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Ordinate Dimension Reference

jcolon
3-Visitor

Ordinate Dimension Reference

I have a drawing that on it's second page uses ordinate dimensions. Out of these, the "X" value .000 dimension lost the reference and is now colored purple. If I erase this baseline dimension, them all other dimensions associated from this base point go along with it. I want to avoid this, is there a way to redefine the dimension so that it is no longer purple or perhaps a way to disassociate the children dimensions form it?

1 ACCEPTED SOLUTION

Accepted Solutions
dgrobe
6-Contributor
(To:jcolon)

this is an issue that has been around forever.  i have yet to find out how to redefine the dimension so it works.  so, to answer you, no.  you cant do that at the moment.

View solution in original post

14 REPLIES 14
dgrobe
6-Contributor
(To:jcolon)

this is an issue that has been around forever.  i have yet to find out how to redefine the dimension so it works.  so, to answer you, no.  you cant do that at the moment.

jcolon
3-Visitor
(To:dgrobe)

Man, that's crappy. Thx!

I fight this often. Here's what I have found to work most of the time (for some reason beyond my understanding it doesn't always work).

1. Find the first dimension that was created and right click, choose "Toggle Ordinate/Linear". (Only the first dimension created will have this option).

ordinate dim (1).bmp

2. Right click on the now linear dimension and select "Edit Attachment".  Re-attach dimension.

ordinate dim (2).bmp

3. Right click and select "Toggle Ordinate/Linear".  Select the same witnessline for zero as the original.

ordinate dim (3).bmp

4. If it works you will get the following message, click "Yes".

ordinate dim (4).bmp

5. Now you will be back to where you started with a purple zero dimension, regenerate the drawings (type "rg").

ordinate dim (5).bmp

6. After regeneration you zero will "come back to life".

ordinate dim (6).bmp

Using Creo 2.0 M060

Dave

dgrobe
6-Contributor
(To:dwelters)

im gonna try this next time.  thanks for the hint.

Just had this issue pop up and decided to search around this time instead of just deleting everything.  I was not able to use David Welters' technique...none of my ordinate dimensions gave a "toggle ordinate/linear" option when right clicked.  However, I did have success using PTC support document CS69648.  I had to read it a few times but the procedure is:

1) Make a new std linear dimension.  Use your intended baseline reference for one of your clicks.

2) Right click toggle the new linear dimension to ordinate and pick the actual magenta baseline dimension.

3) Review tab-->Update Draft

4) Repaint

5) Delete old dimension replaced with the new one made in step 1.

Note: CS69648 has the above procedure for Wildfire.  Procedure for Creo is to just delete everything.  I'm using Creo 2.0 M150 and did not have to delete everything.

https://support.ptc.com/appserver/cs/view/solution.jsp?n=CS69648&lang=en&source=snippet

New to Creo, started working with Creo 4.0. This worked for me. Thanks!

Hey cbowes,

 

Thank you for letting us know the summary of the procedure.

I'm using CREO 5.0 and it worked great!

 

I don't understand why after several CREO versions, they are still missing a simple command like "Edit attachment" or "update attachment" of the Zero baseline dimension.

creuz
11-Garnet
(To:cbowes)

Ditto thanks!

creuz
11-Garnet
(To:cbowes)

Thank you from a new user!

Rick

JWU_14
3-Visitor
(To:cbowes)

Hard to imagine this still an issue in 7.0.5.0, thank you!

pausob
17-Peridot
(To:JWU_14)

So @JWU_14, the CS69648 procedure by @cbowes worked for you?  I'm on Creo4, it isn't working for me - seems I will have to redraw the ordinate dimensions.

JWU_14
3-Visitor
(To:pausob)

@pausob Hi, Darn that's a bummer, Was there a specific function you could not activate/use? Just curious, it did take a few tries for me, the second ordinate dimension can be fussy to right click on.

jwindcoach
5-Regular Member
(To:jcolon)

In CREO-3, got those purple ordinate dims too.  How to edit them --- left click once to highlight purple dim, right click and pick from the pop-up menu 'Edit Attachment'.  Go pick whatever it's suppose to attach to, then middle mouse button click to place it.  Bam-o, done.

Now looking for method to ADD only 4 more ordinate dims.  I do NOT want to delete 95 others and redo the entire view.  That is an insane method in a CAD software!   In CREO-2 and back, it was a bit miserable.

 

StephenW
23-Emerald I
(To:jwindcoach)

You can add more ordinate dimensions by selecting the ordinate dimension icon, then selecting the baseline of your current ordinate dimension, then picking the objects you want to dimensions, then place dimensions. 

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