I have created several weldments made of different PIECES and each
weldment becomes a single part. Then the parts are included in an
Now that it has come time to manufacture the unit, the company wants
drawings of each PIECE that went to make up each PART (weldment). They
didn't want this originally.
Is there any way to convert a multi piece PART into an assembly, so
that I can have each piece become a seperate PART?
Or is there a way to save each piece of the weldment as separate PARTS,
without redrawing everything from scratch again?
Fingers crossed and thanks
Can't help with an answer (don't think there's a good one) but thought it might
help if we were to determine if a PIECE is a part Feature and in essence you
want to know if there's a way to turn the individual features into parts or
otherwise be able to discretely detail each feature somehow (?).
A PIECE is a part of a PART.
it was decided early on that each complete weldment would be created as
a single part.
They didn't want individual parts to make up each weldment.
To make this clearer, if a weldment consists of several different
lengths of square tube, welded into a shape, then the complete weldment
would be the part and each square tube piece would be named pieces.
The original idea was to submit the idea for approval and individual
drawings were not needed. However, it has now been decided to use the
design and I was hoping to make my life easier by using the existing
models instead of creating everything from the beginning.
There are several weldments and each contains quite a few pieces.
I don't imagine that it is possible, but I was hoping that someone has
some ideas that can save me some time.
Jeff Howard wrote:
When I worked at Caterpillar, their tool design department used a LOT of
for making machining fixtures. Weldment pieces were parts that became a welded
component. The weldment, treated "like" a part was actually a Pro/e assembly.
Inside another assembly, everything becomes a component, so a "part's" origins
part or assembly, was of no concern to Pro/e. The weldment components were named
FX304-a, FX304-b, ....-c, ....-d, etc. With the dash numbers, the assembly could
be treated as a part ~ IOW, as a weldment. Yet, the welded pieces could each,
the sake of a cut table, be two sizes. With a feature added to represent
removed for squaring, you'd get the rough cut size; with that feature
you'd be able to assemble the part, in a configuration, as if it had been
machined. In the end, you got an assembly, with weldments of squared blocks; and
you got a cut table, with actual pieces of rough cut stock sizes, to show on a
weldment BOM. It was pretty neat and very effective in eliminating all the
ridiculous contortions you're going through. Part FEATURES into Parts!?! Copy
Geoms? or some other contortions? Don't be silly, just bite the bullet and model
the crap. The only thing at stake here is the vaunted reputation of whatever
shortsighted dumbass came up with this scheme in the first place. Purportedly,
he's got too bigga head to admit he made a horrible mistake and say it's time to
"rethink the old strategy". Hopefully, I'm way off base, 180 off the mark and
owing someone an apology. Maybe I've just seen too much dumbass crap in my life.
Or maybe I just lived long enough to tell the tale.
I guess that the answer to my original question is "NO, you will have
to start again".
I suppose that I knew that from the start. I was hoping for a short cut
but life (especially life with Proe) isn't like that. Anyway, thanks
for the replies.
David Janes wrote:
Guess we know now who made the decision to model it as it was done now, huh?
With any parametric / relational / history based modeler every decision you make
has consequences either limiting or enabling downstream operations. It's the
blessing and the bane of the systems. Learn them, learn to think ahead and use
them to your advantage.
Don't know if this'll help ya: Feature by Feature edit the section sketch
definition and save it to disk with a descriptive name. When you go to create
the new piece parts bring in the saved sections.
David's allusion to some sorta Copy Geom wouldn't be that bad. Place each
weldment into an assy, create new parts, project geometry, copy surfs, ..., etc.
You could even drive the new assy from the original part representation if you
do it right.
If it 'twere me I'd just do it over. Practice makes perfect and at this point
you don't want things to get too complicated.
Well, Jeff, since you opened Pandora's box, there's always the Master Model
* In part mode, figure out how you want your model carved up into parts;
* Add the geometry to facilitate that (usually consists of trimming surfaces)
* Trim away the unwanted surfaces, solidify them and save as Part_A
* Move the insert arrow up, pretend nothing happened previously and repeat for
Part_B (it may be nessary to create duplicate trimming surfaces where geometry
adjacent and contiguous.)
I've done this a few times, not the "easy way", and for good or ill, it retains
common CSsys for each of the parts. If you'd started this process in an
they'd still be there, in their original positions, married to that CSsys, no
other assembly constraints required/allowed. And that is precisely their
limitation as parts: they are slaves of the assembly and nothing exists ouside
their dependency to the original, master part. So, yeah, I could have said that
Pro/e provides these "workarounds" (read as "Pro/e is the Capital of the Kludge
Nation, the Sun of the Kludge Ethos, the Moon of the Kludge Soul, the Heart of
Kludge Psychology and the Backbone of the Kludge Movement: Long Live the Kludge,
May Your Fortunes Ever Wane!"). Not the simple remedy to splitting a single part
I second the motion. Why I didn't get into this in the first place.
The master part suggestion is not a bad one. You could also try two other
1) Make multiple copies of the parts you want to seperate giving each one a
different name. Then, either supress or cut (with a new feature) off the
unwanted sections. Once this is done you can assemble them all back
together in an assembly using only the default location.
2) Take the drawings you hopefully used for the proposal and make them into
line drawings. The best way to do this is probably to do a "save as" to
either .DXF or .DWG format and then import it back into Pro/Detail. Once
this is done you can use the drawing to create a Pro/Notebook, skeleton
model, parts and assemblies.
Although aproach 2 might take longer even than any of the other suggestions
(including starting from skratch) it might still be a good idea to use
Pro/Notebook anyway to help with future changes to the welded assemblies.
The way I look at it, if your customer changed how he wanted to do things
once what are the odds he won't change his mind again.
The original question resulted in several interesting options but as
most of you suggested, I started from scratch. It wasn't (quite) as
painful as I first imagined.
Thanks for the input.