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How do you apply tolerances to a model when ideally you want to produce a model to mid tolerance?
Can some please explain this concepta little deeper for me. Suppose I want to model a bore that needs to diameter 24.9mm to diameter 25.0mm. I would model this at its mid tolerance dimension as diameter 24.95mm. My question is,how do I get the drawing dimension to show diameter 24.9 +0.1/-0 or 24.9/25.0

Thanks in advance,HB (WF2)
First you will need to enable the tolerance options in the & the drawing dtl file

The option is tol_display - set to yes

Thedtl option (right-click on the drawing background, choose Properties -> drawing options)is tol_display - set to yes

The you can edit the dimension, & set the values in the drop-down box next to the dimension (nominal / limits / plus-minus / +-symmetric)
I've changed the dtl file and file as per your email, but I cant activate the Upper and Lower limit fields, they are greyed out.

Why is this so difficuilt ??


It should be a Shown Dimension. Then you can directly enter the limits values.
If you want to show limits for the created dim in thedrawing, Lets take your example. You want the tol of the bore to be between 24.9 to 25.0, so you will model the bore to 24.95. Then go to properties of the dimension created, in the Tolerance mode select Symmetric, Key in .05, then go back to Tolerance mode and now select Limits. That should be it. You can also do it using the Plus-Minus type of tol for asymmetric Tol.

All the best.
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24.9 to 25.0, which is the nominal dimension? you should model based on nominal dim and then define tolerance.
here the nominal dim is 24.95.

if the dim in the drawing is a shown one, you can model using any value, even 10.And when you edit this showndim inthe drawing using the RMB>properties, you can directly go to tol model, select limits, enter 25.0 in the upper limit, and 24.9 in the lower limit. say ok and then regenerate the model.

let me know if it works

I wanted to model to MID tolerance, so that step files etc can be utilitsed by NC machines etc. and that other modeling references etc are taken from these mid points. Is this not the correct theory?

Thanks for all imput btw.
Yes it is very correct, in the previous reply i had mentioned to model the hole to 10, and then give the tolances, and when you regenerate the model, the nominal dim automaticaly is given the mean dim. here it will be 24.95.

got it?
Got it...........sort of !!

Got another related problem now where my mid tolerance model dimension is 0.9625mm but I need to display this on the drawing as 1.0 -0.025/-0.05mm. This one is proving difficuilt to do. I am using the icon "create standard dimension...." rather than the show/erase dimension. I think this is my problem now.


I checked out that it works perfectly fine using Tol mode as Plus-Minus, for both shown as well as created dim.

Here you enter -0.025 in the upper tol and 0.05 in the lower tol,

about displaying it in Limits mode? After entering as above in plus-minus mode, just select Limits mode.

All the best,

by the way where are you from. it was 6.00 am here in india when i recievied yor first mail.
Thanks everyone. I've been able to follow your suggestions, but I need the dimension to be as follow 1.0mm -0.025/-0.05mm in the drawing. The main problem is that the mid tolerance of the modeled feature is 0.9625mm. Sorry to be a pain.......
You CAN have two negative values in the tolerance. Just enter -.025 for the upper value. Note that the absolute value must be less than the lower tolerance.

If you want to have asymmetric tolerances but nominal geomerty it is requires an extra step. Set up the shown dimension exactly as you want it to appear in the drawing. Then in part mode got to Edit/Setup/Dim Bound. Pick Middle (not nominal) and then select the dimension(s) you want to force to the middle value. When you pick done Pro/E will regenerate the part with the new geometry.

I use this all the time to have nominal geometry for CNC programing. It is good for things like radii that only have an upper limit like "R0.8 max." Set the tolerance type to nominal, set the nominal value to 0.8, set the upper limit to 0 & the lower limit to 0.8. Set the Dim Bound to middle and the geometry will be at R0.4 but the dimension will show as 0.8 max.
I don't know WHY would you want to have two minus values for tolerance? It seems like there should be a value that you want the the part to be made (nomimal) and let the tolerance determine how much it can vary from this "perfect" dimension. with two minus values, a perfect dimension will be out of boounds. Or is there something out there that i've been missing.
There are certain classes of fit, etc. where there is always clearance or always interference. For instance, the ISO system for limit allowances and fit specifies that a mominal shaft in the range of 6 to 10 mm diameter with a n6 tolerance class has a tolerance of +.019 to +.010 but with a g6 tolerance class it will have a tolerance of -.005 to -.014.


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