Insert 3 default datums before first feature

[davehaigh]

I pulled up an old part that has no features other than a single protrusion. It has references to an assembly that no longer exist. I can't break the references unless I can reroute the sketcher orientation picks.

I know this used to be possible. Don't know how in Creo. Anyone?
[cid:image001.png@01D07D19.9C0D8310]

David Haigh
Phone: 925-424-3931
Fax: 925-423-7496
Lawrence Livermore National Lab
7000 East Ave, L-362
Livermore, CA 94550


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[iceblink1]

I don't know if this is the most proper way to do it, but you can model
the datums after the feature (#model; #datums; #offset_planes). Then
afterwards drag the feature so it is after the datums.

Best regards,
Patrick

[KenFarley]

Seems like if it's just a single protrusion, you could "Redefine" it, get into the sketch, save the sketch in its own file. Then start up a new part, create a protrusion feature, then import that saved sketch. It'll likely be dimensioned crazily with whatever screwball scheme Creo decides, but you can fix that and move on.

[dgschaefer]

1. Create a default CS.
2. Reorder the CS before the protrusion.
3. Drag the insert line ahead of the protrusion.
4. Click the plane button and you should get the default planes.

--

[SimonLucas]

Here is another way:

• supress everything i nthe model


• create default datum csys


• create default datum planes


• resume everything


• re-order everything after planes.

In Reply to David Haigh:

I pulled up an old part that has no features other than a single protrusion. It has references to an assembly that no longer exist. I can't break the references unless I can reroute the sketcher orientation picks.

I know this used to be possible. Don't know how in Creo. Anyone?
[cid:image001.png@01D07D19.9C0D8310]

David Haigh
Phone: 925-424-3931
Fax: 925-423-7496
Lawrence Livermore National Lab
7000 East Ave, L-362
Livermore, CA 94550

Simon Lucas