Bolt circle dimensions on drawings

[ptc-2708796]

I'm having a heck of a time figuring this simple thing out. I'm trying to dimension a bolt circle. I have a circular centerline on the drawing that is a shown centerline created by selecting holes around a flanged part and I can't select it for dimensioning the diameter. Is there some easy way to create a bolt circle diameter on a drawing?

[ptc-2192247]

In the past I have done it two ways: 1.Sketch a circle on the drawing over the bolt holes and dimension it-this only works if the scale of the part is 1.000. 2.Sketch a circle over the bolt holes, then add a note to the circle-the note is so you can type the dimension when the scale is not 1.000. This method is not the correct way (i do not believe), but I couldn't figure out the bolt circle either so i cheated. I am also interested to hear if someone knows the correct way?

[ptc-2708796]

Your 2nd way was the method I ended up using for now, but I'm going to keep trying to find a better way. Thank you for the help. I'll post back up if I do find a way.

[KlausKirchner]

Hello Gregory, if you want to have this dimension you should create the hole with the option diameter. So you can show it on the drawing. If the hole is patterned you can even show the circle when you show the axis of the holes. Perhaps you need the drawing setup option "create_radial_pattern_axis_circle" (or something like that, it`s just out of my mind) Please don`t sketch it on the drawing. Good luck

[RickGiguere]

Are you trying to get a diameter for a bolt pattern around a flange. I got this to work by enabling show hole diam in the drawing properties.

[RickGiguere]

Use "diameter" when you create the hole like kraus suggested. I used a dimension for the pattern, this will show the hole diameter if you enable it in drawing options.

[RickGiguere]

"Richard Giguere" wrote:

Use "diameter" when you create the hole like kraus suggested. I used a dimension for the pattern, this will show the hole diameter if you enable it in drawing options.

[ptc-2708796]

Thank you Klaus, that was exactly what I needed. Thank you everyone else as well for your input.

[Theron]

Can you explain in detail, like i'm 10 how to do that...  Create diameter with "diameter&quot

[kdirth · Accepted solution]

On drawing:

* Select - File / Prepare / Drawing Properties

* Select – change for Detail Options

* Select Find button, type in “radial” and select Find now button.

* Select radial_pattern_axis_circle option and change value to yes.

* Select Add/Change button then Close button.

* Select OK button on Options screen.

*Select Close button on Drawing Properties screen.

* Select Annotate tab and select Show Model Annotations.

* Select Datums tab (last tab) and select view showing pattern.

* Select a hole axis and the entire bolt circle will be added.

* Select Apply button

* Done

To show the diameter dimension, the original hole needs to be created with a diameter dimension.

[cgorni]

This information can also be reviewed in the following Knowledge Base article:

• CS54576: How to display radial pattern axis circle in a drawing in Creo Parametric

[Phillip1]

Well Done @kdirth !

[SandraGreenman]

You can still use the method of creating the construction circle in the drawing regardless of the scale if, after creating the construction circle in the drawing, select the circle, right click, and select "relate to view". This will treat the sketched geometry as if it has the same scale as the view. Another way to do this is to create a cosmetic sketch in the model and then show it on the drawing.

[cgorni]

If using a Cosmetic Sketch in the model to simulate the axis in the drawing you may be interested by the following articles to manage its line style or control its visibility per view:

• CS52299: How to change the line style for Cosmetic Sketch in Creo Parametric

• CS58372: How to control the visibility of features/datums in specific views on a drawing in Creo Parametric

The following article may provide more details on using the Relate to view command to control the scale of Draft entities:

• CS249920: How to create sketches with different scales in the same drawing in Creo Parametric