[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
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
the part so that if the part changes, the note value changes also. Here's how you
* 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
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
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
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
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
off, select 'Erase>Erase all'. When you want to see these notes in the drawing,
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
system when the part regenerates. I have CGS units set in my start part because
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
'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.