ME-546 Computer Aided Manufacturing

Lesson 8 -- Pipe Connector

 

Pro/ENGINEER Functions

Datum plane
Datum axis
Mirror

 

Design Objective

This lesson explains how you can use datums acting as references, to aid in geometry construction when sketching a feature, orienting the model, assembling components, or building the complex volumes that bound the solid model.

 

Modeling Strategy

I. Create connector body shown in Figure IV.8-2.

II. Create the datum planes.

III. Create the ear of the part.

IV. Use mirror function to construct another ear.

 

Detailed Construction

I. Create the connector body as shown in Figure IV.8-2.

1. PART - Create
2. Enter a part name [ connector ]
3. - Feature - Create - Protrusion - Done
4. Create the cross section as shown in Figure IV.8-3.
   Note: Use 3 Pt Arc and Concentric to create the cross section.
5. Dimension the sketch, modify the dimensions, and regenerate.
6. - Done
7. Enter extrusion depth [ 600 ]

II. Create datums.

Datums are very useful references for feature construction, model orientation and component assembly. Datum planes are used to create a handle or reference on the part where there is no appropriate planar surface. To select a datum plane, you can select its name (e.g. DTM1, DTM2). In the following material, you will learn how to create an extrude feature by using datum planes.

1. Create a datum axis:
1. FEAT - Create - Datum - Axis - Thru Cyl
2. Pick surface A as shown in Figure IV.8-2.
   A center axis will appear on the screen.
2. Create the first datum plane which has an offset distance from Plane B:
   The Offset option will create a plane which is parallel to a plane and is offset from the plane by a specified distance.
1. FEAT - Create - Datum - Plane - Offset
   Pick Plane B as shown in Figure IV.8-2.
2. Enter Value
3. Enter offset in the indicated direction [ -200 ]
   The green arrow indicates the direction which the datum plane will face. Entering a negative value in the above command indicates that you wish to place the datum plane in the opposite direction.
4. - Done
   A datum plane named DTM4 should appear on the screen. Be sure to set up Datums ON from the ENVIRONMENT menu.
3. Create the second datum plane which has an offset distance from the first one:
1. FEAT - Create - Datum - Plane - Offset
   Pick the first datum plane named " DTM1."
2. OFFSET - Enter Value
   Enter the offset value [ -200 ]
3. - Done

III. Create a flange on the part.

1. FEAT - Create - Protrusion - Extrude - Solid - Done
1. - One side- Done

Up to Surface features are created from the placement surface to a surface or datum plane that you select on the part.

1. - Setup New - Plane - Pick
2. Pick the first datum plane named " DTM2."
3. - Pick the datum plane named " DTM4." (The red arrow indicates the direction in which the feature will be created. In this case, it will be created between the two datum planes.)
4. Orient the sketch as shown in the figure
1. Sketch and dimension the extrusion cross section, as shown in Figure IV.8-4.
2. Align points A and B to the arc.
3. - Regenerate
4. Modify the dimensions.
5. - Regenerate - Done - Direction -Okay
6. - Up to Surface - Select by Menu - Datum
7. Choose DTM5
2. MAIN - View - Orientation - Default - Done/Return

IV. Create another flange by using the Mirror function.

1. FEAT - Mirror Geom
   Select the third datum plane named " DTM3." This datum plane acts as the "mirror" about which the flange is mirrored; the second flange should now appear at the bottom of the connector part, and your part should now look like the one in Figure 8-1.

Redefine the second protrusion to create a thin concentric cylindrical channel instead of a solid rectilinear one and include it as a separate file.