Assembly modeling - copying a part?

Here's my situation.

When i'm modeling an assembly, i'll usually be in the assembly.. then
create a new part to add to the assembly (insert -> component -> new
part), then start modeling, still in the assembly. Then when i'm done,
i'll go back to the assembly level, and create a new part. etc, etc..
I'll sometimes create external references in the process, but thats
fine, i want this as i have reference planes in my main assembly that
i want my parts to follow. Also when creating a part (for reference,
this is mostly woodwork, 3/4" panels, etc) i'll sometimes 'extrude to'
a surface of another part, just so that if that panel is ever further
away from it, it'll still extend to match, etc.

Now, if i end up having say, a box.. I'll create my bottom, my back,
then one of the sides. For efficiency in manufacturing, i'd like the
other side to be identical (in fact, i want to use the same part file
so that our CNC system recognizes the duplicates), so i'll go ahead
and use a copy of that first panel, and mate it into position. I'll
usually only do this when i know that those panels stay identical if i
have to change the dimensions of the bottom or back.

Now say i have a panel in between these two sides, thats also
identical. so now i have 3 identical panels, one of them being the
'original' with the 'in place' mate, whereas the others only have
mates, and their geometry comes from the original. Now i'll continue
working, adding say.. doors, a counter top, etc.. If at one point i
need to add a hole to one of these panels (and not just at the
assembly level, it needs to be in the part, since we CNC cut
everything and it only loads the part, not the assmebly). What would
be the best way of making that modification? Have i painted myself in
a corner? If i open my original panel, make a 'save as' and replace my
panel in my assembly with this new 'copy', i'll have likely lost my
external references, but at least i can add my hole without it
affecting the other 2 panels. This sounds incredibly iffy to me.. if
ever my bottom and back change shape.. this panel probably wont follow
the shape of the other panels.

Have i gone about it in the wrong direction from the start? what
should i change in my procedure to allow me to make these kinds of
changes in the future of the modeling process. This mostly happens for
holes i need for wiring, so i don't know where i need them until my
model is almost done. At the same time i don't want to create half a
dozen identical panels as separate parts if i don't have to, it's much
more efficient to know i have 6 x 24"x12" panels, than to know i have
1x 24"x12" named as part 1.. 1x 24"x12" named as part 2.. etc, all
being identical anyway.

Thanks for any insight into this. Dont be afraid to get technical,
i've been using SW for years, but i've never been able to wrap my head
around a procedure that would work in my situation without adding alot
more work.

Thanks

André Richard

 

can you just create separate configurations in the said part for your
holes?

search the help file for "Configurations and In-context Components."

 

Good question. I'll have to try that.

Actually, i think i can but i'll have to try it.. We use BOM's as a
cutlist and each part has their information (X, Y, thickness,
material, description) saved in some custom properties, i'll just have
to make sure for those parts that they use configuration specific
custom properties. I dont think i'd have any other issues.

When you mentioned configurations, my memory was jogged in that i
think i had tried it at one point, but i cant remember why we didn't
go ahead with it, there might have been some sort of technical problem
but i cant see what offhand.. seems to make sense that it would work.

Thanks,

André

 

Andre,

Use layout sketches where it is applicable, that way you don't lose the
references.

ca

 

Configurations are also a great solution, but you will need to learn a
whole new skillset, and be very very vigilant. SW has some odd rules for
how it treats references in configurations. And no, I can't explain the
rules either.

ca

 

You could try using insert-part as a way to share the common data...

example:... http://www.zxys.com/misc/insert_part_asm-zxys.zip

...

 

This might spart a debate...

Do NOT use part-to-part mates unless it is absolutely necessary.
Do NOT refer part geometry to other parts at the top level assembly.

What you should do it create top level reference geometry (sketches
and planes) that every part and sub-assembly in the assembly refers
to. This allows you to change, substitute or delete any part at any
time without the risk of anything in the assembly breaking. This
concept takes some getting used to and it does take more work to think
throught and setup the first time you do it, but it really works much
better than relating part features and mates to other parts.


-Martin