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displaying mass property info

sherbert

New member
Is it posible to display mass proprety info in the form of a note on a drawing? I am trying to display the area of a surface, that has an irregular outline.
 

xcad

New member
Hello



In part mode click Analysis>Model Analysis> Model Mass Properties > compute.

Go to : Relations > and write down this sentence : AREA = MP_SURF_AREA () for a surface measure of the model or : WEIGHT = MP_MASS ()

If the system asks you to recalculate the values recalculate them untils the software accepts the relations

Make a drawing of this part and Insert > Note

THE WEIGHT OF THE PART IS &WEIGHT SQUARE UNITS

THE TOTAL SURFACE AREA IS &AREA



Something for the expert users : you can see that the software automatically when we create the relation as I described above creates a parameter AREA (real number) or the parameter WEIGHT. Access the parameters to see it yourself. That is why when we create the parametric notes in the drawing the software finds the parameters &AREA and &WEIGHT.

Very efficient this option, well done quys from PTC



Try it yourself and reply me your comments



Karavasilis Christos
 

proed

Moderator
In addition to xcad's good info:



To measure a particular surface



- Analysis > Measure > Area

- Select the surface

- This will give the value

- Click the Add Feature button

- Enter the name (say: Analysis1)

- In your relations, add:



surf_area=area:FID_Analysis1



Where surf_area is your parameter name, FID means Feature ID (or something), Analysis1 is the feature name.



Then add a note:

Surface area = &surf_area



(Notes - this may require certain special Pro/E modules to add the Analysis feature. Also, it'll usually require a regen after changes to get the correct value.)



Merry Christmas

Ed
 

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