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Inheritance tolerance display problem:(

Forum|Forum|13 years ago
October 15, 2012
4 replies
5278 views

Hi Guys,

I am struck again, below shown image tells my problem i.e. I couldn't add tolerance to the dimension(22) that came from inheritance(Tolerance mode tab itself is greyed out), tried changing the tol_display option & no result. waiting for the solution guys:)

FYI.. the dimension is from core which is used in casting & below shown is the casting drawing, there is no seperate drawing for core i.e. core details also shown in this drawing only.

Cheers,

Hari

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2D Drawing

Best answer by vzak

Hello Hari,

Not sure if this will answer your question , just some info on Inheritance feature & tolerances :

1. When modifying Dim Properties of inheritance feature dimension, it is impossible to change Tolerance Mode. It is always the same as in base model. So if you have just "Nominal" type dim in core part, you will not be able to add any Tol on cavity it it uses core Inheritance cut. Same in 3D or in Drawing.

2. In general if you have some tolerance defined on base part dimension, its value can be easely modified on inheritance feature. Either through inheritance Varied Dimension table (show tolerances on the screen and pick one for Var Dims), or by direct edit/pick on TOL value on 3D screen. This should provide confirmation to add this TOL to varied items list and ytou should be able to proceed.

3. Do not try to use Properties dialogue to create/modify varied dimensions or tolerances - use direct selection of nominal / tolerances from the screen

4. When workingin show tolerances mode, you will not be able to make any modification to LIMITS type dimension of Inheritance feature - so hope you do not use LIMITS. Any other type (nominal, plus/minus, symmetrical) is available.

However if you switch off tolerances you can add any type of DIM to varied items of Inheritance feature ... since it handles all as nominal.

If this does not help feel free to ask more precise one.

H

Hongjie

1-Visitor

Hi, Hari,

try to set different "tolerance mode", hope it is work for you.

other wise, you need to modify configuration.in file>properties>drawing opetion, you can find a lot of setting. if above tolerance mode tring do not work, tell us, I find some possible setting optional for you.

Best regards, Hongjie

H

hmr

Author

1-Visitor

Hi Hongjie,

Thanks for you reply,

But the option "Tolerance mode" itself is greyed out, please let me know how to activate that option.

Cheers,

Hari

H

Hongjie

1-Visitor

try to set optional: tol_display to yes.

I have just try it in my ProE WF4.0 and found "tolerance mode" grey out during "tol display' is setted in no.

for setting config, go to file>properties>drawing opetion

Best regards, Hongjie

T

tmorishita

1-Visitor

Harish,

I think you may be getting the .dtl file that comes with the inheritance. Have you tried loading and applying the .dtl file that your company uses? In WF5 this can be accessed from File, Drawing Model. You could also edit the existing .dtl file with the following: tol_display YES.

Hope this helps,

Tim

avillanueva

23-Emerald I

Was there ever a solution to this? I've seen many SPRs related to tolerances and inheritance features. In my case the base part is released and read only. You can vary a dimention in the child model but changing the tolerance is greyed out in part and drawing mode.

T

tmorishita

1-Visitor

I have noticed that when I bring drawings up in Creo the tolerance mode is greyed out. What I have found is that if I go to File, Prepare, Drawing Properties, then click the change in the Detail Options, it brings up a file in which the tolerance display is set to no. After I change that setting to yes, the tolerance is no longer greyed out. I don't know the reason for this, as my config.pro and my .dtl file both have the tolerance display set to yes, and the tolerance mode to plusminussym. I haven't played with Creo that much so I haven't been able to make it work correctly from the start.

V

vzak

Answer

12-Amethyst

Hello Hari,

Not sure if this will answer your question , just some info on Inheritance feature & tolerances :

1. When modifying Dim Properties of inheritance feature dimension, it is impossible to change Tolerance Mode. It is always the same as in base model. So if you have just "Nominal" type dim in core part, you will not be able to add any Tol on cavity it it uses core Inheritance cut. Same in 3D or in Drawing.

2. In general if you have some tolerance defined on base part dimension, its value can be easely modified on inheritance feature. Either through inheritance Varied Dimension table (show tolerances on the screen and pick one for Var Dims), or by direct edit/pick on TOL value on 3D screen. This should provide confirmation to add this TOL to varied items list and ytou should be able to proceed.

3. Do not try to use Properties dialogue to create/modify varied dimensions or tolerances - use direct selection of nominal / tolerances from the screen

4. When workingin show tolerances mode, you will not be able to make any modification to LIMITS type dimension of Inheritance feature - so hope you do not use LIMITS. Any other type (nominal, plus/minus, symmetrical) is available.

However if you switch off tolerances you can add any type of DIM to varied items of Inheritance feature ... since it handles all as nominal.

If this does not help feel free to ask more precise one.

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