Showing results for 
Search instead for 
Did you mean: 
Showing results for 
Search instead for 
Did you mean: 

modeling/drafting vs. production


modeling/drafting vs. production

We do a lot of modeling/drawings where there is nearby geometry that
requires unidirectional tolerancing on a feature, some plus others minus
tolerances within the same feature.

Gaps between parts must be verified/controlled so we model to the actual
required part size and measure gaps and look for interference on parts
in the assembly. When satisfied we then generate drawings and apply all
the tolerances.

When production gets the drawings they like to work to the center of
the unidirectional (symmetrical) tolerance which means that they have to
calculate these values.

With the number of features on some of the parts converting back and
forth in the models or calculating takes a lot of time and usually gets
some errors due to typos.

Is there a method within Pro_E that allows quick switching back and
forth between the part actual size that requires unidirectional
tolerancing and the size needed for manufacturing using symmetrical

Is there a work around that will do the same?

Anybody have any suggestions?

Thanks for any input

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.

There is a very nice capability in Pro/E that lets you change how a dimension regenerates within it's limits.. By default, all dimensions regenerate at nominal when they are created, however you can set them to upper, middle or lower as well. Go to edit/setup/dim bound. In your case , you probably want to pick middle, then select dimensions that you want to regenerate to the middle value. When you are done selecting the part will regenerate. So if you have a dimension of 10+1/-0 set to middle the geometry will measure 9.5 but the dimension will still read 10+1/-0. Notice that there is a select all option so you can easily return all dimensions to nominal (or upper/middle/lower). There is also the Dim Bound table option where you can set up a certain condition (such as MMC) and quickly return to it any time you want to study it again.

All that said, I would seriously re-examine your motives for using asymmetric tolerances. In most cases I have found you are really kidding yourself if you think manufacturing is going to intentionally make the parts to anything but the middle. There are some asymmetric manufacturing processes but they are pretty special cases. I find it better to dimension everything with symmetric tolerances and then do MMC/LMC studies to look at the fits & clearances.

One place I do use both asymmetric tolerances and the dim bound functionality is with max or min dimensions of rounds or chamfers. If I want R0.5 max on a drawing and I know the minimum cutter radius is R0.2 I will make the dimension nominal 0.5 but set the upper tol to 0 and the lower tol to .3 the set the dim bound to middle. This gives me a radius that measures 0.35 with a dimension that reads R0.5 max.

The upper and lower is not an MMC or LMC condition. In the case of
internal radii, outer radii, the larger/smaller value is used,
regardless if it moves the geometry towards an MMC or LMC condition.

Correct, you have to make the proper selection on upper and and lower tolerances to achieve MMC or LMC. But once you have all the dimensions properly set you can save that combination and go back to it if you have changed the tolerances. Note, it is possible to have dimensioning schemes where it is impossible to achieve a true MMC or LMC boundary condition.
Attention: Creo 7.0 Customers
Please consider upgrading
End of Life announcement here.

NEW Creo+ Topics:
PTC Control Center
Creo+ Portal
Real-time Collaboration