Diameter dimension in sketcher

[KevinGarrett]

Is there a way, when sketching a revolved protrusion, to get the default(shown) dimensions to display the diameter of the sketch instead of the radius?
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[WillyC]

Shown dimensions show the number as it appears in the sketch. If you dimension your sketch as a diameter--- click sketched line, centerline, and then sketched line again--- you will be able to "show" it as a diameter.

[KevinGarrett]

What I mean is that when you sketch a revolved protrusion, Pro adds dimensions to the sketch from the centerline to the sketched line. I then must re-dimension the sketch to get the diameter, sketched line, centerline, and then sketched line again. It's this re-dimensioning that need to be avoided.

[RodneyDecker-di]

In the sketcher mode I have placed a point on the opposite side of the centerline, constrain it and the edge of the sketch where I wished to pull the diameter, then dimension between the points.

[WillyC]

Oh, gotcha. Good idea. I just found this. Haven't tried it yet. According to p.141 of WF4 Config Options, add 'sketcher_dim_of_revolve_axis' to config.pro and set to YES. Description: If this option is set all dimensions created by Intent Manager to Axis of Revolution will be diameter dimensions. Give it a shot.

[KevinGarrett]

Willy, That config option is exactly what I was looking for. Thank you!

[BillDaugherty]

I will try posting this elsewhere also, but just wondered. Does anyone have a comprehensive list of all config options? Used to have one years ago, but cannot place it now. I am sure there have been additions over the years as well with the new revisions. Thanks !

[pwyndham]

They are on PTC's website.

WF4: http://www.ptc.com/WCMS/files/65779/en/WF4.0_012408_configoptions.pdf

WF5: http://www.ptc.com/WCMS/files/99859/en/WF5M060configoptions.pdf

Not sure if you need specific login access to get to the docs. If you do, let me know and I will see if I can upload them on to PlanetPTC

[DennisRehmer]

Paul,

I know you posted this back in 2010, but it is just what I was looking for today. The config options for WF4.0.

I was able to get to this without any problems.

Dennis

[TomD.inPDX]

FYI, Creo does this by default now. It seems to re-evaluate the sketch each time you click the "add dimension" button. Once you add a proper centerline(*), it changes your radial intent dimensions to diameters. It does this with angles as well which is a nice improvement from 2000i.

(*) I didn't know we had dedicated centerlines for rotation in Creo (2000i didn't have this). Drove me nuts! ...but I understand why this was needed as you could only use one centerline in 2000i "successfully" in rotations.

[s.iyer]

With effect from WF5, PTC has introduced "Geometry Centerline". Sketch the geometry cl first and then sketch the profile for revolve protrusion. The dimensions are then taken as Diameter Diamensions.

I know this is an old post. I am still posting it if it helps somebody.