Moving Datum Tag to a Note in drawing

[merlin1012]

I'm trying to relocate (move!) the datum tag from the hole to the note:

Similar to this view:

I'm using version 7.0.9.0

Thanks In Advance (TIA)
Merl

[KenFarley]

I am using version 9.0.1 and to move a tolerance attached to a hole to the geometric tolerance I do the following:

(1) Select the datum feature.

(2) right mouse button

(3) In the menu that pops up, select the one that looks like two chain links.

(4) Pick the geometric tolerance and drag the datum into the proper position.

I don't know if this method is the same for your version of Creo, but hope so.

[merlin1012]

Sorry, I don't get the "chain" (Change Reference) when I RMB on the Datum Tag. 😞

When I RMB on the Note & "chain", I am not allowed to select the Datum Tag. 😞

[KenFarley]

A possible reason: Did you create that datum tag in the drawing, or was it created as an annotation in the model? I don't believe you can change the reference of a datum tag that was created in the model. I just tried it and was not presented with the option to change reference when in the drawing.

[merlin1012]

Yes I did create the Datum Tag in the model.

Creating the Datum Tag in the drawing does give me the option to move the Datum Tag but I'm not given the option to attach it to the Note (which references a dimension, located on another hole). Should I redefine the Sketch with dimensioned holes & move the dimension so I don't have to reference it in a Note?

Thanks for keeping at it & responding!

[KenFarley]

I only use the "note as dimension" trick when I absolutely have to. For example, if there's a round I want to dimension but it's on a part that has been bent to a radius. A big drawback is when you want to change the tolerances or decimal places of the referenced dimension, you have to go back to the model to do so, etc. Also, if someone changes the rounding settings of a shown dimension, it could cause the actual dimension of your particular feature to be changed to that rounded number (i.e. 1.204 becomes 1.20 because someone rounded it to 2 places), which can be problematic.

I used to try to use the model dimensions as much as possible in drawings, but have found it is much more convenient to just create drawing dimensions in the drawing. In general, with the version of Creo I'm using (Creo 9) I find it much simpler to create all the dimensions, datum tags, and geometric tolerances in the drawing.

[merlin1012]

I tried both possibilities: redefining the sketch to move the dimension & just making the dimension in the drawing.

This is the result:

Still NOT the solution I was looking for, the Datum Tag attached to the bottom of the GD&T modifier; the Datum Tag will ONLY attach to the extension line.

Any other options? Hunt for some meaningless_named_setting? (Can you sense the sarcasm?)

Thanks again,

Merl

[pausob]

Not sure how it works with notes, or with Creo 7, but in Creo 4, you have the option of adjusting where the DFS is located.

Again, this is for the case of a dimension that has a GD&T control already attached and to which you then attached a DFS.

The tricky part I find is getting that DFS symbol to be selected, then right-clicking to bring up the menu:

In 3D model:

In drawing:

[merlin1012]

Good suggestion! But in 7 I don't get the option to move the Datum Tag anywhere from the Dimension Elbow. Is there a Config Option? (I'll take a look...)

Thanks for trying!

Merl

[merlin1012 · Accepted solution]

FINALLY found a "solution"; multi-stepped as it is:

1. Using a model dimension (may or may not work for a drawing dimension).

2. Add a drawing GD&T control frame (Geometric Tolerance) ; attach to dimension in Step #1.

3. Add a drawing GD&T datum target (Datum Feature Symbol)  ; *IMPORTANT* when attaching, or selecting point on screen, select the control frame made in Step #2.

=> 

Special thanks to coworker who played with my left-handed mouse and figured this problem out!

Thanks to everyone else who tried!

Merl

[pausob]

Thanks for summarizing the solution!  To be honest, still confused as to what the problem was.  I do think the root cause is the confusing implementation on PTC's part as to what is a drawing annotation and what is a model annotation and where that information is stored, and that they look the same but you can do some things with one but not the other.... yada yada yada.