One-sided diameter dimension

[Sergey]

Hello.

How do I show one -sided diametral dimension in Creo drawing application as shown below?

Best regards,

Sergey

[tbraxton]

If you use a shown dimension in a drawing view it will appear with arrows across the diameter. After showing the dia dimension use the flip arrows options and it should create what you want.

[Sergey]

It is not so simple.

I have made a Detailed view of a cross-section. Center line isn't there to create a diametral dimension. Any thoughts? 

[StephenW]

Show your dimension from the model OR create your dimension in the main view and move it to the detail view OR temporarily change your detail view boundary to include the centerline, create the dimension, then re-sketch the boundary as desired.

[StephenW · Accepted solution]

Select the witness line you want to remove then RMB erase witness line.

Depending on your drawing settings, you will get different results. If you need to, go to file - prepare - drawing properties - detail options change

and set the option clip_dim_arrow_style NONE

then you can "drag" the "none" arrow side to however you want it.

[Sergey]

Hello again.

Thanks for help. It worked. 
Please, combine both your posts into one so that I will be able to accept it as the complete solution.

Sergey

[Sergey]

One more question, if I may:

How do I convert linear dimension into diametral?

[StephenW]

If you've already created it, select the dimension, then in the ribbon, select DISPLAY, then "double value" toggle box

If you are creating it, RMB just before placing the dimension and the "double value" option is there.

You have to add a diameter symbol

[JS_9824412]

It works. Thanks for the teaching. 

(However, there is still some bug in CREO 6, as shown in below snapshot. One dimension is right, the other is wrong)