Product Design Engineering: NX Surface

Impeller Blade:

Build the impeller using wireframe profiles, revolved features, imported geometry, and free form features.

1: Create a new part in millimeters. Assign the part any name but create it in the directory assigned to your workstation or your home directory.

2: If your company has a layering convention, use it instead of the layers specified throughout the project. Try to keep the different profiles on separate layers because you use them in different operations as this project progresses.

3: The two profiles are built in the RIGHT view. Orient your WCS so the XC-YC plane is in the same plane as the Right view, and the origin of the WCS is located at the (0,0,0) location of the Absolute Coordinate System. If you are comfortable using Sketcher, create both profiles in different sketches. Create the three fixed datum planes or use a Datum CSYS to attach the sketches.

4: Start by creating the wireframe profile shown. You use these curves to create the hub for the impeller blade. Create this geometry on Layer 5. Make a note of the WCS location as shown. The profile consists of three lines, one (full radius) fillet, and one optimized curve that pass through four defined points. Make the slope of the optimized curve match the slope of the 1.5mm fillet and as smooth as possible with no reversals in curvature.

5: On Layer 6, create the second wireframe profile as shown. You will use this profile to create a trim sheet for the blades. Make a note of the WCS location in the diagram. The profile consists of one line, one fillet, and one optimized curve that pass through the four points. Make the curve tangent to the 9.5mm fillet and as smooth as possible with no reversals in curvature. Use the same optimization tip as specified for Profile A.

6: Profile A creates the inside hub solid body and Profile B creates the sheet body that trims away the top of the impeller blades. Revolve Profile A about the long horizontal line from 0 degrees to 360 degrees on Work Layer 10.

7: Change the Work Layer to Layer 11. Revolve Profile B into a sheet body, 360 degrees about the same axis as Profile A. Remember to save your part.

To create a sheet body, you must change the settings for Solid to the Sheet setting. Even though it is an open profile, when it revolves the ends are planar and therefore NX closes the ends and creates a solid body.

8: The data for the blade profile has been created in another part file. This part file contains the geometry necessary to create a solid body using free form features. Import the part blade_profile.prt on Layer 15 and orient it to the Absolute Coordinate System.

You can orient the WCS to the Absolute Coordinate System before importing the profiles or specify a CSYS during the import.

9: Create a solid body on Layer 16 through the 14 curve profiles using Through Curves. Use a Parameter alignment and the Preserve Shape toggle activated. Check your solid body to make sure there are no twists.

10: To create the other 11 solid bodies, use the Pattern option. This option allows you to create the other blades while maintaining associativity to the original. The 12 blades should be equally spaced around the hub.

11: After you create the 12 blades required for this part, you need to trim away the upper portion using the sheet body produced by Profile B, located on Layer 11.

Unite the blade to the hub.

12: Create a 60mm diameter thru hole through the center of the hub.

Review: In this project, you created an impeller by using both imported and parametric geometry. By this method, changing the hub profiles defined by Profile A and Profile B is accomplished quite easily. Changing the number of blades in the impeller is also easy. However, changing the blades themselves is a more difficult task because they are constructed from imported geometry. You could change the curves in the impeller file individually, or import a new file, which necessitates adding and removing string from the existing blades. Keep these factors in mind when creating your models and estimating the time necessary to complete the part.

Control Pad Task:

Main commands used:

Ruled
Through Curves

Process: Construct a series of datum planes that you use as attachment faces for sketch profiles. You will create and constrain three separate sketch profiles. Then you use these sketch profiles to create ruled bodies. Remember to place your geometry on separate layers.

1. Create a new part file in your home directory called control_pad. Make sure to set the units to Millimeters.

2. Create an offset datum plane from the Z-X plane at a distance of 150mm.

Create another offset datum from the first offset datum by 75mm.

3: Create a sketch called Profile_1 on the Z-X plane of the datum coordinate system. Make sure the vector normal (Z-axis of the sketch) points in the -Y direction.

Use the X datum axis as the horizontal reference. Make sure the X vector of the sketch points in the X direction. Create the curves as shown.

Make Line 1 collinear to the vertical datum axis or plane, and Line 2 collinear to the horizontal datum axis or plane.
Place the arc's center on Line 1.
Mirror the sketch about Line 1.
Create the sketch dimensions as shown.

Use Insert | Sketch in Task Environment

Assure Continuous Auto Dimensioning is toggled off.

Finish the sketch.

4: Create a sketch called Profile_2 on the 150mm offset datum plane. Make sure the vector normal (Z-axis of the sketch) points in the -Y direction. Use the X-Y datum plane as the horizontal reference. Make sure the X vector points in the X direction.

Create the curves as shown.

Make Line 1 collinear to the vertical axis or plane, and Line 2 collinear to the horizontal axis or plane.

Place the arc's center on Line 1.
Mirror the sketch about Line 1.
Create the sketch dimensions as shown.

It may help to hide the first sketch to avoid confusion.

Finish the sketch.

5: Create a sketch called Profile_3 on the 75mm offset datum plane. Orient the sketch in the same way the first two were oriented. Create the curves the same way you did the first two sketches.

Make Line 1 collinear to the vertical axis or plane, and Line 2 collinear to the horizontal axis or plane.

Place the arc's center on Line 1.
Mirror the sketch about Line 1.
Create the sketch dimensions as shown.

Finish the sketch and hide all of the datums.

6: Create a ruled body, goto Insert | Mesh Surface | Ruled, using Profile_1 and Profile_2. Make sure to select both profiles from the same location to force the arrows in the same direction. Use Parameter as the Alignment and activate Preserve Shape.

7: Create a second body but this time use Insert | Surface | Through Curves command using Profile_2 and Profile_3. Again, select both section strings in the same manner. Use Parameter as the Alignment and activate Preserve Shape.

Set the Continuity for the First Section to G1 (Tangent) and select the 5 faces of the first solid body as shown. Select Perpendicular in the Flow Direction drop down menu.