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Diameter dimension in sketcher

KevinGarrett
Newbie

Diameter dimension in sketcher

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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10 REPLIES 10

RE: Diameter dimension in sketcher

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.

RE: Diameter dimension in sketcher

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.

RE: Diameter dimension in sketcher

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.

RE: Diameter dimension in sketcher

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.

RE: Diameter dimension in sketcher

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

Re: RE: Diameter dimension in sketcher

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 !

Re: RE: Diameter dimension in sketcher

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

Re: RE: Diameter dimension in sketcher

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

Re: RE: Diameter dimension in sketcher

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.

Re: Diameter dimension in sketcher

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.

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

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