deleting Geometric Tolerance

[amitk_001]

Hi,


I am working in Pro/E drawing module and recently I put some incorrect
geometric tolerances on dimensions. I clicked the Geometric Tolerance,
and selected the tolerance and placed it on a dimension. Now the
problem is I need to delete the tolerance. I cannot delete the
dimension, I can only erase it. But If I select the feature again and
select show dimension the tolerance shows up again. It also shows up in
the model file.


I found one way around it. It is to go in sketcher mode for that
feature and delete the dimension and create it again. That way you can
get rid of the tolerance.


Is there any other way?? I tried searching for Gtol through find feature, I found the Gtols but was not able to delete it.





Let me know if there is any other way to solve this issue








Thanks,


Amit

 

[prohammy]

Try using Show/Erase to erase the geom tol, that should solve it


Kev
Edited by: prohammy

 

[amitk_001]

Kev,
Thanks a lot. With show erase, it still keeps the Gtol associated with the dimension. It will not show if I do the erase, but its still there. If i do a show it will come up. I want to delete it completely.


Thanks again
Amit

 

[charleskim]

In WF2.
Edit > Setup > Geom Tol > Clear and select the Geom tol you want to get rid of.


Charles

 

[prohammy]

Sorry Amitk,


I misunderstood your OP. I think (and I'm sorry I don't have time to test this) that if you query select to select the geom tol itself , then you can delete the geom tol only.


Yeah, just checked it and that does work


Cheers


Kev

 

[prohammy]

Amitk,


In WF.... go RMB (anywhere on the geom tol text) to query through to the geom tol, LMB to select the geom tol, and then RMB and a pop up menu will allow you to both delete and/or erase the geom tol only


Kev

 

[amitk_001]

Thanks a lot. It helped to solve the issue.


Thanks
Amit

 

[Maike13]

In Creo 2.0

Old thread I know but it came up when I did a Google search, so I thought I'd add this so I know exactly what to do next time (I do this so seldom I'll have forgotten again by the next time I have to do it

The suggestions here helped me get there, but it didn't seem to work quite the same in Creo 2.0 (or more likely it's my ineptitude in Creo . Anyway here is a step by step that worked for me:

To Remove a Geometric tolerance:

With selection set to General:
Left click and release over geometric tolerance. This selects dimension and geometric tolerance.
Right click and release over geometric tolerance. This de-selects dimension and geometric tolerance.
Left click and release over geometric tolerance again. This selects just the Geometric Tolerance.
Right-click and hold. This brings up the Geometric Tolerance menu. Select Erase

With selection set to Geometric Tolerance
Left click and release over geometric tolerance. This selects just the Geometric Tolerance.
Right-click and hold. This brings up the Geometric Tolerance menu. Select Erase

 

[Dan_Pasholk]

To remove GTOL from a dimension.
1. Hover mouse cursor over the dimension.
2. RMB => pick from list.
3. Select the (GTOL). OK
4. RMB => Properties => Geometric Tolerance menu pops open.
5. Select the Model Refs tab.
6. From the Placement: Placed, Type drop down, select As Free Note.
7. Click anywhere in the graphic area to place the GTOL.
8. OK to close.
9. Select the GTOL => RMB => DELETE

 

[hobby_man]

I have to try this