Pro/rNGINEER Wildfire Tips & Tutorial (Pro/E Wildfire 4.0, Wildfire 3.0, Wildfire 2.0 and 2001)

TIPS: Dimensioning Techniques in Pro/E Sketch

(FLASH) TIPS: Dimensioning Techniques in Pro/E Sketch

Version: Wildfire, Wildfire2.0, Wildfire3.0

Sketcher dimensioning is very important because it directly reflects our 3D model in Pro/E. Most of the geometries are pretty easy and straightforward, however some require special techniques. Below are 5 special case dimensioning techniques in ProE sketcher.

A. Diameter dimension in revolve feature (instead of linear type)

To create the diameter type dimension in sketch, select (LMB)

1: the desired object
2: the centerline (revolve axis) and then
3: the desired object again.
After that, hit the MMB to place the dimension.

Or alternatively, select (LMB)
1: the centerline (revolve axis)
2: the desired object and then
3: the centerline (revolve axis) again.
After that, hit the MMB to place the dimension.

B. Diameter dimension for Arc (instead of radius)

By default, a radius dimension will be created when dimensioning an arc. To create the diameter dimension for arc, select (LMB) the arc twice and then place it by clicking the MMB.

C: Dimensioning Arc Angle

Most of the people I met normally create centerlines or construction lines when they need the included angle of an arc. By knowing this tricks, you can saves some clicks next time when you want to dimension the included angle of an arc.

To create the included angle of an arc, select (LMB)
1: end point of the arc (side 1)
2: end point of the arc (side 2) and
3: the arc
** selection order is not important here. As long as these 3 items are selected, the dimension can be created.
Next, hit the MMB to place the dimension.

D: Dimensioning Arc Perimeter

Select the arc (highlighted in RED when selected).
In the menu, click Edit> Convert To> Perimeter.
Next pick an arc dimension which you want it to be driven by perimeter.
** Note that you can specify the arc perimeter now and the dimension you have picked become vary dimension.

E. Dimensioning the angle at the end of a Spline

Besides dimensioning the points of a spline, you can also create and control the angle at the end of a spline. This angle allows us to control the spline tangential and it is important when we are dealing with symmetrical object or we need to specify a draft angle for object.

To create the angle, select (LMB)
1: the spline curve
2: spline end point
3: the reference plane / line
** Again, the selection order is not important here. As long as these 3 items are selected, the dimension can be created.

Next, hit the MMB to place the dimension

ENJOY!!

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