Reassign 0-0 for Ordinate Sims - CREO 10

Are you creating dimensions on a drawing rather that showing model dimensions? It is almost always better to dimension to a centerline in a sketch that is constrained coincident to sketch geometry so that later one can move the centerline and therefore the baseline of the dimensions as required.

Anyway, try some of the suggestions here:

Applying ordinates in the drawing - not at part level. Yes, I understand at model level and bringing them into the drawing is the preferred way. The link you posted from PTC forums is a workaround if you lose a reference - this happens often in CREO. So yeah, it would be nice to reassign - or reattach a broken 0-0 reference. I posted on PTC's forums as well.

This has been going on since 2015 (from the link you posted). How can this not be fixed???? It's standard edit and update. NX and SolidWorks allows for editing the origin and automatic update once reassigned. CREO - you have to delete the whole string. Unless someone here can tell me different. If you do I would be greatly appreciative. I looked high and low.

Used Creo (and Pro/Engineer) for 20 years and never just "lost" a reference. Had people do a bad job of redefining or just deleteing and recreating features because they didn't know or didn't care and then blame the software for doing as they asked.

I don't know that I ever went into a design without a plan so I never had to re-baseline a dimensioning scheme, but planned for it with the model dimensions.

A drawing that has one scheme on the drawing and a different one in the model is twice the work.

It's possible to extend the model problem to the created dimensions by creating a datum plane in the model to be used as the origin of the created dimensions so that the datum plane can be redefined to relocate the origin.

3D this is something I will look into as a solution. I still think a better solution can be implemented. You can click on any chain ordinate Dim and redefine - just add 0-0 as well.

I haven't looked into this - but you say when you start your detailing things never change. I have a different experience. I believe a simple modification to the 0-0 face causes the reference to be lost (I think the 0-0 turns red or purple). If you, for whatever reason, remove the first ordinate dim feature in a chain the whole chain falls apart. There is no recovery from that. The kludge of a fix proposed as far back as 2015 is unacceptable. Just allow for redefinition of all dims in an ordinate chain. Boom done. This feature just seems logical.

3D someone else proposed you solution on the CREO forums, but they even went so far to state that the datum plane CANNOT reference the surface for Datum because the same issue presents itself - if for whatever reason the surface is modified the reference for the Datum plane will fail. I will play with this.

The key is that PTC is Parameteric Technology, not drafting technology. NX traces back to when drafters were the primary user of the product and SolidWorks is SolidWorks.

What "simple" modification? Deleting a feature and then creating a new feature that is nearby or redefining a feature and using the replace function to keep the references?

I started at Rev 12 and continued to Creo 3 or 4; I forget which the last one was. Models I made 20 years before still functioned correctly, not a hitch. Also avoided created dimensions like the plague. They are fine for non-parametric parts - imports of IGES and STEP, but why design one dimensioning scheme in the model and use an entirely different one on the drawing? It means that instead of a change to a single dimension as expected, one might have to change 100 because the drawing dimension origin is changed and check all the other drawing dimensions.

I think some users liked to do that so they could pad their time and claim that Pro/E was very complicated; usually hourly contractors stretching their contract fixing what they designed to be broken. Sometimes they were NX users who would have been more productive with a drafting machine on a drawing board.

It worked out best for me to dimension between non-solid and surface geometry generative references: Datum planes, datum curves, sketch centerlines, and so forth and then just align the generative geometry to the non-generative geometry. This is very handy for your case - often one can redefine the sketch and drag and drop the references as desired and the generative geometry comes along for the ride and dimensions remain intact, expecially nice if there is late decisions about use of cylindrical holes or slots. The locating dims are to the centerline sketch.

3D someone else proposed you solution on the CREO forums, but they even went so far to state that the datum plane CANNOT reference the surface for Datum because the same issue presents itself - if for whatever reason the surface is modified the reference for the Datum plane will fail. I will play with this.

Click to expand...

If it fails, it can be rerouted or redefined. Does anyone ever look at the instructions? How is the surface "modified?"

I have not logged in any new stuff on PTC Community for a long time - still in the top 20 of ranked users, with those above me being either VAR representatives or work-for-hire users running their own business, in part, on PTC software.