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Without more details on what you've tried already...
Insert this into your note: &pro_mp_volume
In Reply to John Scranton:
OK I give up! ;^(
I am trying to create a note on a drawing that displays the volume of the part that drives the drawing.
I have tried a number of things with no luck.
Please help.
WF5.0 & PDMLink 9.1
John M. Scranton
Manager Design Drafting
and Configuration Management
Ultra - USSI
4578 E. Park 30 Dr.
Columbia City, IN 46725-8869
*Voice: 260.248.3576
*Fax; 260.248.3509
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Ever see a post where someone mentions a feature not working as expected then wonder how many people scramble to test it out themselves?
Anyway, a couple of quick tests leads to the following...
Adding to what Doug mentions in his post, leaving 'mass_property_calculate' set to 'by_request' leaves only one way to get the note to update (that I found in a quick test). After the model changes and has been regenerated, you have to go to Edit > Setup > Mass Props and pick Generate Report. Doing so forces a note using &pro_mp_volume to adopt the new value.
The best option is to use the analysis feature Doug outlined.
In Reply to John Scranton:
Setting the option 'mass_property_calculate' to 'automatic' does work but then we will be calculating mass properties every time a change is made on every part. That does not sound like that is making good use of resources. In fact if my memory serves me correctly I had the option set that way some time ago and changed it because of the problems that caused.
The issue here is that with the option set to "by request" it does not update the note or table no matter how many times things are updated or regenerated or the mass properties are calculated. Do we have a bug in WF5.0?
John M. Scranton
Manager Design Drafting
and Configuration Management
Ultra - USSI
4578 E. Park 30 Dr.
Columbia City, IN 46725-8869
*Voice: 260.248.3576
*Fax; 260.248.3509
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Mike mentions (in the quoted reply) there might be a way to get that into a drawing note.
There is a way to get material parameters into a normal note. (Note these instructions are for WF4.0)
These take place after creating a parameter in the material as per Mike's instructions.
1. PickTools > Relations.
2.Pick the 'Insert Parameter Name from List' icon. (It looks like a pair of parentheses.)
3. Change the 'Look In' pull down menu from Part to Material.
4. Select the material and pick the OK button.
5. You can now see the parameter you added to the material per MIke's instructions. Select it and pick the Insert Selected button.
Your relations will display the string necessary to enter the value into a note. Something similar to
Go to your material library and add a user defined parameter to a material (I just created one called WEIGHT_UNIT), gave it a Description of Pounds, and set the Unit to lbm
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Create a repeat region in your drawing format and select "mdl.param.unit" in the cell. When you change the units in your model the repeat region value will automatically update the next time the drawing is opened/updated
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Might be a way to capture that in a drawing note (haven't figured that one out yet) but at least you could capture the mass units of your part in our drawing format
My 2 cents 🙂
Mike Brattoli
Moen Incorporated
Global Strategic Development
Engineering Systems Administrator
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