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imoldes1-Visitor
1-Visitor
May 10, 2018
Solved

Problems with tolerances in Creo 4.0

  • May 10, 2018
  • 3 replies
  • 13332 views

Hello all.

 

I just moved from Creo 2.0 to Creo 4.0 M030 and I'm experiencing a lot troubles with the adaptation,  which is normal, but I'm having some problems that don't know how to solve:

 

1. How can I change dimension tolerances from the  part? When I select the dimension the tolerance tab is deactivated.

 

2. In the drawing, when I select a dimension to change its tolerance, I can't change them unless I change the tolerance option from "Nominal" to other option, e.g. Plus-Minus. Is there a way to change the tol. without changing the option.

 

3. Because Dimension properties windows is no longer a window, I can't edit a dimension that is in a drawing note, so I can't do anything with it, for example, I can't change the tolerance, can't add symbols to the dimension, can change the location of the dual dimension (If I want the dual dim. located on the right or below). When I try to select the dimension from an added note, Creo opens the note format tab, but not the dimension tab, this is a pain in the...

 

4. When I have more than 1 dimension in a note, I can't change the decimal places for just 1 dimension, the "Decimal Places" option changes the decimal places for ALL the dimensions in the note (even angles), and the option that existed in Creo 2.0 with [.X] after the D number is no longer available (or at least it's not working for me in that way). Is there a way to change the decimal places individually for dimensions that are in the same note?

 

Thanks in advance.

 

 

 

Best answer by imoldes

Hello all.

 

I'll answer this case with the solutions, it may be helpful for someone of you.

 

1. As Pushkar said in his answer, the config option tol_display must be set to yes so you can edit tolerances in dimensions from the part.

 

2. This problem was solved in the version M050, I guess I have to update mine.

 

3.  In the drawing, select the Annotate tab, then go to the smart filter and select the option "Individual Text", with that filter activated, you are able to select the dim. from the note and open the properties window like in Creo 2.0.

 

4. This can be solved following the same steps as in point 3. 

 

I hope this can help some of you. It is still a longer process than it was in Creo 2.0, but at least it had solutions...

 

Thank you.

3 replies

P
pushkarkhanna14-Alexandrite
14-Alexandrite
May 15, 2018

Hi

For changing the tolerance in part/assembly mode, config option tol_display needs to be set to "yes"

Pushkar

I
imoldes1-VisitorAuthor
1-Visitor
May 16, 2018

Hi.

 

Thanks for your reply. I tried it and worked, didn't have it activated because it wasn't required in Creo 2.0, however, it doesn't work like the previous version; when I activate this option the dimension in the part is shown as the selected tolerance option; for example, if I have a dim. as limits then the part shows the dimension in limits, not the actual value; that's how it worked in Creo 2.0 and it was awesome for me, I think they changed it and there is no turning back for it... Time to adapt.

 

Thank you very much.

    I
    imoldes1-VisitorAuthorAnswer
    1-Visitor
    May 25, 2018

    Hello all.

     

    I'll answer this case with the solutions, it may be helpful for someone of you.

     

    1. As Pushkar said in his answer, the config option tol_display must be set to yes so you can edit tolerances in dimensions from the part.

     

    2. This problem was solved in the version M050, I guess I have to update mine.

     

    3.  In the drawing, select the Annotate tab, then go to the smart filter and select the option "Individual Text", with that filter activated, you are able to select the dim. from the note and open the properties window like in Creo 2.0.

     

    4. This can be solved following the same steps as in point 3. 

     

    I hope this can help some of you. It is still a longer process than it was in Creo 2.0, but at least it had solutions...

     

    Thank you.

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