Help with Tolerance Tables

[peterbrown772]

Hola -

Longtime Creo/WF/ProE user (2000i2). Having an issue with fit tolerances using the tables. I've configured both the part and drawing to use the tables.

Problem example:

I have a 20mm shaft for a bearing; recommended shaft fit is h6. For a 20mm dia, h6 is:

+0

-13.

In inches, that is + 0, -0.0005". So the drawing should show 0.7874/0.7869 if I show limits.

I set the diameter to nominal, 0.7874. I apply an h6 tolerance.

If is specify plus/minus, the dimension appears at 0.7874 + 0.0000 / -0.0005 (perfect!)

If I show 'limits', it changes to the nominal 0.7871 and then applies the -.0005 to that, so 0.7866. This is wrong.

What am I doing wrong?

TIA

[tbraxton]

I was able to replicate the issue in Creo 7 in both SI and imperial units models. Creo is shifting the nominal value of the dimension but the limits from the shaft table are calculated accurately, they are just not displayed/stored with the dimension in the model. The limits shown in yellow are accurate from the table but the nominal in red is shifted from the staring value. If no one provides a resolution here in the near future, you should open a tech support case.

[peterbrown772]

I have opened a support ticket - 

[Van_AG]

I confirm the same behaviour in Creo 8.
To fix the issue, add one step: set tol tables to 'no' and only then switch to 'limits'

The following dimension format does not comply with any standards, afaik.

And the program should not and is not required to support the automatic generation of such a dimension format

 

[peterbrown772]

I'm not quite understanding your solution nor the statement "

The following dimension format does not comply with any standards, afaik.

And the program should not and is not required to support the automatic generation of such a dimension format"

[Van_AG]

I meant that ISO tolerances for dimensions specify how much the measurements of a part can deviate from the nominal value. In other words, by specifying the tolerance class, you indicate the deviation from the nominal value, not the limit values.

Why specify the nominal value + tolerance class + limits instead of deviations from its nominal value, as required by the ISO ?

[peterbrown772]

There are two reasons to show the limits AND move the geometry to the nominal value:

1) Showing the limits prevents a mis-calculation of the correct value by the machinist making the part.

2) Having the geometry at nominal is the practice for users who have Pro/NC. 

We are a manufacturing company with a major investment in Creo, Pro/NC, and Vericut. We do not export STL files or similar to 3rd party software like MasterCam. When creating a toolpath, the geometry should be at nominal. For example, if you are machining a 50 mm bore with an H7 tolerance of + 0.03 / -0.00 mm, so 50.03 / 50.00.  The model should be at 50.015 mm. If the geometry is at 50mm, the toolpath will describe a circle of 25mm + the radius of the tool. In my example this will be a 10mm dia tool.  If the feature actually measures 49.90 mm the machinist will correct the program by using what is known as a cutter compensation, where he will in effect tell the machine that the  tool is not a perfect 10 mm but is 10.05 mm in diameter. The toolpath will now follow a circle where the tangency of it is 50.00 mm. 

This is fine only IF this is the only feature that the tool creates on the part, because the cutter compensation (known as tool offset) is specific to that tool. If that same 10mm tool is used for another feature, it will be wrong and basically impossible to correct without same fancy G-CODE utilizing variables on a per-feature basis in the G-CODE. Even worse would be if the same tool makes a shaft-type feature and a hole-type feature. Now you are in a situation where it is impossible to get a good part because the geometry is at the maximum and minimum sizes for each feature and ANY tool compensation, larger or smaller, will cause the other feature to be out of tolerance.

For this reason, models used for manufacturing should be at modeled at the nominal of the dimension tolerance, not at a limit in either direction. Models created at the limit of the tolerance zone lead to scrapped parts.

Best regards