Fairly new

Hi,

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.

Anyone got any ideas what the problem could be?

Thanks in advance,

Joseph

 

There is always a reason. When you say jumbles what exactly do you
mean?

TOP

 

I mean it loses the mates. The parts just jumble?

Thanks, Joseph

 

By jumble, do you mean they move around?

TOP

 

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.

Very weird!!!

 

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.

Bo

 

I have it when I don't do anything but change custom properties???

I'm ready to go back to anything but SW...

 

In the Tools/Options/External References menu pick what are the
settings? All of them.

What setting do you have in Tools/Options/FileLocations/References?

Do you have files with the same name stored in different directories?

TOP

 

I have not experienced what you speak of and I use SolidWorks nearly
every day since SP 3.4 was released, so I know it can work.

Bo

 

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.

Hope this helps,

EdT

 

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.

Thanks for your help!

Joseph

 

Sometimes it works just fine?

 

Hi and thanks!

Under Tools/System Options/External References/Assemblies;

should I select: Do not create references external to the model?

I don't see the option for External References Off

Thanks, Joseph

 

Check that last line of my earlier reply. I do have a "Huge" button called no External References, duh!

 

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.

Bill

 

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.

Thanks - Bo

 

Please post under this link if you find it.....

-Joseph

 

"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."

There is a reason. You just need to figure out what the reason is.

I would strongly suggest you buy The SolidWorks Bible. It will give
you many insights into how SolidWorks works behind the scenes.

If you decide to take my advice and buy this book look at:

Chapter 12 which discusses in-context reference update holders. In-
context reference holders can be examined to see what parts the in-
context relations go between.

Chapter 16 Modeling In Context. Page 485 covers Multiple Contexts...
the dangers and necessities of.

Page 490 covers In-context file management and why you should use
SolidWorks Explorer to rename parts and assemblies.

 

"I ask, because the issues of assembly problems and quirks in
SolidWorks seems to come up over and over again."

Of course they do. SolidWorks Corp. causes this buy not providing the
documentation with SolidWorks on how to properly model.

Suggest you start recommending someone lay out $50 and buy the
SolidWorks Bible as well as giving the pages in the SolidWorks Bible
where the issues they are raising are covered.

 

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.


matt

<Good Luck on this. I think it is fixable -- Bo>