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dgschaefer21-Topaz II
21-Topaz II
May 11, 2010
Question

&model_name

  • May 11, 2010
  • 20 replies
  • 9576 views
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

20 replies

R
rollinsn1-Visitor
1-Visitor
May 11, 2010
Wow,

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

Thanks Doug!

-Nate

B
BobFrindt1-Visitor
1-Visitor
May 12, 2010
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

T
TedOtto3-Newcomer
3-Newcomer
May 12, 2010
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
R
rrich1-Visitor
1-Visitor
May 12, 2010
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


H
HugoHermans12-Amethyst
12-Amethyst
May 12, 2010
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
T
TedOtto3-Newcomer
3-Newcomer
May 12, 2010
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

B
BobFrindt1-Visitor
1-Visitor
May 12, 2010
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

D
dgschaefer21-Topaz IIAuthor
21-Topaz II
May 12, 2010
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
H
HugoHermans12-Amethyst
12-Amethyst
May 12, 2010
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
B
BobFrindt1-Visitor
1-Visitor
May 12, 2010
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

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