Skip to main content
M
mheath1-Visitor
1-Visitor
December 1, 2011
Question

Override value for created dimensions in the drawing.

  • December 1, 2011
  • 8 replies
  • 4156 views

I just submitted a case with PTC that we wanted to know how to disable a feature we found in Creo Elements/Pro 5.0. If you create a dimension in a drawing and go to the properties of that dimensionthere is a radio button that says Override Value with a box next to it. I found that if you select this option that you are able to input any value you want for this dimension. PTC basically doesn't have an issue with this and that if I want an option to disable this then I need to submit an enhancement request. My question to all of you is do you find this acceptable? I know we should be using model created dimensions, but sometimes our user will create dimensions within the drawing. I asked if ModelCheck would find these Override Values and he reported to me "NO". I have submitted an enhancement request, but I don't see this as an enhancement.


Thanks for your time,


Mike Heath


This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

8 replies

P
ptc-8798271-Visitor
1-Visitor
December 1, 2011
You've always been able to do that with &O and the fake number.
Thanks
Greg

Greg Ames
greg.ames@suburbantool.com
Designer
Suburban Tool & Die
4940 Pacific Ave.
Erie, PA 16506
TEL: 814-833-4882
FAX: 814-833-1370
www.suburbantool.com
T
tcooper1-Visitor
1-Visitor
December 1, 2011
There used to be a config option that prevented using the @O capability, so PTC used to agree that it should be controllable. That was also detectable in MC. Why the shift in that thought PTC?

What's more scary is that override radial button only allows numerical values, not text, so it's intent seams to be just to lie on the dimension. However if you go to the Display tab you can then replace the @D with an @O and then your back to the OLD style of overriding created dimensions. Perhaps that is where MC will detect to override like the "old days".

Tim P. Cooper
LM IS&GS-CIVIL, Houston
Launch & Recovery Systems PTVPC
LM2 / Cube 228L

Physical Address: Correspondence:
2400 NASA Pkwy LM2, 304B
Houston, TX 77058 P.O. Box 58487
(281) 333-6735 Houston, TX 77258-8784
(281) 333-6300 (F)
W
wattsteam1-Visitor
1-Visitor
December 1, 2011
There are isolated, infrequent individual cases in which overriding a dim value is acceptable and necessary, so I would never support outlawing it.

However -new / junior users should be warned against abusing the ability to override the value and in normal use it should not be done.

Best regards Jeff Dayman
D
DonSenchuk12-Amethyst
12-Amethyst
December 1, 2011

In the modelcheck file 'default_checks.mch' there is an option for overwrite dimensions.


DIM_OVERWRITE


The options are YNEW, so you can set your modelcheck to error on finding any overwritten dimensions. (Though I'm not sure how to do it, I've heard that you can set your PDM system to reject the check-in of any models/drawings with modelcheck errors. That'll teach em! (Yes, yes, I know it turns out to be rather impractical to use this option.))


The underlying issue isn't really whether either Pro/E or PTC or ModelCHECK will flag or allow this to happen. The issue really stems from users taking the effort to fake these in the first place. After all, a user can ignore any rule or policyyou put in place that's not hard-coded into the system.

D
DeanLong1-Visitor
1-Visitor
December 2, 2011

I have not used an overridden dimension to fake a numberin 20 years. Usually this occurs when one is dimensioning "resultant" as opposed to "deliberate/explicit" features and the house of cards is too precarious to fix. In a simple sentence, good modeling practices never result in the need to over-ride a numericaldimension.


Now to thequestion. Yes, we do want the ability to over-ride dimensions for cases when one wants text instead of a dimension. This function is one I have used forever. What would be nice is when a dimension is overridden it stays a different color other than the normal dims. Not the purple, un-regenerated characteristic (bold print) but the same weight as regenerated dims. This would cut down on the abusing of over-ride by sheer guilt.


As Don, stated....beware the blatant mis-use of power.

P
ptc-5936191-Visitor
1-Visitor
December 2, 2011
"In a simple sentence, good modeling practices never result in the need
to over-ride a numerical dimension."



Dean, that may be right for your company but...



Then you have never had to dimension a three place tolerance where ProE
insists it is two? Or to put in a maximum material condition on a
nominal model? I can think of several reasons why you need over-ridden
dimensions not least where stretch and shrinkage are concerned. Try
producing models detailed in both Imperial and Metric without
over-ridden dimensions!



Not a criticism, just an observation.



Richard A. Black

Lead Design Engineer

Eaton Corporation

440 Murray Hill Road

Southern Pines

NC 28387 USA



tel: 910 695 2905

fax: 910 695 2901

-

www.eaton.com

B
BobSchwerdlin1-Visitor
1-Visitor
December 2, 2011
How about using an override dimension to show something like, "L" for a part length and then having a repeat region table on the drawing with a column header showing "L" for all the various part lengths.

Bob
G
gwalker1-Visitor
1-Visitor
December 2, 2011

If you want to show a dimesnion symbol instead of the dimension value, use @S instead of @D. You can edit the dimension properties so that the dimension symbol is "L" instead of "d42". That way if you decide later the change the dimension symbol to "LENGTH" it will update the dimension on the drawing and in any tables it is used in.

In Reply to Bob Schwerdlin:


How about using an override dimension to show something like, "L" for a part length and then having a repeat region table on the drawing with a column header showing "L" for all the various part lengths.

Bob

Terms & ConditionsCookie settingsAccessibility statement