configuration of inserted part

For convenience, I have called the parts 'A' and 'B' to describe my
issue.

I have inserted several instances of part 'B' (which has 2
configurations) into part 'A'.
When 'A' is opened, I am unable to select a configuration in part 'B',
UNLESS part 'B' is opened as well: right clicking on part 'B' and
selecting Edit in context (which effectively opens up that part file
in a second window).

The Help file says:
To change the configuration of the inserted part:
1- Right-click the part and select List External Refs.
2- Select Use named configuration, select a configuration from the
list, and click OK.

This is true if the inserted part is also opened. If not, the options
to
change configurations are grayed out.

This make part 'A" very unstable, as all the instances of part 'B'
revert back to their default configuration when opening 'A' on its
own.
When opening 'B' as a second window and switching back to part 'A',
SWX rebuilds 'A' and changes 'B' to the originally selected
configuration for each instance.

Is there a setting in Tools / Options that controls this behaviour, or
does this mean that 'B' needs to be opened systematically when opening
‘A'?
Thanks.

 

There must be more here than meets the eye because I haven't seen any
problems changing configs of parts.

So:
What SW version are you using?
Is "Part 'A'" actually an assembly?
Are there parts other than 'B' in there?
Do they work ok?
Is the 'B' part on a network that has trouble seeing the drives?
Is 'B' a part that is defined in context of some other part, or is it whole
in itself?

Normally to change the config you do a RMB and select Properties - that
gives you the "change config" box. Please provide a step by step process
that we can duplicate to try to figure out what is going on.

WT

 

Hi Wayne,
thanks for looking at my post. Apologies for the delay, and this 'A'
and 'B' business, but I try to be as clear as possible; it is not
obvious to describe in writing, worse when English is not your native
"lingo"...!
To answer your questions:
2004 sp2.1
Part 'A' is not an assy, it's a part file.
Part 'B' is on its own, not defined in context.
The intention here is to create a sheet metal part with relatively
complex tabs, folds and holes.
In fact, 'A' is a part that starts its life as a succession of
features:
Extrude thin followed by some cuts and a few more extrudes. One of
those cuts
creates an "opening", where 'B' will be positioned.
Part 'B' is created in a similar way: an extrude thin, a cut, more
extrude thin and cuts (holes), and is inserted into part 'A': 8
instances including 2 using a different configuration.
Then I Insert Bends to make 'A' a sheet metal part.
As said before, if 'B'is opened in the background, 'A' behaves
perfectly: every thing flattens perfectly!
If 'A' is opened on its own, 'B' reverts back to the default config,
and the option to swap config of 'B' is grayed out (List External
Refs, use named Config).
Opening 'B' and doing a Rebuild, will fix this.
One might argue that there are better ways to create this part (A),
but the features that are created using part 'B' are relatively
complex and are not positioned in a regular way.
Incidentally, I have come across the same problem when parts with a
right hand and a left hand are required.
I create the original part, use Insert Mirror part (selecting a plane
first) and that creates a new part.
I found this part unstable if the original part is not opened as well.

 

My side this time - sorry for the delay. I had never done this before so I
didn't know what you were really talking about. I tried it and it appeared
to work fine. I opened a part, inserted a part with multiple configs, and
then changed the config. The only thing I saw close to what you talked
about is the bullet selection of "Use model's in-use or last saved
configuration." Let us know what you see on yours.

WT

 

Thanks again Wayne for following up.
Looks like you are the only one interested in trying to answer my
post.
My question is probably not "exotic" enough for some...!
Anyway, I appreciate your time.
Yes, that's the one (bullet selection): if the inserted part
is opened in a separate window, then one has access to the options of
selecting
any of the configurations. If not, the option are grayed.
I've reported it to my VAR, following is an extract of his answer
including
a fix:
I have recreated the issue and I think it's a bug.
I will report it to SolidWorks.
here is the workaround
try this just leave part "b" closed - in part "a" right click on part
b in feature tree>.edit feature>>ok,ok this seems to relink without
having to edit in context.
Now you will also have option to select configuration.
I will let you know what SolidWorks have to report.
'Havent heard back...
Best regards.

 

Interesting - let me know what they say. And don't be too hard on the folks
here - most of the time when a request goes unanswered, it's because nobody
has an answer. It's not that nobody cares about little-ol-you, it just
doesn't make a lot of sense to say "Don't have a clue as to what you are
talking about." I'm still confused, though, as to why my test seemed
to go just fine. You might try upping to SP3.

WT

 

Point taken. Sorry for sounding "paranoid", I didn't mean to be hard
on anybody.
It's just the frustration with this issue.
For me, the Newsgroup is one of the most vital source of info on SWX.
I'll put a post if I find out more. Re. sp3, I have to follow the sp
(upgrade) path of the Company I am contracting for. Until they do
upgrade, I am stuck with sp2.1. Thanks for the suggestion though.
Best regards.

 

John:

Why have you chosen this inserted part technique for making a sheetmetal
part? Are you coming from another software like Unigraphics or Mechanical
Desktop? I would try to use native sheetmetal functions unless you have
something specific that you are trying to acheive which can only be
accomplished by this method.

Are you doing a progressive die? If so, that may change my answer a bit.

If you really have to make this method work, I would just insert a design
table, even if the DT only controls one configuration of the final part, it
allows you better control over the inserted part configs.

The syntax is $configuration@inserted_part_name. If you have multiple
instances of the inserted part, it will just put a 2 at the end of the part
name.

The reason things are grayed out when you have the part closed is that SW
considers this an in-context relationship, in the same way as if you had
created the part in the assembly. Notice the "->" and "->?" symbols (in
and out of context, respectively).

There is a Tools, Options setting which will automatically open all
referenced files. Tools, Options, System Options, External References,
"Load referenced documents" should be set to "All".

Honestly, you are cross-breeding things here I wouldn't dare to mix. I
think that is part of the reason why so few have responded to your
question, and you haven't had any definitive answers. It is a complex
question, and it seems to me to be more complex than necessary because
there is probably a better way of doing what you are trying to do. No one
can really tell you what the better way is, though, since you have not
shared, in the words of Gimli the dwarf, "What madness drove 'em in there?"

Anyway, good luck.

matt



(john) wrote in @posting.google.com:

 

I have to agree with Matt - let us help with some suggestions by posting a
..jpg of the part.

WT

 

Thanks for the suggestions (DT) Matt.
I realise that the way I modelled this part is probably not the best,
but
in the "heat of the moment", and in need of a part that would flatten
and not fail in doing so, considering the shape and irregular
placement of the various features... I went for that technique.
I don't want to waste your time and make a big deal. Furthermore, the
design of that part has already been changed... (joy of R & D!....).
Again, thanks for your assistance.