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Tolerance mode: Nominal vs Limits

23-Emerald II

Tolerance mode: Nominal vs Limits

In my standard drawing .dtl file that I am using to upgrade drawings from and old standard to a new, there is a setting that I may be missing because it changes a lot of the drawings dimension from nominal to limits. What parameter do I have to adjust to keep this from happening. Thanks, Dale

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Do you have the following .dtl option set how you want?


Would you find that under the section -These options control dimensions?

If so, I do not see that.

How would I either add it or have it be shown?

Creo 2.0:

File--> Prepare--> Drawing Properties -->Detail Options

"These options control dimensions" --> about 1/2 way through the section, "default_tolerance_mode"

Or just start typing it in the Option window at the bottom

I am using WF5/Creo. After I type "default_t" nothing shows up. There are things until I type the T.

I have had your issue. Nothing that I know can be done about that except to either turn tolerance display off all together or select all the dimensions (filter and window select) and change them to all to Nominal.

I don't know about WF, but in Creo, you also have to be careful about limit dimensions as they try to change geometry. Something wants to change the geometry of limit dimensions to the mean nominal. This has not always been the case. Very disturbing! Often I define a tolerance as Plus-Minus say +.01 -.02 and then change it to Limit. Creo wants to change this to a nominal using +/-.015. Personally, I want to define my nominal the way I want it, not how Creo wants it.

I knew about the limits wanting to change the CAD before and yes that is distubing. Especially for shafting and bearings where you have one sided tolerance and someone wants them displayed with limits instead.

This was just in changing the .dtl file for a new drawing standard and not knowing why most dimension then change to limits and I have to go and change them to nominal.

All my old 2000i drawings, and several imported Pro|E parts from internet libraries come in with limit dimensions assigned to all model dimensions. Very annoying.

I just tested Creo 2.0. Assigning new limit dimensions does not try to change the nominal. It seems to be an issue with a legacy converter as we open old files.

It's not a problem with converter. In all versions, default_tolerance_mode is an option also in and it also governs tolerance mode for parts' dimensions in 3D mode. Prior to Creo release this option had default setting to limits, thus all parts made in earlier software will have limit tolerance. Somewhere with Creo release it has been changed to nominal as default for new parts, but of course it hasn't affected models made with ProE.

Interesting. That means that dimensions that -were- changed to a different mode such as +-symetrical, they should not have changed on drawings or in model sketches when opened in later versions.

Sounds like you've been through this. Lukasz

Yeah, I think they remain with changed tolerance mode, but I'm home now and have no way to verify this .

And yes, I've been through this couple of times, but from different angle: I work for Polish VAR and among other things I do trainings for our customers - the issue with tolerance limits came up alwys with drawing module and showing how to set up tolerances in ProE . They were always in limits mode after enabling tolerance display so that got me to work thorugh this and see what's the reason.

Please refer to my answer in ISO Standard Fits and Tolerances This should answer most questions raised.

As for nominal dimension changing, please check your "Dimbound" mode. Dimbound takes the tolerance value and adjusts the dimension to either, uppper bound, Lower Bound or to Mean.

I do not have proe open right now and hence quoting from memory.


See if WF5 has this in

maintain_limit_tol_nominal yes

I can have a nominal value and have 2 plus tolerance values.


It will be in WF5, as it is in WF4, and from memory it was new in version 20

Not sure why the default has always been 'no' you would have thought you'd always want to model at nominal

I did not find it in the when opening it up from the computer, but when I went into a model and typed it in, it was there.

Do I have to check every part? If so, will it keep the dimensions that are set to symmetrical and anything other than the default?

use Tools > Options and type in the config exactly as shown i.e. maintain_limit_tol_nominal and then in the value box type yes the Add/Change button should then be available to you and you can add it.

otherwise, go to your and open it up in wordpad or similar and enter it there, it should then be there.

I am sure it will be as I am on WF4 and it is a config option for me, and it is an option in Creo2

Correct. I added it to my default when I found the option. Not one you would think you need to find. Logically it will only affect subsequent limit tolerance changes since any pre-defined ones will already have changed the nominals. However, it should solve the issue of opening older files when this feature was not present. The files I've had trouble with was back from 2000i.


Are you recommending that I open up the and just add that line to the file? Then when they are opened in the future, it will read that?

Thanks, Dale

Yes, I have this set by default in all my files. I have not had the issue since I added it. I forgot about it until I was looking into this thread so I looked in my template version of the Sure enough, it brought back all those memories in fighting with this.

This is the default (as installed) in Creo 2.0.

No part needs to be opened to assign the maintain_limit_tol_nominal option.


I have now added that line to the and we'll see how it goes into the future.

maintain_limit_tol_nominal yes

(back on the board with a little trepidation from the ~2000 spam emails).

I am still getting the. "This will need to be approved by the moderator" on this post. Just thought I'd try a new one.