shaft tolerance

[ghunk]

Dear All,

in setup > tol setup > tol tables > shaft, i want to know what is the tolerance shaft function?? how to use it??

i have a case, if i have shaft that assembly to the bush...then in the 2d drawing, i would like to show shaft diameter dimension with the tolerance automatically...can pro/e do it??

thanks

 

[walkerone]

This functionality in Pro/E allows you to specify a tolerance table for a part and assign a dimension to that tolerance table. The ISO standards for shafts and holes are available if your model schema is set to ISO

i.e. config.pro option tolerance_standard is iso (ansi is default)

To use the functionality for a shaft that you want to be ISO f7 (for example):

In the part (this then allows all driven dimensions to be toleranced in this way), call in the required tolerance table. You can see the various tables using

edit.. setup.. tol setup.. tol tables.. retreive.. - you should see the default Tolerance table Directory containing hole and shaft tables. In my example, shaft_f exists, so I'll retreive that one.

You can see what the table looks like using show (from the tol tables menu manager) shafts and then enter f (because that is the table we have retreived...). This will show you the tolerance table which you can check against the ISO standards / a Zeus reference, etc

Now, go to the drawing that shows the shaft, and show/erase the shaft diameter dimension. This should show the diameter of the shaft as its basic dimension. Highlight the diameter dimension and right click.. Properties. change the tolerance table pulldown to shaft. The table name will be f and then pick the class you want to use (in my example, 7 to make f7).

Changing the tolerance mode pulldown gives different display results. Nominal shows the basic diameter and the tolerance class (e.g.

 

[sdshriram]

yes.........grate


i have done its working


nice


shriram sd

 

[ghunk]

yeah...its so great !!!

thank you so much

 

[Jacon]

Hello

I tried it and can get the table in the part correctly set to hole f but when I go back to the drawing and set the tolerance mode to limits the tolerance table still just give me the 3 default option (none, general and broken edge)

Is their maybe a setting that in my config.pro that I have to set.

Thank you

 

[Jacon]

Hello

I got it to work in the drawing. But it only applies to that drawing. How can I get it to apply to all my drawings. Can I set it once in the config.pro?