Drawing shows bolt-hole pattern, but no dimension

[jraice]

New to Creo 3.0 coming most recently from NX 8.5 (fun learning curve so far!).

After a bunch of fumbling, I got my drawing to show the bolt-hole pattern with the dashed line, but I cannot get the diameter to display in the drawing for the pattern.

I made the first hole as a diameter placement, used a pattern with the degrees/qty, and have the radial_axis_pattern_circle activated.

Any help would be appreciated, thanks!

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[rcrerar]

Hi, I don't understand why this wouldn't work other than the syntax of the variable is wrong. Should be radial_pattern_axis_circle set to yes.

[StephenW · Accepted solution]

I read that wrong...I agree with Roy. Verify the config option.

Also, I seem to remember if you create the pattern BEFORE applying the setting, the model doesn't update. You may need to recreate the pattern again to get it to show.

To test this, after having the option set, create another hole and pattern it. If that diameter axis shows up on the new one but not on the old one, you'll need to delete and re-create your original pattern.

[StephenW]

Are you SHOWING dimensions or trying to create the diameter dimension in the drawing? You can SHOW MODEL ANNOTATIONS by selecting the view to get your model dimensions to show. Oddly, you can't select the bolt circle diameter (radial axis) to create a dimension, it's one of those odd things in creo.

[jraice]

Thanks guys, let me give it a shot. I can't remember if I set the radial_pattern_axis_circle before or after making the pattern. I am trying to do in Show Model Annotations as mentioned.

Also, once I do get it working, is there anything special needed to save this configuration so it defaults to yes? There are options in the Configuration Editor and the drawing specific options, do both save fully?

[jraice]

. Well, I ensured the setting was on yes, then I deleted and re-performed the pattern, and not only does Show Model Annotations not show the bolt hole pattern, but the circular symbol around the diameter is gone as well.

Am I correct in dimensioning the initial hole placement as a Diameter rather than Radial?

[StephenW]

Just to be sure, you are wanting the axis to show something like this, correct?

Creating your first holes as diameter is correct provided that is the dimensioning scheme you are after.

I apologize again for mis-speaking, the option is only a drawing setup option, not a config.pro option.

Drawing setup option is in the drawing under file - prepare - detail options change

radial_pattern_axis_circle YES

I'm not sure why yours isn't working.

I created the initial hole as a diameter type specifying bolt circle diameter and angle from datum.

I created the pattern using AXIS instead of dimension pattern but I tested the dimension pattern and it worked too.

[jraice]

Appear to have got it! When clocking show model annotations and clicking in the general area of the part, I was not selecting the entire view but some subset (datum perhaps?) thus it was giving me far less options for dimensions to show.

[JonathanHodgson]

Time to turn off preselection highlighting and learn to use Query Select instead.  This gives you clear visibility of exactly what you're about to select.