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12-07-2016
08:35 AM

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12-07-2016
08:35 AM

How to convert radial dimensions to diameter dimensions automatically

Hello,

Does anybody know what command is responsible for converting radial dimensions to diameter dimensions when one works in a sketch mode within a model? Refer to the attached images.

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12-08-2016
10:05 AM

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12-08-2016
10:05 AM

I work in Creo 2.0. Note that I've configured my system such that sketches start out without any "pre-selected" references.

So when creating the sketch that defines the section in a revolve feature, first thing I do is defines the axis of revolution. I do this by right clicking in the empty graphics area and choosing "Axis of Revolution". After I draw this special axis, then when I sketch my geometry lines that define the section, Creo automatically puts in (weak) diametral dimensions.

If I try to do it backwards and first draw the section and then designate the axis of revolution centerline, I **do not** get an "automatic" conversion from radial to diametral dimensions.

So to answer your original question, there is no setting that will "convert" radius dimensions to diameter dimensions, but there is a workflow where the diameter dimensions will be automatically created.

13 REPLIES 13

12-07-2016
09:45 AM

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12-07-2016
09:45 AM

Hi,

you cannot convert radius to diameter. You have to create new diameter dimension and delete radius dimension on demand.

MH

Martin Hanák

12-07-2016
10:34 AM

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12-07-2016
10:34 AM

Let me be more precise. Here is the link to the video: Видеоурок Creo Parametric 3.0 Моделирование цапфы. - YouTube . The issue that I concerned with is raised at 1:18. Take a closer look - the diameter dimension appears automatically instead of the radial dimension.

12-07-2016
10:56 AM

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12-07-2016
10:32 AM

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12-07-2016
10:32 AM

Have you tried setting this config.pro option?

sketcher_dim_of_revolve_axis yes

12-07-2016
10:35 AM

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12-07-2016
10:35 AM

Sure. No changes.

12-08-2016
09:16 AM

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12-08-2016
09:16 AM

The dimension you show looks like it may be a strong or locked, if so it won't change when you a geometry centerline. It only works with weak dimensions.

12-08-2016
09:26 AM

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12-08-2016
09:26 AM

I misunderstood your question. If you want a radial dimension **instead** of a diameter set the option sketcher_dim_of_revolve_axis no.

12-08-2016
09:43 AM

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12-08-2016
09:43 AM

I think you understood correctly and your first response was correct, the images shown appear to be posted in reverse order.

12-08-2016
10:05 AM

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12-08-2016
10:05 AM

I work in Creo 2.0. Note that I've configured my system such that sketches start out without any "pre-selected" references.

So when creating the sketch that defines the section in a revolve feature, first thing I do is defines the axis of revolution. I do this by right clicking in the empty graphics area and choosing "Axis of Revolution". After I draw this special axis, then when I sketch my geometry lines that define the section, Creo automatically puts in (weak) diametral dimensions.

If I try to do it backwards and first draw the section and then designate the axis of revolution centerline, I **do not** get an "automatic" conversion from radial to diametral dimensions.

So to answer your original question, there is no setting that will "convert" radius dimensions to diameter dimensions, but there is a workflow where the diameter dimensions will be automatically created.

12-08-2016
10:17 AM

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12-08-2016
10:17 AM

For me, also using Creo 2, I can either create the axis of revolution and then the geometry or the geometry and then the axis of revolution. For the second case the dimensions that would get changed to a diameter need to be week dimensions in order for them to convert automatically, strong or locked dimensions don't.

12-07-2016
10:49 AM

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12-07-2016
10:49 AM

Hi,

I tested the option. It is related to sketcher dimensions created automatically by Intent Manager.

MH

Martin Hanák

12-07-2016
10:46 PM

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12-07-2016
10:46 PM

The centerline which acts as a central axis for revolve is the real cause of the diameter dimension. If the centerline is removed the dimension automatically taken from the reference.

12-12-2016
12:57 AM

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12-12-2016
12:57 AM

Dear All,

Thank you very much for all your answers. Although I`ve already chosen the right answer, I will highlight the main stages in creating diameter dimensions:

1. Set sketcher_dim_of_revolve_axis yes in config.pro;

2. Create a new model;

3. Choose `Revolve` in the model Ribbon (it will help Creo to understand that you are going to create a solid revolution)

4. Draw `Axis of revolution`;

5. Draw the intended profile;

6. Click `Ok`.