Skip to main content
ptc-38891751-Visitor
1-Visitor
July 25, 2012
Solved

Getting part weights to show up in title block

  • July 25, 2012
  • 8 replies
  • 23812 views

Does anyone know how I can get a mass property weight to show up in a title block? I'd like to see the part weight show up in the drawing, and potentially see the full weight of an assembly printed in the title block as well.

Any assistance is greatly appreciated!

-john


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.
Best answer by ptc-3889175

Thank you so much! Awesome!

8 replies

KshetrabasiMaha1-Visitor
1-Visitor
July 26, 2012

Hi

There is a system parameter for it pro_mp_mass

There are two ways for getting it in drawing

1.Use it in a part/asm template relation

eg- Weight=pro_mp_mass

and use Weight parameter in drawing format table(title block table) as &weight

2.Directly use this in drawing format table(title block table) as &pro_mp_mass

You can reduce decimal places by using &pro_mp_mass[.3]

But remember to set one config option

mass_property_calculate automatic

By setting this value system will automatically calculate wt upon regeneration.

Regards

K.Mahanta

ptc-38891751-VisitorAuthorAnswer
1-Visitor
July 26, 2012

Thank you so much! Awesome!

Patriot_1776
Patriot_177622-Sapphire II
22-Sapphire II
July 26, 2012

Be careful using:

mass_property_calculate automatic

It means the part or assembly is automatically regenerated a lot, marking the files as changed in Windchill, causing issues on check in. After using that setting, and encountering problems, I think a better setting is:

mass_property_calculate by_request

This means it's only done when you do a mass prop in the model. Then just update your dwg and it's fine.

    BrianMartin13-Aquamarine
    13-Aquamarine
    July 27, 2012

    I would agree with you, Frank.

    Even though the automatic setting may be convenient, it usually causes more headaches than it solves. I prefer keeping mine set by_request and taking responsibility for making sure the drawing is updated. Honestly once you've run the mass props calculation ONCE, I find I don't have to bother checking to make sure the drawing is updated- it's just done automatically.

    Two things I would add to Kshetrabasi's post...

    I would move the relation weight=pro_mp_mass into the "Post Regeneration" area of the relations. This way the weight is calculated after any dimensional changes to the model are incorporated. This prevents the dreaded "double-regeneration" problem and insures your weight parameter is always correct. See below...

    relations.png

    The second thing is to always make sure you've generated the mass properties report at least once by hand if you're using by_request. In Wildfire 5, go to File->Properties->Mass Properties and select Generate Report. In Creo 2, go to File->Prepare->Model Properties to access the Generate Report button. You must generate the report manually one time before your mass properties values will update.

    This sounds like a pain in the neck and a good reason to choose automatic, but I still believe there are more downsides to using automatic than the slight inconvenience of running an initial mass properties report.

    Thanks!

    -Brian

    Patriot_1776
    Patriot_177622-Sapphire II
    22-Sapphire II
    August 2, 2012

    Yep, what Brian said!

    We don't use it here much, but when I was working for the INL I designed large weldments, and we needed to know weights and CG's for the riggers (crane).

    Terms & ConditionsAccessibility statement