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Change driving surface on sheetmetal part...


Change driving surface on sheetmetal part...

I have a user here that would like to switch a sheetmetal parts driving
surface to the other side, basically, flip white and green sides on
first feature. The first feature is a flat wall, and not an extruded
wall. I've never had a need to do this before, and I couldn't find a
way to do this. Is it possible?

WF 2.0, M170...

Darrin Hiebert
Excel Industries
Hesston, KS


How to put "mass properties" into a drawing


Is it possible to have the "mass properties" report in a drawing such
that as the design changes the values will be updated? If so how? I am
interested in the mass and volume values.


SUMMARY: Change driving surface on sheetmetal part...

First off, thanks to everyone who responded!

Also, to anyone on WF 3.0 or greater, this is really simple. There's a
direction change button in the dashboard, and clicking that button will
flip green to white.

For us poor suckers that are on a prior revision (us included), this can
be done, but it's a little more tricky.

You need to change/redefine your sketching plane. While in there, you
need to reselect your sketching plane, and you will be presented with a
"FLIP" option. Choose flip there, and then sketch as normal. This will
flip the white to green, or vice-versa. Several users told me to do
this, and I tried this several times, and I could not get it to work.
The key to making this work is that you need to actually reselect the
SAME sketching plane, and then you will get the flip option.

Also, be very careful when using this either of these methods. While
this is an option, it can hose up some of your downstream walls, forms,
etc. You may also have to reselect edges if you want walls flipped in
the opposite direction, and again, that may hose up some of your
downstream operations...

SUMMARY How to put "mass properties" into a drawing

Summary Below ( a few methods)

I think the key is the option

mass_property_calculate automatic


Here are steps that I know of, which work for us.

Wf2 .prt / .drw attached.

In have parameter mass_property_calculate set to "automatic"

In our part / assembly relations we have this line:



On the drawing we just put &weight into a note.[see attachments]


Create an Analysis feature and put it in the footer of your part, with
the appropriate relations and parameters. By placing it in the footer
every time the part regenerates the values will be automatically be
updated. Attached is a copy of our default template part with
everything setup for your reference. I included images of the part
parameters and drawing relations for your reference. We have parameters
in our drawing title block for estimated weight, volume, and surface
area in English and metric units.

Works great! Let me know if you have any questions

We're using Wildfire 3 but it also works with Wildfire 2[see attachemnts]


In my parts and assemblies I have a post-regeneration relation, mass =
Then in the drawing I make a note &mass.
It will update on a regenerate.

Caution - behavior with family tabled components with instances with
differing densities can be problematic.


SUMMARY How to put "mass properties" into a drawing


One thing to keep in mind when settiing the config option mass_property_calculate?to "automatic".

Depending on the size of the assemblies you are working with, you might want to have each Pro/E user place the config option in their personal rather than settinig it in the system

This option can seriously extend regeneration in large assemblies.

Try the setting in your config first pull the TLA and test the regeneration before changing the system config. Make a few simple changes and test your times.