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How to convert radial dimensions to diameter dimensions automatically

atrukhin
1-Newbie

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.

1 ACCEPTED SOLUTION

Accepted Solutions
psobejko
12-Amethyst
(To:atrukhin)

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.

View solution in original post

13 REPLIES 13
MartinHanak
23-Emerald V
(To:atrukhin)

Hi,

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

MH


Martin Hanák

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.

MartinHanak
23-Emerald V
(To:atrukhin)

Hi,

you have to set config.pro option mentioned by Tim Morishita

MH


Martin Hanák

Have you tried setting this config.pro option?

sketcher_dim_of_revolve_axis yes

Sure. No changes.

Kevin
10-Marble
(To:atrukhin)

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.

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

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

psobejko
12-Amethyst
(To:atrukhin)

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.

Kevin
10-Marble
(To:psobejko)

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.

Hi,

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

MH


Martin Hanák
bmohapatra
5-Regular Member
(To:atrukhin)

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. 

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`.

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