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help with parametric notes

  • Thread starter richard.woodford
  • Start date
R

richard.woodford

Guest
Hi
currently i am using wildfire2
I have a drawing of a pressure valve. The release pressure of the valve is controlled by inserting different weights into a valve body.
I am now completeing the drawing, I would like to show the detail of each weight on seperate views - easy enough so far, with each view I also want to write a note - easy so far - in the note I would like to include the mass of each weight. I would like the weight to be parametric. I am fairly sure that some years ago I did a similar thing, I write a note that used the mass calculated by model properties. I have forgotten how to do this can anyone help
?

regards

Richard
 
Last edited:
K

kurtstark

Guest
From Pro/E Help:

To Reference a Mass Properties Symbol in a Note
You can create a parametric note that references a mass properties symbol. After the geometry changes, you can update the note to reflect the latest value of the mass properties parameter.

Set a user-defined parameter. For example: [volume].

Add a relation, assigning this parameter to a mass properties symbol that you want to reference in a note. For example: volume = mp_volume("").

Add a note containing the user-defined parameter. For example: [&volume].
 
R

richard.woodford

Guest
many thanks for the reply, i nearly had it!

hi i was putting in volume = 'mp_volume' as you point out i should use volume = mp_volume"")

many thanks

richard
 
J

jayafelix

Guest
HI ,
first you have to create parameters
volume
mass with realnumber variable.(by using parameter command)

then u have to give relation

volume=mp_volume("")
mass=mp_mass("")

here mp_mass("") and mp_volume("") bothe are calculated by system.
now we are assigning the value to your variable(volume and mass).

this all should be done at model.

now you have to retrive this to your drawing.
make a note &mass and &volume.

now you will get mass and volume which is calculated by model.

takecare

with love
felix
 
K

kurtstark

Guest
Part Parameter in Assembly Drawing

If you want to show a part-parameter in a assembly drawing you have to add the Session-ID to the parameter: &parametername:Session-ID
You can find the session-ID from the relation window with Show/Session ID in the opend Menu Manager: Part and select the part you want to know the session ID
 

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