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how to change default tolerance value in drawing

Newbie

how to change default tolerance value in drawing

Hello,

 

just wondering how the default tolerance value works at new created dimension in drawing. Since i use mostly the +- symetric - would it be possible to set the default tolerance (maybe in drawing setup file) value this way?

 

Thanks in advance

 

T.

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12 REPLIES 12

Re: how to change default tolerance value in drawing

You can set this in config.pro. It seems to be very convoluted but once set, it works.

For some reason, it has to be in config.pro, and not changed in the options editor.

The values are set to a factor of 1000x. Drawings take on whatever the current config.pro settings are.

These are the valid options in config.pro (linear and angular):

tol_options.PNG

I used whole numbers in the settings in config.pro. These are the default ones that show up on the screen.

tol_options_II.PNG

If the current default_dec_places is 3, the .008 will be used on drawing dimensions as well.

If, like me, you use default decimal places is 4, I cannot seem to get these to be recognized by default. I suppose I need to file yet another support case. Config.pro is recognizing the linear_tol_0.0000 50 but the actual value comes in at .0001 in both drawings and models.

Re: how to change default tolerance value in drawing

I created a case for using values greater than 9 in these default toerlance settings. Options shows it is accepted but in reality, it doesn't work.

Use case, my drawings use 3 digit dimesnions but I want to see 4 digits when modeling. I want the default tolerance value to be .005(0)". I can't do that with 4 digit dimensions!

Re: how to change default tolerance value in drawing

Can you try these in your config.pro:

default_dec_places 4

linear_tol 1 0.2

linear_tol 2 0.05

linear_tol 3 0.008

linear_tol 4 0.0050

However, for me this doesn't really work, because it seems the system makes all new dimensions have 4 decimal places, and +/- 0.005 tolerance.

So if I want, for example, a dimension of 50.0 +/- 0.2, the system will actually first create one that is 50.0000 +/- 0.0050.

Now, if I change the # of decimal places to 1 by editing this dimension's properties, the system will set the dimension to 50.0 +/- 0.005, and upon displaying the tolerance on the drawing, it will say 50.0 +/- 0.0 !!!

BUT, if I then edit the dimension's properties and change its tolerance display to "nominal", exit the dialog and modify the value of this dimension to 50.0 (yes, just re-enter the same value), then the dimension will be "automatically" set to 50.0 +/- 0.2.

Basically, it seems like I have to change the # of decimal places, then re-enter the value of the dimension if I want my "default" tolerance values to be in effect.

So where am I missing the step where I can specify the # of decimal places at the time of entering in the value of the dimension?

Highlighted

Re: how to change default tolerance value in drawing

The syntax is different in config.pro for Creo. It uses the linear_tol_0.000 format and the values at x1000. And the value of 50 doesn't work.

However, the syntax you provided -does- work! So something went wrong in the translation into Creo. linear_tol is not an option in Creo but it must be from a previous version and is now hidden.

I walked through this with customer support earlier. I was able to show what was going on. I will post what they learn. If they try to tell me it works to specifications, I will point out this finding.

Your other findings on having dimesnions take on a different value with an edit is scary to say the least. I can see the logic as to why, but having values change just because the decimal places of the dimension value changes, that has some serious implications! A quick test in Creo 2.0 says this doesn't happened.

Re: how to change default tolerance value in drawing

The only time tolerance values change in Creo is if you disable (uncheck) "rounded dimension value" in the dimension properties. It rounds the current value to the appropriate decimal places.

The default_dec_places specifically states it only affects newly created dimensions. Changing the properties of an existing dimension does not qualify. However, in cases where you change a hole type, it does an internal delete and replace where these -are- in fact new values.

Re: how to change default tolerance value in drawing

Hi Tomas,

You didn't say if you were working in Imperial or Metric. Seems the discussion so far has been about Imperial (inch based) figures.

If you work in metric you can set the config

tolerance_standard ISO/DIN and this allws you to select

tolerance_standard medium (or fine or coarse) and these work according to length not the number of decimal places.

There is also as setting under TOL SETUP for Tol Tables so maybe it is possible to have some sort of general rule under that. Have never tried it as have always used metric tolerancing system though apparently this uses a set of ISO/DIN tolerance tables

Regards, Brent

Re: how to change default tolerance value in drawing

Well, I am using Creo 2.0 M120 and this is where I see this "weird" behaviour.

I'm curious about your "quick test" in creo 2.0 which says it doesn't happen.

Can you do it again and note the following:

- tolerance mode for the dimension has to be "Nominal"

- you are changing the value of the dimension by double-clicking on the dimension in the drawing or model (so that the little entry box shows up).

I find that under these circumstances, the system will change the dimension's tolerances to match the linear_tol settings (according to the number of decimal places specified for the dimension). The "rounded dimension value" setting doesn't matter. If the dimension's tolerances are set to other modes (Plus-Minus, +/- symmetric, ..) then they will not be changed when the dimension's number of decimal places or its value are changed.

Re: how to change default tolerance value in drawing

See if I covered your use case, Paul...

Video Link : 5458

Re: how to change default tolerance value in drawing

Support in this case is becoming very frustrating. I am being told that indeed you cannot apply a value greater than 9 (DUH!). I did not hear that this is functioning according to specifications.

Support also came up with the fact that linear_tol is a valid option although it does not show up in the options>find dialog. Support said they will file the SPR for the missing option.

I see this being escalated! There is no reason the option linear_tol_0.0000 cannot accept .0050 as a value. Even the dialog is accepting it in options. But it is not being carried forward to newly created dimensions.

I even asked specifically if the linear_tol (and angular_tol) were WF/Pro-E options that were being replaced with no answer. I only received the link to the options guide that still includes the two in Creo 2.0.

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