Part and Assembly weight

I was wondering if there is a way to automaticly calculate the weight
of a part and enter it into a drawing. Also the part could change and
so could the weight. How can I make this work? Any help is greatly
appericated.

Thanks in advanced,
Darrell

 

I have a macro that allows the user to select a drawing view and a block
that we use to display the weight, and then go get the mass of the displayed
configuration and paste that value into the appropriate note in the block.
When I wrote it, I put in the ability to paste in the English value, the
metric value, or the property. But at the time, there were issues with
precisions and units and who controlled what, that didn't allow the property
scheme to function well, and I haven't tried it since due to lack of time.
It might be of some help to you - free for the asking.

WT

 

In the part:

Go to File > Properties > Custom Properties
In the Property Name field select the Weight option (it's a pulldown
menu)
In the Value / Text Expression field, hit the pulldown and select Mass
- this will pull the "" variable
Close out of the box
No go define a material in the FeatureTree and then check the custom
properties again. You'll both values are now updated. If you change
the material in the FeatureTree again, they'll keep updating.

On the drawing:

Either edit the sheet format or just insert a note
While editing the note, select the Link to Property button (should be
right below the angle - it's a paper, with a hand and a yellow chain
link)
In the next dialog, select Model in view specified (3rd down)
the in the pulldown you will see Material, Weight and any others you
created in the part custom properties.

Again, if you change the part material, the drawing will update when
it's opened again.

Enjoy,

Steve O