess with the network permissions of our engineers. Unfortunately I am not in IT nor privy to exactly what they changed and what they had to change back to fix the problem, but it caused plenty of problems for us. Some of the engineers are still having problems because IT did not do exactly the same thing to each computer. Perhaps it is a permissions issue? Do you get any unusual messages when opening Solidworks?

debodine

 

[TheTick]

Check this setting under your options:

"Automatically generate names for referenced geometry"

Look under "Tools --> Options --> System Options --> External References" to find this setting.

I believe that if you have this option checked, the name is written to the component. This name is lost if your component is read-only. You will need to have this option unchecked.

I could be the world's greatest underachiever, if I could just learn to apply myself.

http://www.EsoxRepublic.com

-SolidWorks API VB programming help

 

[nitan]

Well,
I am on a single pc, no network, the problem seems to just happen, then stays that way. I have had the ext refs checked and unchecked, depending, so I am not sure what the cause is.

I work with assys, and sub assys, etc, and the more complicated I get, like a front suspension/steering system, the more likely it will happen, then I need to reattach everything.
Just wondered if anyone else has had this problem.

 

[SBaugh]

When you are done making your mates, or after you make a few mates try a crtl-Q. I bet the errors are there before you close and save the file and a ctrl-Q will help you figure that out.

Regards,

Scott Baugh, CSWP

http://www.scottjbaugh.com

faq731-376

 

[EEnd]

We have had problems with “fragile” assemblies. There are many different ways of putting together an assembly, and SolidWorks handles some better than others.

Scott has some good points in a document on his site. It is Assembly Mates and Best Practices in the Tips and Tricks section. Another good read is thread559-160440. Here are a few tips, in addition to (and probably repeating) the points in those locations:
[ul]
[li]Create and use reference geometry (planes, axes, points) in your mates. They are more stable than surfaces, edges and vertices. I also try to keep my mates between things directly in the assembly, i.e. not mating features of components of one subassembly to features of components of another subassembly. This is typically accomplished by creating reference geometry in the subassembly that coincides with mating features of the component.[/li]
[li]Arrange the components and mates in an order that is easy to resolve. SolidWorks will let you plop down a bunch of parts, and throw in a mate here and a mate there until it is all locked in place. However, it can become confused and fail to resolve everything at some later time. By carefully arranging the components and mates in the feature tree, you can make it easier (or harder) for SolidWorks to get it right. Move static components up, followed by things that are mated to them. Have the mates for those components at the top as well. When you have a group of components whose positions need to be solved simultaneously (linkages and the like), keep them and their mates close together.[/li]
[li]Avoid over constraining the model. This is probably the guideline that I do the worst job of following. I often use coincident mates of the 3 default planes to locate parts. That is enough to lock in 9 degrees of freedom, when an object only has 6. Usually you can get away with it, but not always.[/li]
[/ul]

I’ll admit that structuring your models in this manner takes a little more up front work. However the result is generally more stable within SolidWorks and more robust to design changes.

Eric