Making Datum Targets in Models

[pauldelong]

In Part mode there is an option in Edit>Setup>Geom Tol>Make Target -- its greyed out. Does anyone know how to use this functionality?

All I can find is info on creating draft datum targets in the drawing... I'm sure they can be created in a model and shown/erased on the drawing, right?

TIA,

Paul

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[RaphaelCNascime]

Paul,

Datum targets are unsupported in 3D modes up to and including Wildfire
4.0. They are only supported as 2D items - hence the menu is grayed out
in Part mode.



In Wildfire 5.0, we added support for datum targets as 3D annotations.
You will find the new Datum Target Annotation Feature under the Insert >
Annotations menu.



Regards,

Raphael







Raphael Nascimento

Product Manager

Pro/ENGINEER Detailing

[ehill]

Unless this has been changed in the latest release of Pro/E, you can
only create datum targets in drawing mode. I thought I had written up a
guide on geometric tolerancing idiosyncrasies in Pro/E before, but I
can't find it 😞 Here's the quick version for datum targets.



Although it might be nice to be able to show target callouts in the 3D
model, Pro/E considers datum targets "draft datums" and therefore they
are only available in a 3D model. Datum points in the model are the
analogue in the 3D model, but the way to set it up is not very well
documented.

1. In the model, create datum points at the three target locations
(I name them "DTM_X_TGT_PNT" or something similar to identify their
purpose).
2. In the model, create a datum plane through the three "target"
datum points and make it a "set datum" with your datum name (e.g., "X").
You need a datum plane to be able to reference it in tolerance callouts.

3. In the drawing, create the datum target callouts by referencing
the datum plane and points from the model.



Best Regards,

[ehill]

Edit to original reply:



"...callouts in the 3D model, Pro/E considers datum targets "draft
datums" and therefore they are only available in a 3D model the 2D
drawing. "





Best Regards,