Drawings of more than one part?

This may be a really dumb question, but I'll ask anyway:

Are you able to create drawing views of more than one part without
those parts being in their own assembly? For example, if I have a
plate and a set of screws that are a part of a larger assembly, can I
choose just those items for a drawing view, or do I have to choose the
entire assembly and hide everything else?

Hope this is an easy one. Thanks in advance...

Brian

 

No it's not a problem with bringing just one part into a drawing view.....if
You're in 2004 just add a new view and choose model from the opened
dokuments....or drag it in directly from FM design tree

Krister L

 

...
" ......
Are you able to create drawing views of more than
one part without those parts being in their own assembly?
........"

If you don't mind my tacking on a related curiosity
question: Assume a drawing in which several parts are
detailed. If somewhere along the way one of those parts is
renamed (assume drawing is not open at the time), how is
resolving the name change handled when the drawing is next
opened? Will the drawing open with missing views, frozen
views, not open until all references are resolved....?

 

It should just pop up the "Can't find the file..." box and allow you to
point to the renamed file.

WT

 

...
"It should just pop up the "Can't find the file..." box and
allow you to point to the renamed file."
----------------

Thanks, Wayne. If you chose to not resolve the link (can't
remember or someone else monkeyed with it) will the drawing
open with old views, missing views, not open? Just
curiosity; this always seems to be a problem when drawings
reference multiple files and it's understandably difficult
to find a "friendly" way to deal with the eventuality.

Is this common practice or do most people detail individual
parts in the assembly drawing or detail one part per drawing
file? This has probably been asked many times. Hope once
more isn't once too many. 8~)

 

If you

If you detail an assembly and pick a single part to create a view off of the
view will be of that part file if you then SaveAs or replace the part in the
assembly without the drawing opened the view will still reference the
origional part unless it is deleted or moved in which case it would ask you
if you want to locate the model (now that I think about it even with the
drawing opened if you do a replace part it will not update, though if you
SaveAs it will update the drawing with the new part). To update it you
would have to change the references or select the model for the view if
asked. If you choose not to locate the model the drawing will open up with
a crossed out view pane for every part that is not resolved.

We do the one part per drawing thing. If your company standards require you
to detail everything in the same drawing (which I am sure most in this group
would advise against) and you want views of detail parts to always be upto
date and change with assembly level part changes you will have to make a
view of the assembly and hide every part you do not want to see.

Regards,
Corey

 

Thanks, Corey.

 

We would have a few sheets for the Weldment drawing in a single drawing file
(we stadardize on A size sheets) and a BOM on the first of these sheets and
then have a separate drawing file for each "-XX" part. The advantage to
this is if you replace a part with a new one all you have to do is create a
new drawing file for the new part and the assembly drawing will update
properly the first time it is opened and saved. Also you will see marked
improvement on Drawing file speed I would say better than ten fold on larger
drawings.

Corey Scheich

 

ever consider the weldment feature (multi-body part)?

i'm considering this method for the next frame i have to do.

 

I apologize--I think I worded my question wrong...

What I mean is that I want a drawing view that contains two parts (or
three or four). Say I have a main assembly that has parts A, B, C, D,
E, F, G and H. I want to show parts B and C in one drawing view so I
can show how C attaches to B. Do I have to:

-create a subassembly of B and C, and create a drawing view of that?

or

-create a drawing view of the entire main assembly and hide all parts
except B and C?

or

-none of the above, & somehow select only parts B and C for the
drawing view?


Does that clarify my question? Thanks...

Brian

 

one word, configuration

 

you got it brian?

create derived config , hide unwanted parts
insert main assy view into drawing,
select view and rmb,
properties,
change config
done

 

Probably two words, Derived Configuration. Then it is always the same as
the main config except for all the supressed parts.

 

I considered it briefly we don't do structural weldments too often but I
used it to create one of our current weldments which are mostly irregular
trailer frames. Anyway it wasn't for production. I was able to build the
frame quickly and easily. Though the method I would take now is to create
the frame as a single part and use the split command to create the individal
part files for the structural members and also to create an assembly. This
way I could easily manipulate changes to the overall frame and update each
piece drawing at once. This works best for our company since we require
each piece of a weldment to have an individual part number. The split
command also allows you to save out identical bodies to the same file. (Be
careful though because mirrored parts are not checked well enough to be sure
they are identical. I have an SPR out on that one.)

regard,

Corey Scheich