note on drawing

Hello Pro/E Gurus!

I am using ProE 2001 (DateCode:2003320), and I would like to create
on a drawing a special kind of note. I have an asm as model of the
drawing, and I'd like to attach the note to a component, and a note
will be the name of the component, I have already used the following:

&model_name:att_mdl

,but it doesn't work. With other parameters (user defined params) it works:

&PARAM:att_mdl

PARAM is a user defined parameter, but how can I use the system
parameter?
Anybody has an idea?

Thanks,

Peter Bo

 

: Hello Pro/E Gurus!
:
: I am using ProE 2001 (DateCode:2003320), and I would like to create
: on a drawing a special kind of note. I have an asm as model of the
: drawing, and I'd like to attach the note to a component, and a note
: will be the name of the component, I have already used the following:
:
: &model_name:att_mdl
:
&model_name is already a system parameter. If you have created a parameter with
this name, delete it. Also, you don't need to follow this system parameter with
:att_mdl. As with drawing notes and table parameters, it will pick up the value of
whatever model is active. Before adding hte format or creating the note, go to
'File>Properties>Drawing Models and Set Model (or Add Model, if it is not already
on the list of available models; remember, just adding the assembly doesn't add
all of its models).

David Janes

 

Thank you David, it works perfectly, after to create the note, ProE put
a number after the parameter automatically, it seems as member ID of the
asm, but in the model tree there are other numbers.
Where are these number from? It would be good, if I could print a list
with this numbers: which number is which part, then I could wtrite the
numbers manually after the parameter. How about it? Can ProE do such list?

Thanks
Peter

 

: Thank you David, it works perfectly, after to create the note, ProE put
: a number after the parameter automatically, it seems as member ID of the
: asm, but in the model tree there are other numbers.
: Where are these number from? It would be good, if I could print a list
: with this numbers: which number is which part, then I could wtrite the
: numbers manually after the parameter. How about it? Can ProE do such list?
:
: Thanks
: Peter

The Info menu will tell you a lot about your assembly and models. 'Info>BOM' will
give you a break down of all the subassemblies and components in your assembly.
'Info>Model' will give you a similar list, one entry per part. These can be
printed. Also, with 'Info>Save Model tree', the tree with all the column
information and column headings will get saved to a file called Treetool.txt which
can be opened and printed. If you would like to see additional information,
including parameters, shown in the Model Tree, go to 'View>Model Tree Setup>Column
Display'. This lets you select from several menus of things that can be displayed
in the Model Tree. Besides the Info items, there are also Parameters and several
others.

Just curious ~ what do you need all these numbers for? You started by mentioning
&model_name:att_cmp. We got that straightened out, but even the correct useage of
<param_name>:att_cmp doesn't require any numbers. The :att_cmp postfix merely says
to Pro/e to look in the component the note is attached to for the value of the
&parameter referred to. There is also an att_edge, att_mdl, and att_feature which
say respectively, look in the note's attaching edge, attaching model or attaching
feature for the parameter value referred to by &parameter. Because the note has a
physical attachment, there is no need to refer to component numbers. But, when the
note is attached to an edge, Pro/e needs to know whether to take the parameter
from the edge or the feature the edge is part of or the model the edge and feature
are part of or the component all of them are part of. The :att_ postfix tells the
program at what level to start looking for the parameter.

David Janes

 

Hi David,
I just wanted to create notes on a drawing, which contains the name of
the part and a parameter which is the weight of the part. I did it so,
that I made a parameter for the weight in the part: (weight : real
number), this parameter I can get on the drawing in a note so:

&weight:att_mdl
(_mdl is not neccesary, system puts it after automatically)

and in the help there is nothing about the system parameter in note.
Therefore I thought that the part name I can get so:

&model_name:att_mdl

but it doesn't work. I realized that only user parameter can I get on
the drawing in a note. So first I made in the part a parameter
(part_name : string) and a relation also:

part_name=rel_model_name

But it is not suitable for me, because we have a lot of standard parts,
wich I can not modify. So it is better if I do what you told me, but
it is a bit hard to do befor each note creation to set model. So I
tought, if I could make a list with the number of the notes, which
ProE puts after the parameter automatically, it would be good. So
I could save a little time, I don't have to do the set model. I attached
the note to the part on surface. So the level is the model level, so
ProE puts _mdl after it. I am going to try to make such a list with the
numbers, today I didn't have time to do this, but tomorrow...

Thank you David and sorry for my bad English!

Peter Bo

David Janes:

 

: Hi David,
: I just wanted to create notes on a drawing, which contains the name of
: the part and a parameter which is the weight of the part. I did it so,
: that I made a parameter for the weight in the part: (weight : real
: number), this parameter I can get on the drawing in a note so:
:
I found another way to do this that I think is much better. You don't create any
parameters, you don't create any relations. You just add one feature at the end of
the part and then create the note on the part, based on this last feature. The
nice thing is that the note is parametric: it shows the calculation of the mass of
the part so that if the part changes, the note value changes also. Here's how you
do it:

Preliminary step
Go to 'Edit>Setup> Units to make sure that the units are the same for each part
and the assembly
Then make sure the density value is set with 'Mass props'

Make last feature
Do 'Insert>Model Datum>Analysis' to make an analysis feature. Click the radio
button for Model Analysis then click Next
Click compute and Close which gets you back to the Analysis parameters.
Under Result params, you'll find a list of parameters, based on the computation
that can be turned into local analysis feature parameters. The one you are
interested in is MASS, so highlight this line and click the radio button for Yes
to create this parameter.
Click the green check mark for okay. Now you'll see a new feature in the Model
Tree called ANALYSIS1. You can name this anything you want.

Make parametric note on part
With ANALYSIS1 highlighted in the model tree, RMB over it and go down the list to
'Setup note>Feature'
In the box headed Text, write your note using the parameter for mass you just
created as follows:
Weight is &MASS:FID_ANALYSIS1 gs. (Capitals for identification only)
You could even add, as a second line
Model name is &Model_name (This will pick up the file name of part or put
another parameter in here that you've already created)
Click Place and select Note type/Done and Attachment type, click on part
somewhere, click in empty part of screen to place note and Done/OK
The mass property value for mass will be substituted in the note for
&MASS:FID_ANALYSIS1.

As you go through your parts this way, you will see these notes turning up in your
assembly, as well. If you wish to turn off the display of the notes or edit the
text or delete a note, go to 'Edit>Setup>Note'. To turn the display of all of them
off, select 'Erase>Erase all'. When you want to see these notes in the drawing, go
to 'View>Show and Erase', pick the notes icon, pick 'By part and view' and start
picking components. Or do 'Show all' and switch them from one view to another.
When you are done showing them, you can select them, move them around or modify
their attachment as you do any other note.

David Janes

 

[same as previous post with some additonal points and better formatting]
: Hi David,
: I just wanted to create notes on a drawing, which contains the name of
: the part and a parameter which is the weight of the part. I did it so,
: that I made a parameter for the weight in the part: (weight : real
: number), this parameter I can get on the drawing in a note so:
:

I found another way to do this that I think is much better. You don't create any
parameters, you don't create any relations. You just add one feature at the end of
the part and then create the note on the part, based on this last feature. The
nice thing is that the note is parametric: it shows the calculation of the mass of
the part so that if the part changes, the note value changes also. Here's how you
do it:

Preliminary step
* Go to 'Edit>Setup> Units to make sure that the units are the same for each part
and the assembly.
* Then make sure the density value is set with 'Mass props'.

Make last feature
* Do 'Insert>Model Datum>Analysis' to make an analysis feature. Click the radio
button for Model Analysis then click Next.
* Click compute and Close which gets you back to the Analysis parameters.
* Under the Result params heading, you'll find a list of parameters, based on the
computation,
that can be turned into local analysis feature parameters. The one you are
interested in is MASS, so highlight this line and click the radio button for Yes
to create this parameter.
* Click the green check mark for okay. Now you'll see a new feature in the Model.
Tree called ANALYSIS1. You can name this anything you want.

Make parametric note on part
* With the ANALYSIS1 feature highlighted in the model tree, RMB over it and go
down the list to 'Setup note>Feature'
* In the box headed Text, write your note using the parameter for mass you just
created, as follows:
Weight is &MASS:FID_ANALYSIS1[.1] gs. (Capitals for identification only;
decimal value in brackets sets number of decimal places shown which ranges from .0
for a rounded integer value to .14)
You could even add, as a second line,
Model name is &Model_name (This will pick up the file name of part or you can
put another parameter in here that you've already created).
* Click Place and select Note type/Done and Attachment type, click on part
somewhere, click in empty part of screen to place note and Done/OK. The mass
property value for mass will be substituted in the note for &MASS:FID_ANALYSIS1.

As you go through your parts this way, you will see these notes turning up in your
assembly, as well. If you wish to turn off the display of the notes or edit the
text or delete a note, go to 'Edit>Setup>Note'. To turn the display of all of them
off, select 'Erase>Erase all'. When you want to see these notes in the drawing, go
to 'View>Show and Erase', pick the notes icon, pick 'By part and view' and start
picking components. Or do 'Show all' and switch them from one view to another.
When you are done showing them, you can select them, move them around or modify
their attachment as you do any other note.

Another nice thing about doing this parametrically is that you can reset your
units of measure to another system and the value in MASS recalculates with the new
system when the part regenerates. I have CGS units set in my start part because it
is the most convenient for setting density. In CGS, 1 cc of water = 1 g. so you
can use the widely available values of specific gravity for density without
worrying about the thousand different ways that density can be expressed and
trying to translate between them.

If you would like to systematize this, use it frequently and do it efficiently,
set up the analysis feature and the parametric note (probably 'Note Type>No
Leader') in your start part, then slide the Insert bar above it. When you've
finished your last feature, slide the Insert bar below the analysis feature and do
'Edit>Setup>Note>Show>All' to see the contents. You may wish to attach the note
with a leader so go to 'Edit>Setup>Notes>Modify'. Pick Mod Attach, select On
entity or On surface and pick a place on the part to attach the note. Do it once
in the start part and with a couple quick steps at the end, there's your part
weight in a note.

David Janes