volume parameter

[bmozley]

ProE users,

I want to have a note on a drawing call out the volume of a part, such
that when the geometry of the part changes, the note would update.
How would you set up a parameter for volume, and add a relation,
assigning this parameter to volume?

Brad
WF 3, xp




This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[kim]

Hi
You can enter this in a note to get the volume:
&PRO_MP_VOLUME
And this for the mass:
&PRO_MP_MASS
If you want this to be updated automatically upon regeneration you need to set the following config.pro option:
mass_property_calculate automatic

I hope this helps
/Kim

[kdemont]

I have used &pro_mp_mass sucessfully. Currently I have been trying to get the principle moments of inertia to show but cant seem to get that to work. Any suggestions?

[cweigold]

I create a parameter called volume (a real number) then use the relation volume = mp_volume(")

[mwimberly]

If you go into the parameters dialog box, at the bottom where it says
"Main" change that to "Reported Mass Properties" you will see all the
parameters that are recorded when running a mass properties calculation.



Michael Wimberly

Engineering Applications Support Specialist II

Security & Survivability Systems



BAE Systems Land & Armaments

9113 Le Saint Drive

Fairfield, Ohio 45014 U.S.A.

(513) 881-4843 Direct

(513) 881-5087 Fax

(513) 881-9800 Main

-

[dgschaefer]

If you use a relation (Don't you have to use a relation? At one time
you couldn't display these system params on a drawing) make sure you put
it in he 'Post Regen' section of the relations dialog (see the drop down
in the lower right corner). That will avoid the need fro a double regen
to make sure the parameter is right.

Doug Schaefer

[kim]

In Reply to Brad Mozley:

Thanks for your help.
My part is very small , therefore the volume is a very small number. Is there a way to set the number of
places (at least 5) or set the answer in engineering notation?

Brad

Hi Brad
You can decide how many digits you want to have shown on the left side of the dot this way:
Volume: &PRO_MP_VOLUME[.0] mm³
Weight: &PRO_MP_MASS[.3] kg.
In this example the volume will be shown like this: Volume: 456987 mm³ and the mass like this: Weight: 2.698 kg.
It is also an option to either change the units in your part or use an relation to calculate another unit.
/Kim