Bolt Circle Issues - Dimensions

[GO_10898978]

Another day and another CREO issue 🙂

So, I'm starting to get into detailing parts in CREO 10. Just to clarify - I have used NX and SolidWorks before and never ran into this issue.

I wanted to dimension the part attached and use Bolt Circles for the two different holes. I tried using "Show Model Dims" and bring in the axis and dims. Well one feature was created using a circular pattern - and the other was two separate features (I did not create this model). I figured out how to display a circular centerline by changing drafting settings - but when I brought the dimension in it was a Radius. There was no way for me to change this to a Diameter. So, I decided to create my own sketches in the view and decided to just dimension to this directly. I'm sure people will say, "That's not how CREO works - you create in model and then bring in the model features/dims" Sure - but when it doesn't show what you actually want - I want to have other options/features to present the dimension how I want it. Well, when I placed the two Dimensions it doesn't scale to the drawing view. The 2.800 dia should be 0.560. The 2.500 dim should be  0.500 (as you can surmise - the scale of the view is 5X).. Why doesn't CREO scale secondary dimensions on sketched features??? When I click on physical geometry the dimension scales appropriately (which should be expected). Why does this happen - and is there a way to fix this?????

Thanks

[GO_10898978 · Accepted solution]

Ignore.

So I sketched the Bolt Circles on top of the view - but did not associate or link to that view. Once you do this then the dims scale. Trial and error - I learned. Thanks.

[MartinHanak]

Hi,

just a note ... you can also create Sketch feature representinf bolt circle inside the model. and set its line style in drawing.

[KenFarley]

When you sketch things on a drawing view, they're just "there" unless you relate them to the view. If you don't relate them, you get the dimensional wrongness you experienced. Another thing that can happen is if you move that view, any drawn items in the view that are not related to the view will NOT be moved along with the view. They are "left behind". A very unpleasant experience, to be sure.

[Kotom-Eng]

You are in the wrong forum.

PTC has two CAD systems:    Creo+ and Creo Parametric    and     Creo Elements Direct.

Which makes it confusing.

More, for Creo Elements Direct:

- The 3D software name is Modeling, and

- The 2D software name is Drafting.

For Creo+ and Creo Parametric, use only this tab:

You should move your post to this community to have a better chance to get an answer.

To move your post, click on the three vertical dots on your initial post and click on "Notify Moderator".

[kdirth]

In order to show the dimensions you want, you need to define the model in the same way.  I would suggest redefining the first hole from radial to diameter to show the diameter dimension.

Otherwise you need to add your own dimension.  Selecting the bolt circle twice will create a diameter dimension.  You can also change a created dimension by changing the "Orientation":