I'm fairly new to SW. The company I'm doing work for only has SW 2006 and for some reason it just jumbles the assemblies at times for no apparent reason.
Also for some unknown reason it will at times link several other components to a single file. e.g. You open a part to detail it and several others open up with it.
It seems to be very unstable over all. You can be working on an assembly for two days with no problems at all. Then all the sudden it goes stupid.
Yes they move around. Also sometimes you will save and everything is fine, no errors or anything. Then you re-open the same file and all the sudden you have several mate errors.
I notice this happens quite often when you make a change to a part in the assembly.
e.g. You add a hole or a cutout that has nothing to do with your mates, then when you re-open the assembly you'll have mate errors, or jumbled components.
Sometimes you just get errors and sometime the parts all shift/move.
I have seen this when I add or remove a radius or chamfer on a face which serves as the mating surface in an assembly.
Sometimes there is no way around just redoing the mate.
Other times, if you know you are going to mate to a surface you can make sure the mate surface is "colinear" with a plane in your solid model, and then you mate to the plane and not the specific surface which may be modified by lots of other operations.
Sorry that you have had so much trouble. "jumbled" assemblies is one of the main reasons why I dumped Inventor. I have had this happen in SW a time or two but it was more the result of having "External References". This basically "ties" various features of one part to another if they were developed in an incontext assembly, (such as a hole). Then if one of the parts is moved this can cause some very strange interactions when combined with mates and the assembly can really be messed up..
External References can be useful at times but for the beginner I highly recommend to besure these options are "off". There is a button, "No External References", (it has a big red X over the button) this should always be left on.
Another thing is to ground the main part in an assembly, (such as the frame) and mate everything to it.
The other thing that can cause some real problems is when there are sub-routines in a main assembly. Then if a part is placed into the main assembly and some of the constraints are made to the sub-assembly SW gets confused. In these cases if a part is associated with the sub- assembly it should be moved into the sub-assembly.
Allow multiple contexts for parts when editing in assembly; checked Load referenced documents; changed only Serach file locations for external references; checked Update oout of date linked design tables to; prompt Update component names when documents are replace; checked
all others in this menu are blank.
Don't see "References" but do have Referenced Documents. There is nothing listed.
Sometimes; when I use commercial parts I will copy the commercial part from my library to the working directory so I don't forget to collect it for the customer.
One really simple technique you might try for simplification of a troublesome assembly is to eliminate some of the mates. When your design is "mature" and some of the major components/subassys aren't going to move relative to each other (or to the assy origin), you can Fix them. At this time a number of mates will become overdefined, but they can now be deleted. Assembly rebuilds are also somewhat quicker. If a component needs to be moved in the future, you can always set it back to Float and recreate the appropriate mates. This approach works only if the assembly is "static", and components are not repositioned in different configurations.
At one time there was a document available on how to work with largish assemblies better which started back in 2004, according to my notes, but I lost track of whether it was a document from Matt or another user or SolidWorks.
Does anyone know where that document is located on how to do assemblies "better" and faster?
I ask, because the issues of assembly problems and quirks in SolidWorks seems to come up over and over again.
Here is an old list Matt Lombard posted in this newsgroup from his hair-raising (or hair pulling experiences he has necessarily endurred in helping himself and others become more productive:
Here are things that will slow down SW:
- unnecessary incontext references
- circular incontext references (PartA has a feature which is dependent on PartB which has a feature dependent on PartA)
- mates made to time dependent assembly features (incontext, assembly cuts, children of patterns, etc)
- incontext relations across subassemblies
- flexible subassemblies
- hundreds of mates at the top level (no use of subassemblies)
- all hardware (screws) mated individually instead of using patterns
- display quality maxxed for assembly and all components
- anti virus software set to scan all opened documents
- not fixing errors on mates or features (tries to solve every rebuild)
- opening SW by double clicking on files on a network drive (journal file is written to constantly across network)
- no use of any of the tools SW has provided to speed up performance (large assy mode, lightweight, hidden, suppressed, simplified configurations, fast hlr, low quality transparency, subassemblies, locked incontext relations, etc.)
- unnecessarily detailed models (geometrically accurate springs, threads, etc.)
- autorecover settings set low
- load referenced documents set to always
- verification on rebuild
- software OGL
- anti alias turned on
- using hlr in shaded mode or wireframe
- poorly ordered equations
- using sketches with a lot of entities rather than separate features with simpler sketches
- sketch patterns instead of feature patterns
- other generally bad modeling practices
Just because SW gives you the flexibility to be able to do what you want doesn't mean that you are immune to the effects.
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