4.3.3 Creating planes

In this exercise you'll learn about the feature Datum Plane.

Open the model block, if you previously created it. Otherwise create the model block according to the naming convention and add a block with the following dimensions to it:

Dimension	Value [mm]
Length	200
Width	100
Height	50

Plane defined by surface

Select Datum Plane alt .

Should a plane be aligned with a body surface, just select the surface and enter 0mm as distance.
The plane appears after confirming with OK. (refer figure "Plane defined by surface")

Plane at a distance to a surface

Again, select the desired surface by clicking on it. An arrow that indicates the positive direction appears. Since the plane should be located within the body, enter -20mm as distance. Clicking OK creates the plane. (refer figure "Plane at a distance")

Plane at an angle to a surface

Open alt .

As positioning method, choose .

In the first step, select the surface that the angle should be measured from. Next, select the edge that the plane should run through. Now enter 30 as Angle. Clicking OK creates the plane. (refer figure "Plane at an angle")

Planes on cylindric surfaces

Open the model cylinder, if you previously created it. Otherwise create the model cylinder according to the naming convention and add a cylinder with the following dimensions to it:

Dimension	Value [mm]
Diameter	20
Height	50

Plane in the center of a body

between two flat surfaces

Open alt . Select the first flat surface by clicking on it. (refer figure "Menu center plane")

NX now offers a proposal for the new plane - just ignore it!

In the second step, select the second flat surface as seen in the picture on the right. NX now places the plane in the center between both surfaces.

Confirm by clicking OK. (refer figure "Center plane created")

Hint:

The disadvantage of creating a plane in the center of a body by specifying an offset is that it won't be located in the middle after later changes to the dimensions of the body. To avoid this, you can enter a parametric offset (refer chapter 4.6 parametrics) or create the plane defined by two parallel surfaces, as explained above.

Plane through a cylinder shell

Open alt .

Click the centerline of the cylinder (Not the coordinate system, but the blue dashed centerline!). The Datum plane appears in the center of the cylinder.

Confirm by clicking OK. (refer figure "Plane across")

Tangent plane

Open alt .

Highlight the cylinders mantle. (refer figure "Tangent plane")

NX now also needs a second reference - a point that the tangent plane should run through. Select the circular edge of the cylinder. (refer figure "Tangent plane with point")

Make sure that Quadrant Point alt within Snap Point toolbar is activated. A point of reference appears on the surface, through which the plane runs.

Confirm by clicking OK.

Hint:

When you press return/enter after entering values for planes, NX renders a preview of the respective plane. Only by clicking OK the plane is actually created.