Tolerancing

[AndreLTR]

Hello everyone,


How to define a tolerance specific to one feature instead of the general which is quite direct please? Is it possible? I apreciate very much any information about it.


Thank you verty much indeed,


Andr

 

[robertib]

First you need to have 2 settings in your config.pro file


tol_display yes


tol_mode nominal


Then select the feature in the model tree, right-click & choose Edit not Edit Definition.


Select the dimension you want to tolerance, right-click & select Properties.


Choose the tolerance mode from the drop-down box:


nominal - basic dimension
limits - highest & lowest values
plus/minus - basic dimension + value 1, - value 2
symmetric- basic dimension + & - the same value


Tolereance as desired.

 

[AndreLTR]

Hello Mr. Robert,


Thank you very much indeed for your answer. I still have something to learn it is the truth. BTW is there any form to have the tolerances exported to a STEP file or STEP doesn

 

[dr_gallup]

To my knowledge, STEP only exports nominal geometry (typically solid), not dimensioning schemes or tolerances. There are multiple STEP output formats (AP202, AP203, AP214, etc.) and I do not pretend to understand the differences so perhaps there is a way. You need to research STEP to find out more.

 

[pjw]

Maybe you could export your STEP file at middle limit on all dimensions if you intend cutting die moulds with it?


Wildfire:


Edit>Setup>Dim Bound>Set All>Middle Limit


We sue it for producing CNC part programs. we create programs for the parts at middle limit then manufacturing doesn't run out of the specified tolerance due to it being machined at nominal sizes.


Hope this helps


Phil

 

[AndreLTR]

Hello Mr. PJW,


Thank you for he response. It will not help because my only objective is to have tolerancing data in the STEP file that is used in a design framework that has STEP as its base data.


Sincerely yours,


Andr