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Orientation of chamfer dimension in drawing

MichalLukac
4-Participant

Orientation of chamfer dimension in drawing

Hi,

Is there a way to switch orientation of chamfer dimension in drawing?

I mean the chamfer dimensions showed from model, not created in drawing.

(Creo 7)

a.jpg

 

Michal.

 

11 REPLIES 11
Mathpp
5-Regular Member
(To:MichalLukac)

Hi,

You can change the shape of the chamfer by drawing options.

 

Mathpp_0-1620304072652.png

 

When you have the drawing open, go to File -> prepare -> drawing properties

Click on "change" in the detail option.

Click on "FIND" and look for the command in the image above.

 

The commands shown above are from CREO 4, but I believe it should be the same for 7.

 

In addition, the dimensions taken from the Chamfer must come from the "Show models annotations"

The orientation of the shown dimension is based on the orientation of the feature.  In the model, edit the definition of the chamfer and flip its orientation.

kdirth_0-1620312548543.png

 


There is always more to learn in Creo.
MichalLukac
4-Participant
(To:kdirth)

But I have't this option ...... (Creo 7)

 

MichalLukac_0-1620319328069.png

 

I am on 4.0.  However there should be a way to determine what surface to measure the angle from.  The RMB menu or one of the tabs should have something.


There is always more to learn in Creo.
MichalLukac
4-Participant
(To:kdirth)

Just noticed, this option is available with angle x d but not 45 x d. When I use angle x d it shows both dimensions angle and d in drawing regardles setting in default_chamfer_text

Mathpp
5-Regular Member
(To:MichalLukac)

In the settings of the drawing I sent you, I believe that it has not helped you.

Have you tried to make the dimensions of the chamfer by "show models annotations"?

 

Br,

MichalLukac
4-Participant
(To:Mathpp)

Yes, the dimensions are showed from model, not created in drawing. The option You mention is for chamfer text format but only for chamfer of type 45xd . This setting is correct for me but for this chamfer type a cannot select orientation horizontal/vertical in this case. 

 

It would by fine if for chamfer of type angle x d would be possible to set text format dx45, because there is possible to change chamfer side in model.  

Mathpp
5-Regular Member
(To:MichalLukac)

I was able to understand what you need. I'll take a look at the manual and see if CREO 7 really has this option.

Add both dimensions to drawing and add one dimension to the other manually.  In the dimension text add "&d**" to place the dimension in the text.  Erase the referenced dimension.  Dimension names can be seen by Selecting Switch Dimensions.

kdirth_0-1620323771193.png

 

 


There is always more to learn in Creo.
MichalLukac
4-Participant
(To:kdirth)

yes this is one solution, but I think ineffective, imagine there are many chamfers dimensions they need to edit. Lot of work..... I use mapkey that adds x45° to the selected dimension.

 

anyway, thanks for help...

 

If there are many dimensions you want to edit and add the same thing, you can edit them all at the same time by selecting all of them then editing text as usual. It changes all simultaneously.

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