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
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: 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
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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

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: 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
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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:

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: 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
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[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
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