Assembly Mating Scheme - Why does it change?!!!

[Ewan]

Hello all,

Soliworks 2001plus SP4.1 with PDM2001

A recurring problem that I and a couple others here are experiencing is that while we are working on a top level assembly the mating scheme changes thus producing a knock on effect that sends us into oblivion with many, many mate errors. This has happen to me twice today however the same process produced different errors (seems a bit random).

It seems as though it is a bug, however we don't know what the catalyst is.

Is it the complexity of the assembly?
Is it to do with our PDM? (this started to happen a little while after PDM installation, coincidence?)
All the mate errors seems to be linked to a common cabinet frame that is used in 3 different projects could this be the problem child?

The reason for the thread.
Can anybody shed any light on this dark situation. The amount of reworking/rebuilding the assembly is really slowing down projects.

Is this a Service Pack problem if so can any body recommend a service pack for 2001plus that has a mininium amount of bugs (I understand that some times increasing SPs solves one set of bugs only to gain others). We don't have a Maintence agreement.

It might be possible to get Service Pack v6.0 from our SW distributer who is sympathic to our cause, however denies all knowledge of bugs in the system (understandably).

Any help of any kind will be warmly recieved.

Many Thanks

 

[TheTick]

an untested theory....

One possibility is that the component files are getting altered by the parent assemblies. Try turning off the automatic naming of entitites used in mates. It is under "Tools --> Options --> System Options --> External References --> Automatically generate names for referenced geometry".

If you can, try manually adding names to component geometry that will be used for mates.

Good and evil: wrap them up and disguise it as people.

 

[SBaugh]

It sounds like to me you have in-contexted a single file "cabinet" and it is used in multiple assemblies. When you in-context a part in an assembly, you are not to in-context in another assembly. It will cause mate errors. There is away around this. You would have to suppress all features and sketches in the current model now and add a configuration, then rebuild the "cabinet" with all new features. Now you can in-context them to another assembly.

You should read the help on In-contexted models if you haven't already. Number one advice I give for In-contexting. BECAREFUL - and watch and remember everything you do when in-contexting if you don't it will haunt you later. Which I think is what your seeing now.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[Regg]

On other possibility. When you open the assembly, are all the features of the cabinet frame resolved. I have several large assemblies (different parts) that I have to open one or more of the sub parts (or subassemblies) first because (for whatever reason) when I open the assembly first, not all the features build correctly and I get mate errors that look like I have major problems with the assembly. If I open the sub parts first, they build correctly and when I open the assembly, it opens without any mate errors at all.

Just a thought,

Regg

 

[automationbabe]

Check if any of the assemblies are flexible vs. rigid. I've seen this cause problems when creating/modifying mates.

Flexible assemblies are cool to use, but it carries the same warning Scott gives about in-context parts.