dual dimension

[dpinho]

Hello mates


I am having the hardest time placing second dimensions on my drawing. My case is complicated because I want to show All dimension in mm apart from a single one which should be in inch. Any ideas?


Sorry for the elementary question, but I

 

[PRStockhausen]

You could create the inch dimension and overwrite the text. Change the "@D" to "@O" and add text to show the inch value. Or you could create a parameter to be the inch value, relate the metric dimension to the parameter and use the parameter in your created dimension. Do not forget to indicate that the dimension is in inches.

 

[dpinho]

Thanks for replying.


The second manner seems the best, so it keeps the link with 3D model. I just couldn

 

[PRStockhausen]

For your example use: "@o@inch"

 

[trillicomm]

dpinho

you model in inches or mm?

 

[dpinho]

it

 

[vlad1979]

Create the relation in part relations. It's got nothing to do with drawing parameters. So don't create any drawing parameters, create all parameters in your part.


So in part relations write inch=d56/25.4 (as you say the part is in mm then you need to divide it by 25.4 to convert to inch) then in your drawing create a dimension (not show/erase because it's not working) then right click on it / properties and delete the D and write @O&inch


PS: You don't have to create the parameter "inch" you can directly enter the relation and the parameter will be automatically created as real number, you create parameters for relations when you want specific types: integer, string, yes/no .........

 

[trillicomm]

I agree with VLAD.

 

[dpinho]

Cheers Mate.


There must be some configuration option that is blocking me. But I

 

[PRStockhausen]

Check to see of you have the config option "CreateDrawingDimensionsOnly" set to yes. If you change it to no, the "@o@inch"should work.

 

[dr_gallup]

The dimension must be created in the drawing. You can not use @O in shown dimensions.

create_drawing_dims_only has nothing to do with it.

 

[PRStockhausen]

When the "create_drawing_dims_only" option is set to yes, the &inch is shown as &inch instead of the value of the model parameter inch. When it is set to no, the value shows correctly.

 

[ravindth]

For your example use: "@o@inch"

Hello,


Kindly reply me as soon as possible for the following question relatedon the Pro-E Drawing.


Qustion: How to Update the Date and Time Automatically in a drawing sheet whenever open. Means, If I open a part drawing at tomorrow then, at the right side should be shown the updated date and time.


I am waiting for your answer... Thanks a lot

 

[PRStockhausen]

You should post this as a new topic.

 

[ravindth]

ok

 

[ravindth]

Sorry for silly question,


I have requested new topic and posted.. But Can u say that from where to get?

 

[dr_gallup]

When the "create_drawing_dims_only" option is set to yes, the &inch is shown as &inch instead of the value of the model parameter inch. When it is set to no, the value shows correctly.

I have the "create_drawing_dims_only" option set to yes and I can show all model parameters correctly with the &parameter notation. This config parameter only controls whether created dimensions are stored in the drawing or in the part file.