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Dimension and tolerance to 3 places

ptc-6661379
3-Visitor

Dimension and tolerance to 3 places

Hi all,

I have struggled with this several times in the past. I have a feature where I would like the diameter to have limits of 5.257 / 5.250. I would like this to display as a 3 place decimal on the drawing. I can't seem to do this. I end up having to have a nominal feature of 5.2535 with a ±.0035 tolerance (switched to limit tolerance for display). I then get a display of 5.2570 / 5.2500. This has repeatedly caused questions internally and externally as it is the only dimension displayed to 4 decimal places. If I change to 3 place decimal display, the dimension changes to 5.258 / 5.250. This is really frustrating me and I'm sure that I'm not the first to run into this problem.

Any help is greatly appreciated.

Greg

3 REPLIES 3
BenLoosli
22-Sapphire III
(To:ptc-6661379)

Try setting the nominal dimension to 5.2533, then apply your +/-.0035 and change to 3 place display. Not ideal, but it is what it is.

Rounding rules for engineering go to the even number when the last digit is a 5. 

 

BenLoosli
22-Sapphire III
(To:BenLoosli)

BenLoosli_0-1635271465839.png

Creo 7.0.5.0


@ptc-6661379 wrote:

Hi all,

I have struggled with this several times in the past. I have a feature where I would like the diameter to have limits of 5.257 / 5.250. I would like this to display as a 3 place decimal on the drawing. I can't seem to do this. I end up having to have a nominal feature of 5.2535 with a ±.0035 tolerance (switched to limit tolerance for display). I then get a display of 5.2570 / 5.2500. This has repeatedly caused questions internally and externally as it is the only dimension displayed to 4 decimal places. If I change to 3 place decimal display, the dimension changes to 5.258 / 5.250. This is really frustrating me and I'm sure that I'm not the first to run into this problem.

Any help is greatly appreciated.

Greg


Hi,

the problem is related to MAINTAIN_LIMIT_TOL_NOMINAL config.pro option. The option is set to NO by default (I used Creo 7.0.5.0 during testing) and because of this Creo changes nominal value to 5.2535 (4 decimal places are needed) after setting Limit tolerance display.

If you set MAINTAIN_LIMIT_TOL_NOMINAL YES, then Creo maintains dimension nominal value after setting Limit tolerance display and you will get what you need.

 


Martin Hanák
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