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Renaming parts and drawings

ptc-1413610
1-Newbie

Renaming parts and drawings

I know how to rename the parts, however, if I don't have the drawings associated with that part open when I change its name, the ProE seems to lose the part-drawing relationship.



Is this just something that I'm going to have to live with, or is there a simple fix for this?


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13 REPLIES 13

That's the way it works. Think about it this way - if you and a
colleague decide to change the name of the server folder project your
working on is stored in and I'm not there to hear the conversation,
there's no way I'll know where to look for the files if I need them.

If the drawing isn't 'in the room' when you change the name of the part,
there's no way for it to know that you did.

Doug Schaefer
--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Of course you need to have the drawing and assemblies in session
whenever you rename something.... But....

I have found that you have to do something to the drawing to force it to
actually save.

It is my finding in WF3 that simply renaming the part file, then saving
the drawing will not work. Even though Pro says it saved the drawing
and there may be a new file on disc it hasn't actually recorded the part
name change.

But when you switch to the drawing, do something, anything, move a dim
or a note or something minor to force a save and you'll be okay.

This only happens when I simply open a drawing and part, don't do
anything to the drawing, rename the part, save everything and exit or
erase. The drawing doesn't save the renamed part information. If you
have been working on the drawing all along, then there usually isn't a
problem because it is actually saving anyway.

I believe this to be a bug but I haven't bothered to report it.

Dave


Robert Steel wrote:
>
> I know how to rename the parts, however, if I don't have the drawings
> associated with that part open when I change its name, the ProE seems
> to lose the part-drawing relationship.
>
>
>
> Is this just something that I'm going to have to live with, or is
> there a simple fix for this?
>
>
>
cfly
4-Participant
(To:ptc-1413610)


Dave:

If you regenerate the drawing after the name change, it will find that its
associated object has changed and update its information. Then, you can save
the drawing and it will open next time with the newly renamed object.

Dave,

You might take a look at the config option' 'save_objects'.  I suspect
that you may have it set to 'changed' and Pro|E isn't seeing the drawing
as changed.  We have it set to 'changed_and_specified' (the default) and
have never seen this problem.

However, I would agree with you that it's a bug.  Pro|E should see the
drawing as changed if the model is renamed.

Doug Schaefer
--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Only if you are seeing this behavior after a regen though, you must regen
for the changes to take.

Brian S. Lynn
Technical Coordinator, Product Engineering

I don't believe this behavior existed in earlier versions of Pro. I've been doing this for years but it only seemed to become a problem recently.

I don't have a habit of regenerating drawings. If I switch to the drawing and it shows the correct part name at the bottom of the screen I figure it is looking at the new name and should be good to save, as it appears the drawing sees the change. And in the message area it does in fact tell me it saved. Otherwise I think I'd get the typical message "....has not been saved because it hasn't changed".

I don't think that regenerating the drawing is a requirement for this procedure. I can simply move a note on the drawing and it saves and remembers the new name just fine... I don't think that qualifies as actually regenerating the drawing...?? I think it just boils down to Pro/E lying to me... It says it saved... but while it may have written a new drw file to disc, it has not recorded any changes.

No big deal... I've learned to live with it. Regenerating is a good idea, maybe I'll start using that technique. But someone else who is not aware, might be getting burned by this. For the longest time I thought I was losing my mind. I would swear I saved all the drawings, but they wouldn't work. Finally one day I just took some time did some testing and figured out what was actually happening to me. At least it put my mind at ease a little; for a while I thought I was suffering from short term memory loss!

Dave



Brian Lynn wrote:
Only if you are seeing this behavior after a regen though, you must regen for the changes to take.

Brian S. Lynn
Technical Coordinator, Product Engineering

One way to verify that the drawing in fact did save would be to check
and see if the filename in the window title bar iterated.

Jeff Horacek
Sr. Designer
STERIS Corporation
440-392-7721 Ph.
440-392-8954 Fax
-

I have a question for other Pro-E users. I do not have the AAX (Advanced
Assembly Extension) module which is required for creating skeleton parts
used in top-down design. After working in SW, most SW users use an assembly
sketch for layout (i.e. skeleton) and assemble parts / sub-assemblies to
those skeleton assembly sketches.

Therefore, what advantage does a true skeleton part (using the AAX module)
offer over creating a part in Pro-E called "skeleton" (containing the
necessary sketches, planes, etc) and using it as a "skeleton" part in the
assembly? What is the advantage of a true skeleton part over creating an
assembly sketch layout and using the assembly sketch as a skeleton for
sub-assemblies?

Using multiple CAD systems, I find I want to standardize on common modeling
techniques when possible.


Chris

Chris,

There are not too many benefits to using an actual "skeleton" part over just
using a standard part that represents a skeleton. It is more of a
convenience factor in my mind (though since I have access to this
functionality, I do use them religiously). One of the main benefits which I
don't feel is such a big deal is that a true skeleton part is automatically
filtered out of a BOM report. No biggie. There is also the ability through
reference control to tell Pro/E to only allow references to the skeleton
part. Again, as long as you are careful when selecting references I don't
feel this is too important

I started using a standard part representing a skeleton long before PTC
incorporated skeleton functionality. As a PTC consultant back then I
recommended numerous times to add true skeletal functionality. Eventually
they listened, though probably not to me.

I feel there are many benefits to utilizing some sort of skeleton model,
whether real or not. Putting many of your critical product references in a
skeleton model allows you to use a combination of publish geometry features
in the skeleton and external copy geometry features in your individual
parts, having the parts point directly at the skeleton model (with no tie to
the assembly) for their information. This allows you to pull the skeleton
model into memory, make a change, and then pull up an individual part and
regenerate the part to see the changes. If you instead just create a bunch
of assembly features at the top level of the assembly which represent some
sort of skeleton geometry, it requires the assembly to opened up into Pro/E
memory (in some fashion), regenerate the assembly, and then regenerate the
part which is pointing at the assembly features. This can be a
time/graphics/memory issue in certain cases. Putting all of the
skeletal-type features into a single model (a skeleton part) consolidates
all of these features into one place to find/modify them. Again, if you
generate these as assembly features, they may end up being completely
interspersed among all of the assembled components in the model tree. I
would not consider this a very clean approach.

There are numerous other benefits to using a skeleton-type modeling approach
to top down design, but I feel what's mentioned above covers some of the
main reasons to consider this methodology. I hope this helps.

Best Regards,

Scott W. Schultz
Principal Consultant
3D Relief Inc.
3700 Willow Creek Drive
Suite 200
Raleigh, NC 27604
(919)259-0610
-

Hi Christopher,



I fully agree with Scott, and want to add some additional benefits :

- when working with a data manager (Intralink/Windchill), isolating your design intent into skeletons enables you to keep track of changes in a group of designers. A skeleton getting 'out of date' is giving another message than an assembly getting 'out-of-date'.

- we tend to reuse skeletons 'read-only' in assemblies, other than the original one. This way, we interchange the interfaces between assemblies.



Regards, Hugo.



In Reply to:

I have a question for other Pro-E users. I do not have the AAX (Advanced
Assembly Extension) module which is required for creating skeleton parts
used in top-down design. After working in SW, most SW users use an assembly
sketch for layout (i.e. skeleton) and assemble parts / sub-assemblies to
those skeleton assembly sketches.

Therefore, what advantage does a true skeleton part (using the AAX module)
offer over creating a part in Pro-E called "skeleton" (containing the
necessary sketches, planes, etc) and using it as a "skeleton" part in the
assembly? What is the advantage of a true skeleton part over creating an
assembly sketch layout and using the assembly sketch as a skeleton for
sub-assemblies?

Using multiple CAD systems, I find I want to standardize on common modeling
techniques when possible.


Chris


<< ProE WF3 M100 - PDMLink 8.00 M030 >>

GavinBRumble
5-Regular Member
(To:ptc-1413610)

Config.pro option: 'changed_and_specified' (the default).reiterated for
emphasis.



Because why would you ever want to push the button to Save "anything" and
have it NOT be saved? That's the "specified" part.ie, Save this object.



And to the original question: Easiest fix.have the drawing in session (but
agreed, we all have episodes of CRS). Work around for a failing drawing
(why can't Pro/E just say "Certain model not found.that view is deleted"
because sometimes you forget about when you Add Model for a part detail
view?) is to temporarily fool the drawing by placing a copy of the renamed
file in an "offline" directory (at the OS level) using the old name, open
the drawing, rename the model again, save the drawing, deal with the
duplicate model file whichever way is appropriate to save the most work. Of
course, upper level assemblies are not going to be happy about this
procedure.ie, you can't have parent assemblies in session.



Gavin B. Rumble, PE

Solid Engineering

336-224-2312






I understand why merge parts, assemblies, and drawings will not see the
name change if they are not in session, however, I would propose a
checkbox on the rename screen to search the current working directory
for references. At the very least, it would identify the references so
you could pull them into session. Optimally you could update and save
the files in question either one at a time or all of them. If you use
Intralink you do not have to deal with this issue since Intralink goes
out and updates the references. Consequently, we know PTC can do it if
they wanted to implement it.


Brian P. Costello
Manager, Development Engineering
-

Tyco Electronics Corporation 650-361-2339 tel
M.S. R33-01A 650-361-3373 fax
306 Constitution Drive www.tycoelectronics.com
Menlo Park, CA 94025



And technically they already implemented a tool to do it.

It is called Intralink or PDMlink, etc. 😉

You just wish they didn't charge extra for it. 😉



"Costello, Brian P" <->
06/18/2008 01:44 PM
Please respond to
"Costello, Brian P" <->


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Subject
[proecad] - RE: Renaming parts and drawings






I understand why merge parts, assemblies, and drawings will not see the
name change if they are not in session, however, I would propose a
checkbox on the rename screen to search the current working directory for
references. At the very least, it would identify the references so you
could pull them into session. Optimally you could update and save the
files in question either one at a time or all of them. If you use
Intralink you do not have to deal with this issue since Intralink goes out
and updates the references. Consequently, we know PTC can do it if they
wanted to implement it.

Brian P. Costello
Manager, Development Engineering
-

Tyco Electronics Corporation 650-361-2339 tel
M.S. R33-01A 650-361-3373 fax
306 Constitution Drive www.tycoelectronics.com
Menlo Park, CA 94025


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