&model_name

[dgschaefer]

if your note has a leader, and that leader is attached to an edge or
surface that belongs to the part in question (not an edge created by a
cross section, that edge belongs to the assy), then you can use the
following:

&model_name:att

The 'att' suffix tells Pro/E to look in the model that the note is
attached to. You have be certain that your note is attached to an edge
belonging to the model you want, however.

Doug Schaefer

[rollinsn]

Wow,

I was expecting to be reminded of something I used to know. Instead you
taught me something new...

Thanks Doug!

-Nate

[BobFrindt]

That's cool.
One I've never seen before.

Bob Frindt
Sr. Designer
Parker Hannifin Corporation
Parker Aerospace
Gas Turbine Fuel Systems Division
9200 Tyler Boulevard
Mentor, OH 44060 USA
direct  (440) 954-8159
cell: (216) 990-8711
fax: (440) 954-8111
-
www.parker.com



Doug Schaefer <>
05/11/2010 04:29 PM
Please respond to
Doug Schaefer <>


To
-
cc

Subject
[proecad] - RE: &model_name






if your note has a leader, and that leader is attached to an edge or
surface that belongs to the part in question (not an edge created by a
cross section, that edge belongs to the assy), then you can use the
following:
&model_name:att
The 'att' suffix tells Pro/E to look in the model that the note is
attached to.  You have be certain that your note is attached to an edge
belonging to the model you want, however.
Doug Schaefer
                                                 designet
6464 Presidential Gateway
Columbus, Ohio 43231
USA

[TedOtto]

You can show a dimension from the component you're searching for the ID for. Once the dimension is on the print, toggle the "switch dimensions" button and it should show the dimension name followed by the ID (example :2). In your note, use &model_name:2 and it'll pull the model name from that component. After you find the ID, you can then erase the dimension.

Thanks!
Ted

[rrich]

Is there something I am missing. This sounded like a great little feature
and I wanted to put it straight into practice but it is not working for me.
WF4 M100. I tried &model_name:att , I tried &MODEL_NAME:att but then my
note looks just like that. I tried on entity picking edges, I tried on
surfaces, I tried on item.







I wanted to use this for a simple instruction manual parts list.
Originally my plan was to use a BOM table and put balloons but that would
require a customer to have to cross reference from the number to the part
number. If I could easily add this type of note it would make this drawing
much simpler.



I have also tried it on a simple 2 piece assembly not exploded and I get the
same results.

Ron

[HugoHermans]

Exactly the same for me.

In addition, is it also possible to show a component model parameter on
an assembly drawing?

Met vriendelijke groeten,
Kindest regards,

Hugo Hermans

-

NV Michel Van de Wiele
Michel Vandewielestraat 7
8510 Kortrijk (Marke)
Tel : +32 56 243 211
Fax: +32 56 243 540
BTW BE 0405 450 595
RPR Kortrijk

[TedOtto]

I'm also not able to make the :att note work.

If you use the ID like I mentioned in my response, see below, you can use any model parameter and include the component ID to the note, and it should pull that parameter from the model you ID'ed.

Repsonse:
You can show a dimension from the component you're searching for the ID for. Once the dimension is on the print, toggle the "switch dimensions" button and it should show the dimension name followed by the ID (example :2). In your note, use &model_name:2 and it'll pull the model name from that component. After you find the ID, you can then erase the dimension.

Thanks!
Ted

[BobFrindt]

If I'm not mistaken, you must also add the model to the drawing.
You do not need a view of the component. just RMB this menu
then and
if you then create a note that says &model_name (or any parameter) Pro
will add a suffix to the parameter and it will look like this
&model_name:2 or &model_name:4 or whatever the assigned model ID is for
the active model.

HIH

Bob Frindt
Sr. Designer
Parker Hannifin Corporation
Parker Aerospace
Gas Turbine Fuel Systems Division
9200 Tyler Boulevard
Mentor, OH 44060 USA
direct (440) 954-8159
cell: (216) 990-8711
fax: (440) 954-8111
-
www.parker.com



Ted Otto <->
05/12/2010 09:36 AM
Please respond to
Ted Otto <->


To
Hermans Hugo <->, Ron Rich
<->
cc
"-" <->,
"-" <->
Subject
[proecad] - RE: &model_name






I?m also not able to make the :att note work.

If you use the ID like I mentioned in my response, see below, you can use
any model parameter and include the component ID to the note, and it
should pull that parameter from the model you ID?ed.

Repsonse:
You can show a dimension from the component you?re searching for the ID
for. Once the dimension is on the print, toggle the ?switch dimensions?
button and it should show the dimension name followed by the ID (example
:2). In your note, use &model_name:2 and it?ll pull the model name from
that component. After you find the ID, you can then erase the dimension.

Thanks!
Ted

[dgschaefer]

Hmmm, I've used this for a long time and I just tried it in WF3 and it
still works there. I'm wondering if there is a conflict here with the
PTC built in parameter for pulling the file name of a part (I assumed
that you were trying to pull a user defined parameter named model_name).
PTC uses the same syntax (&model_name) to pull the Pro/E file name.
Maybe that's causing the problem. I tried &model_name:att in WF3 and it
did not work, whether there was a user defined model_name parameter or
not, so I bet that's it. Try pulling a different parameter to see if
that works or changing your model_name parameter to something else, like
part_name.

Also, try using the syntax ¶meter:att_mdl. Pro/E will change the
:att to :att_mdl after you create the note, maybe :att no longer works
in WF4.

Doug Schaefer

[HugoHermans]

You can also set the filter to 'component' and right click on the model
:



Met vriendelijke groeten,
Kindest regards,

Hugo Hermans

-

NV Michel Van de Wiele
Michel Vandewielestraat 7
8510 Kortrijk (Marke)
Tel : +32 56 243 211
Fax: +32 56 243 540
BTW BE 0405 450 595
RPR Kortrijk

[BobFrindt]

Just checked, the :att or :att_mdl for user defined parameters and they
work fine in WF4.

The PTC parameter model_name does not.

Your suggestion to set up a user defined part_name or part_number
parameter should do the trick.

Bob Frindt
Sr. Designer
Parker Hannifin Corporation
Parker Aerospace
Gas Turbine Fuel Systems Division
9200 Tyler Boulevard
Mentor, OH 44060 USA
direct  (440) 954-8159
cell: (216) 990-8711
fax: (440) 954-8111
-
www.parker.com



Doug Schaefer <>
05/12/2010 09:48 AM
Please respond to
Doug Schaefer <>


To
-
cc

Subject
[proecad] - RE: &model_name






Hmmm, I've used this for a long time and I just tried it in WF3 and it
still works there.  I'm wondering if there is a conflict here with the PTC
built in parameter for pulling the file name of a part (I assumed that you
were trying to pull a user defined parameter named model_name).  PTC uses
the same syntax (&model_name) to pull the Pro/E file name.  Maybe that's
causing the problem.  I tried &model_name:att in WF3 and it did not work,
whether there was a user defined model_name parameter or not, so I bet
that's it.  Try pulling a different parameter to see if that works or
changing your model_name parameter to something else, like part_name.

Also, try using the syntax ¶meter:att_mdl.  Pro/E will change the :att
to :att_mdl after you create the note, maybe :att no longer works in WF4.
Doug Schaefer
                                                 designet
6464 Presidential Gateway
Columbus, Ohio 43231
USA

[DarrinHiebert]

I just verified this here as well, that a different parameter, like part_name works. We have always used &part_name, and not model_name. :att works, but Pro changes the note callout to &part_name:att_mdl when you're done. I don't know if it's a good practice to get into adding :att_mdl, or not, but currently either one works...

Verified on WF 2 and WF 5 (M030)...

[MartinBrown]

Hi All
I have yet to figure out how to touch a part in an assembly drawing and pull the "file name" into a note. You can pull a parameter value (we use a parameter called PART_NUMBER) by attaching a note &part_number:att - but this has been said already.

If you want the "file name" this is one way to get it, &model_name:(session_id)

The problem is getting the session id and this is a free floating note. It does not have to be attached to anything, but if you are careful you can get most of what you need by attaching the note to the right part in the drawing...

The session id may be obtained thru the relations window in a drawing.
TOOLS
RELATIONS
"look in" PART
select a part
SHOW
SESSION ID
PART
start selecting parts and write down the numbers on a paper copy of the same drawing.

Works well in WF4 M092

enjoy

Martin T. Brown
Design Specialist
Merrick & Company
Direct: 865-241-4642
www.merrick.com

[lylebeidler]

Just my 2cents.

I tried it in wf3, and model_name does not work, but any parameter does.



I tried &model_name:att and &model_name:att_mdl (and oodles of variations
with capitalization & not)



Neither worked.



It sounds like &model_name:att works fine for Doug, but not for me or Bob.

Could the difference be being linked to an Intralink session? Doug, are
you running linked to Ilink? How about you Bob? I am, and it's not working
for me.



However, if I find out the session id of the part, and create the note
&model_name:<session id=">, it works fine.



--



Lyle Beidler
MGS Inc
178 Muddy Creek Church Rd
Denver PA 17517
717-336-7528
Fax 717-336-0514
<">mailto:-> -
<">http://www.mgsincorporated.com>

[rrich]

All,

Facts and other stuff on this.

In WF4 M100

¶meter_name_of_choice:att produces ( parametervalue) of part
attached to. Note this parameter_name_of_choice must be a user created
parameter(not system parameter) located in the part you are attaching to.
However review of note after shows this ¶meter_name_of_choice:att _mdl
as Doug pointed out below. I tested this and it worked fine with a
parameter in my part called DESCRIPTION. Note showed proper description to
whatever part I was attached to. Changing the attachment point to another
part instantly updates the note.



PTC why doesn't this work with &model_name which is a valid system
parameter?



&model_name:place_ID_number_here produces (model name) of ID number you
placed. Possibly attached to the wrong part if you do not have the right ID
# for the part. This is not convenient if you have a large number of
components you have to guess at the ID or add dimensions and search for IDs.




Ron

[dgschaefer]

Actually, I got the same results as you. I had assumed on the original
question that he was referring to a user parameter, not a system
parameter. I didn't catch that it was a system parameter until later.

So, user params work, system params don't for me, same as you. 😄 Oh,
and I'm not on Ilink, so that's not a factor.

Doug Schaefer

[dustin]

I actually ran into a similar issue a while back. I was trying to create text that would be attached to the model. The model_name parameter was not sufficient automatically put the correct text in place. So I created a user parameter "NAME" as other's have suggested here, and then created a relation:

NAME=rel_model_name

With this format, you could use &NAME:att for your note, and you wouldn't have to update the user parameter "NAME" for each model. I only have one type of part setup this way, so most of my parts are not setup right for this.

[rollinsn]

Dustin,

This is a pretty easy solution. I am considering adding this relation
to our start part. Thank you.

Does any one know where the "toggle dims" button is in WF5?

confounded ribbon...

Thanks...

Nate

[rollinsn]

I found it -

Annotate > parameters > Switch dimensions

"RightUnderMyNose" syndrome...

Thanks all.

[GavinBRumble]

This :att secret has really tweaked my interest.just how long has this been
around?



By the way, there is an easy way to get the model name (filename) into a
user defined part parameter using a relation in your start parts.

Filename = rel_model_name()

This could obviously be "partnumber", "item_number", or whatever you like.



Inexplicably, this ALSO works:

model_name = rel_model_name()

.which means that I was able to override the system parameter. The drawing
note (&MODEL_NAME:att) was happy.



This works in WF3, WF4, WF5.



Gavin B. Rumble, PE

Solid Engineering

336-224-2312

[dgschaefer]

I know it was in WF2, might have been in 2001, I just don't remember
when I started using it.

Doug Schaefer