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Dec 7, 2016 1:35 PM UTC
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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.

    psobejkoAnswer
    Dec 8, 2016 3:05 PM UTC

    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

    Dec 7, 2016 2:45 PM UTC

    Hi,

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

    MH

    atrukhinAuthor
    Dec 7, 2016 3:34 PM UTC

    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.

    Dec 7, 2016 3:56 PM UTC

    Hi,

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

    MH

    Dec 7, 2016 3:32 PM UTC

    Have you tried setting this config.pro option?

    sketcher_dim_of_revolve_axis yes

    atrukhinAuthor
    Dec 7, 2016 3:35 PM UTC

    Sure. No changes.

    Dec 8, 2016 2:16 PM UTC

    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.

    Dec 8, 2016 3:46 AM UTC

    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. 

    atrukhinAuthor
    Dec 12, 2016 5:57 AM UTC

    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`.