Pro/ENGINEER Tutorial 3 - Working with Datum Planes

In this tutorial, we will be discussing more advanced ways datum planes and axes can be used to create features. In many cases, the default trio of datum planes or existing surfaces of the part do not provide an appropriate sketch plane for the creation of a feature profile. The creation of datum planes and axes follow the rules of geometry. That is, only certain combinations of existing points, axes, planes, and scalar values can be used to unequivically define new axes (lines) and planes. These combinations of existing geometric elements are used in conjuction with datum creation commands. Options include:

In some cases more than one of these options must be used to definitely locate a new datum. For example, an angled datum might be creating by first defining the rotational aixs the plane passes through, then defining the angle the plane makes with an existing plane.

A good example of when new datum planes are needed, is when you create features on the curved surfaces of a part. We will create such a part in this tutorial.

Start is you have in the past two tutorials by creating a new part called con_ring.

Next, create the default datum planes.

Then, create the initial protrusion:

create>protrusion>extrude | solid | done>both sides

DTM2 will be your sketch plane, and DTM3 will be chosen as a Bottom reference plane.

The protruded disk will have an outer diameter of 2.5 and an inner diameter of 1.0 (see Note below). The thickness will be 0.375. As seen in Figure 1. Remember to align the circle centers to the datums.

NOTE: To place a diameter dimension, double click on the circle with the left button, then place the dimension with the middle button.

Figure 1

Next a through hole will be placed, bisected by DTM3 and DTM2 (see Figure 2).

Create the hole using the following commands.

create>solid>hole>straight | done | linear | done

DTM1 is your placement (sketch) plane and be aligned to DTM2 and DTM3, your two reference planes.

The hole will go Thru All on both sides and have a diameter of 0.16.

The next operation will be to create a new offset datum plane. This plane will be used to create a cut. An existing datum, DTM1 will be the parent plane to the new (child) datum.


Click on DTM1 as the reference plane.

Next choose Enter Value on the menu.

NOTE: Ensure the green arrow off of DTM1 is pointing to the right.

Enter 1.10 for the distance of the offset and click on done.

DTM4 will be created as seen in Figure 2.

Figure 2

Use the new datum, DTM4, as your sketch plane and DTM2 as the reference plane to make a Thru Next cut in the part. After choosing DTM4 as the sketch plane, ensure the arrow is pointing away from the center of the disc.

The cut, which will be referred to as a notch, will be 0.375 wide, centered on the horizontal reference plane of the disc, with a height the same as the thickness of the disc. The sketch only requires two elements: a center line aligned to DTM3 and a centered rectangle aligned to the top and bottom of the disk.

The final cut should look like Figure 3.

Figure 3

For the next operation, we will create an angled datum plane. Angled datum planes are defined in a two-step process: First defining the axis of rotation and then the angle of rotation (relative to some feature).

First, define the axis the plane will go through:


click on the axis perpendicular and through the center of the disc (Axis A_1).

Next, define the angle of the plane relative to DTM3:

angle>(click on DTM3)

The prompt line indicates the plane is fully constrained. Click done then click enter value

If arrow is pointing in the clockwise direction, enter -30. Or, if arrow is pointing in the counter-clockwise direction, enter 30.

See Figure 4 to see the location of the new plane, DTM5.

Now will we create a plane parallel to DTM5 and tangent to the outer surface of the ring. Again, this is a two step process to fully define the datum.


click on the newly created angled datum plane, DTM5 Now indicate that the plane will be tangent to the ring:


Using Query Select, click on the outer curved surface of the disk, above the angled datum plane. Make sure you select the curved perimeter surface of the cylinder, not the flat top. Now select:


See Figure 4 to see the location of the new datum, DTM6. Look at the figure to see the new hole and notch being cut. First create the hole.

Create a One-sided hole with a diameter 0.19. You can use DTM5 as the placement plane and align to the center axis of the ring and DTM2 for the references. The hole will go Thru Next, to the center of the disk.

NOTE: If you sent the hole going the wrong direction or did a two-sided hole, you can use redefine to correct it. See the changing features instructional sheet for more information.

Now use the newest datum, DTM6, to create another notch.

Create a blind notch will the same dimensions as the first notch (0.375 wide, centered about the centerline). Since the datum is on the outer surface of the cylinder, we will be cutting towards the center with a blind cut. The depth of the cut will be 0.15.

The part should now look like Figure 4.

Figure 4

Now we will create another angled datum plane and then an offset datum plane for another notch.


Click on the axis going through the center of the disc (Axis A_1).Then choose:

angle >(click on the first angled plane, DTM5)

The prompt line indicates the plane is fully constrained. Click done then click enter value

You will now be prompted for an angle. Enter 60, if showing clockwise direction. Enter 120, if showing counter-clockwise direction.

Using the angled datum plane, offset another datum plane from it. Refer to Figure 5.

create>datum>plane>offset>(pick the datum you just created, DTM7)>Enter Value

When prompted for an offset value, the arrow will be pointing up and to the right. You want the plane to go down and to the left. To accomplish this you will be going away from the green arrow.

Enter the value as a negative, -1.10.

Use the newest datum plane, DTM8, as a sketch plane and DTM2 as a reference plane.

Since this datum is offset so that it is inside the cylinder, you will be making a Thru Next cut away from the center of the cylinder.

Make a notch in the disc with the same dimensions as the original notch (0.375 wide, centered about the centerline).

The final part will look like Figures 5a and 5b.

Figure 5a

Figure 5b

Modifying Features Through Parent-Child Relationships

We are now going to modify features on the disk by modifying properties of the datums we have created and the features created on these datums. You may want to review the Changing Features mini-tutorial before you proceed with this part of the tutorial.

Before you begin, you should save your original file and create a new version for the next part of the tutorial.

File>Save As (call the new file con_ring_mod) Make sure con_ring_mod is the active window.

First, change the depth of the first slot by moving DTM4 backs towards the center of the disk.

Pick part>modify

and click on DTM4. Notice how the offset value of 1.10 appears as a dimension between DTM4 and DTM1.

Change this offset dimension to 0.60 by clicking on the dimension value and entering the new value (just as you do in Sketcher mode).

Regenerate to see the changes (Figure 6).

Figure 6

The slot profile sketch moves back because the sketch is a child of its sketch plane, DTM4 (i.e., DTM4 is the parent of the slot feature profile sketch).

Now change the location of the second hole and its slot. This will be done by changing the angle of the first angled datum, DTM5. The hole and slot are children of DTM6, their sketch plane. DTM6, in turn, is a child of DTM5. This set of dependencies means DTM5 can be used to drive changes in the location of the slot and hole. Change the angle:

part>modify (pick DTM5)

Change DTM5's angle to -60 and regenerate.

The change can be seen in Figure 7.

Figure 7

What else moved besides DTM6? DTM7 and DTM8 moved because they are also dependent on DTM5.

Now we will do two modifications to the third slot made off of DTM8.

First, redefine the slot from a Thru Next cut to a Blind cut.

feature>redefine (pick the slot cut on DTM8).

Now pick the Depth element in the Feature dialogue and then click on the Define button.

Redefine the element as a Blind cut with a depth of 0.20.

Then click OK in the Feature dialogue.

Notice any difference?

Now, modify the location of DTM8 to an offset of 0.60 and regenerate.

How does the slot look now? See Figure 8.

Figure 8

Finish by printing screen captures of both the original con_ring and the con_ring_mod parts.

rev 7/99 EW

Tutorial 4 - Simple Assembly

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