VOLUME NOTE ON DRAWING

[JMSCRA]

We are having a problem getting the volume note on a drawing to update with the changes to the part model.

The process we have followed is as follows:


1. Calculate the mass properties for the part
2. Create a string parameter called VOLUME
3. Write a relation: VOLUME = MP_VOLUME(" ")
4. Create a note on the drawing: volume = &volume IN@+3@#

This is reporting a value but it is incorrect as compared to the model

We are using WF2.0

Can someone offer a solution please?


John M. Scranton
Senior Designer
Ultra USSI
4578 E. Park 30 Dr.
Columbia City, IN 46725-8869
*Voice: 260.248.3576
*Fax; 260.248.3509
[cid:image001.jpg@01CA5883.522D21D0]


--
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.

[dgschaefer]

That should work. I'd add your relation in the 'post regen' section of
the relations (see the lower right corner of the relations dialog) so
that it gets evaluated after any geometry changes. Eliminates the need
for the double regen. You might also want to add the config option
mass_property_calculate automatic so that a new MP analysis is run
automatically.

Doug Schaefer

[blenk]

The config option mass_property_calculate automatic will fix this but has drawbacks. When an assembly is regenerated all models in the assembly will regenerate and show up modified even if they are at a Released state.

Our workaround is to go into your model, go Edit. Setup, Mass Props and hit OK.

This will make Pro/E recalculate the volume and it should be right when you go back to your drawing.

[dgschaefer]

Didn't know about the Intralink / Windchill limitation, that stinks. I
should have mentioned that this will obviously slow things down on regen
as well.

Doug Schaefer

[ScottCrowe]

Back when we upgraded to WF2,we found that the PRO_MP_VOLUME parameter eliminated the need for any relations; however, the Generate Report button in the Edit~Setup~Mass Props dialog box needed to be selected in order to sync the value you see on the drawing versus the value you would see from doing a model mass props via the Model Analysis. Not a particularly obvious solution to the problem. Regardless,

Our solution was to edit the Pro/Program in the start part (and edit exisiting parts as the opportunity presents itself) and include a line between MASSPROP and END MASSPROP at the end of the Pro/Program, for example if the part # is xyz it would be:

MASSPROP

PART xyz (Can be done w/ assemblies syntax is ASSEMBLY xyz)

END MASSPROP

The "xyz" updates fine with renames and save a copy.

We do not use the config option mentioned by Brandon for the same reasons he stated.

<u>Now, the drawback to the method I mentioned is that the UNDO functionality istoast after you regenerate (doesn't affect intent manager UNDO).</u>

Just use the &pro_mp_volume[.x] (x being the sig digits) in a note or in a format cell to report the value.

Other than the UNDO issue, it works fine.

In Reply to John Scranton:

We are having a problem getting the volume note on a drawing to update with the changes to the part model.

The process we have followed is as follows:


1. Calculate the mass properties for the part
2. Create a string parameter called VOLUME
3. Write a relation: VOLUME = MP_VOLUME(" ")
4. Create a note on the drawing: volume = &volume IN@+3@#

This is reporting a value but it is incorrect as compared to the model

We are using WF2.0

Can someone offer a solution please?


John M. Scranton
Senior Designer
Ultra USSI
4578 E. Park 30 Dr.
Columbia City, IN 46725-8869
*Voice: 260.248.3576
*Fax; 260.248.3509
[cid:image001.jpg@01CA5883.522D21D0]


--