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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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.
you cannot convert radius to diameter. You have to create new diameter dimension and delete radius dimension on demand.
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.
I tested the option. It is related to sketcher dimensions created automatically by Intent Manager.
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.
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.