Impeller Blade Project

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.

NX - Fan Blade Project

Objectives

• To create a Fan Blade using basic and advanced features. Surface development, using sheet bodies, is necessary to manage a challenging draft issue.

Overview

You will use Sketch, Ruled Surface, Trim Body, and Extract to develop the model. 

Prerequisites

• If there is difficulty finding the feature or command please type it in to the Command Finder to find its pathway with in NX.

Instructions:

Step 1:

Create a new millimeter file called fan_blade.prt using a Model template.

Step 2:

Press the W key to hide the display of the WCS.

Step 3:

Create a Cylinder with a diameter of 39 and height of 21.5 in the positive Z direction.

Step 4:

Create a Sketch on the XY plane as shown.

Step 5:

Extrude the sketch 40 in the positive Z direction with a 1.0 degree draft using From Start Limit. Do not unite the two solids.

Step 6:

Create another Sketch on the XZ plane. Be sure the orientation of the sketch is altered as shown.

Create and constrain the following curves. The reference line is used to define a tangent constraint with the arc. The reference line should also contain a Constant Length constraint.

Step 7:

Select Curve tab > Derived Curve group > Derived Curve gallery > Section Curve to create a section cutting through the indicated arc, with the YZ plane. This should produce a point.

Step 8:

Create a Datum Plane using the XZ plane and section point just created.

Step 9:

Create a Sketch on the Datum Plane just created oriented as shown.

Constrain two arcs using the following constraints. The 15 dimension measures the location the two arcs meet.

Step 10:

Select Surface tab > Surface group > More > Mesh Surface gallery > Ruled to create Ruled surface using the two previously created sketches. Be sure to deactivate Preserve Shape and use the Arc Length alignment method. Using the Arc Length alignment method eliminates a tangent line created if the Parameter Alignment method is used.

Step 11:

Select Home tab > Feature group > More > Offset/Scale gallery > Offset Surface to create an Offset Surface upward with a distance of 1.5.

Step 12:

Use Trim Body to trim the blade solid using the surface just created by the offset.

Step 13:

Hide the top surface and select Surface tab > Surface Operations group > More > Trim gallery > Divide Face to divide the outer tangent vertical faces of the blade solid using the bottom surface as the dividing object. Be sure that Hide Dividing Objects is active.

Hide everything but the two solids and the Datum Coordinate System.

Step 14:

Select Home tab > Feature group > Draft to create a 10 degree draft using the positive Z direction for the Draw Direction and the newly created edges as the Stationary Edges.

Step 15:

Create an Edge Blend with a radius of 1.5 around the tangent edges of the blade solid.

Step 16:

Show the original Ruled surface and use it to Trim the bottom side of the blade solid.

Step 17:

Select Home tab > Feature group > More > Associative Copy > Pattern Geometry to create two more blades, using a Circular layout, a Count and Pitch spacing and a 120 degree angle.

Step 18:

This step removes the extra material on the inside of the blades interfering with the center cylinder.

Perform three Subtract operations making sure Keep Tool is active.

The blade is the target and the cylinder is the tool.

Step 19:

The next few steps will be used to create draft on the cylinder. Since the draft is required on both sides of the cylinder (bottom & top) a parting line needs to be developed. Start this by creating a sketch on the YZ plane as shown.

The sketch consists of only two lines and is coincident to corners of the blades.

Step 20:

Select Curve tab > Derived Curve group > Project Curve to project the sketch you just created on to the cylinder face in the positive X direction.

Step 21:

Use Pattern Geometry to copy two more projections around the cylinder. Use a Circular layout, a Count and Pitch spacing and a 120 degree angle.

Step 22:

Use Divide Face to divide the projections and top edges of the blades around the cylinder face. Hide Dividing Objects should be active. Select the outside face of the cylinder for Faces To Divide. Select the projected curves and the top edges of the blade as the Dividing Objects.

Hide the blades.

Step 23:

Add a 2 degree draft using the To Parting Edges type. Use the positive Z direction for the Draw Direction, pick the top cylinder face as the Stationary Plane and pick the newly created edges as the Parting Edges.

Step 24:

At this point draft has been added only to the top side of the cylinder. If draft is attempted on the bottom side, an error is given. Before we get much farther, let's see how the cylinder and blades look together. Show the blades and Unite them to the cylinder.

Step 25:

Zoom to the areas shown to visually analyze the connection of the blades.

Based on the steps performed, you will notice problem areas.

These bad areas are caused because of how we drafted the cylinder. Not only is the draft causing a problem, but the bottom side of the cylinder is not drafted at all. 

Step 26:

When using To Parting Edges draft type, draft is created up to the parting line as we desire, but knife edges are created. This is because a 90 degree angle is created at the intersection of the base face and parting edge.

If the blades were 90 degrees and flat, we would be fine, but obviously this is not the case. 

Step 27:

The logical step to attempt next would be to Unite the blades first, then apply draft to the cylinder. After attempting you may realize this does not work since the blades themselves will also draft. In this case the geometry is too complex and therefore an error is given. Even if the draft worked, the blades would alter, and this is not the intent of our design. Plus we still need the bottom side to also have draft. To accomplish our task, a manual approach is necessary. Start by deleting or undoing the last Unite, Draft, Divide Face, and the Instance Geometry commands.

Step 28:

Next, a cleaner more accurate draft will be created. This will be done by creating a parting surface first, and then trimming commands to trim the solid. First Show the Projected Curve feature created earlier.

Step 29:

Select Home tab > Surface group > Swept to create a Swept feature using the projected curve as a Section Curve and the two edges of the blades as Guides. Be sure to use the Parameter alignment method and activate Preserve Shape.

Make sure the Curve Rule drop-down in the Top Border Bar is set to Single Curve.

Step 30:

Select Home tab > Feature group > Associative Copy > Extract Geometry to extract four faces from the first original blade. Set the Type drop-down to Face and activate Fix at Current Timestamp.

Make sure the Face Rule drop-down in the Top Border Bar is set to Single Face.

Step 31:

Hide the blade solids and change the color of the extracted faces to the same color as the Swept feature.

Step 32:

Perform another Pattern Geometry operation to pattern all sheet bodies to form a complete circular chain of surfaces. Select Home tab > Feature group > More > Combine gallery > Sew to sew all surfaces together when complete.

Step 33:

To be more organized and to reduce the part history count. Group the features that make up the parting surface by creating a Feature Group.

Be sure to Embed Feature Group Members and name the group Parting Surface.

Group from the Swept feature to the last feature. Ignore example feature numbers. These number will vary based on mistakes, deleting, undo's, etc.

Step 34:

Extract the cylindrical face of the cylinder.

 All extracts should always have Fix at Current Timestamp active.

Step 35:

Hide the cylinder. Draft the extracted surface 2 degrees using the From Plane draft type. The Draw Direction should be in the positive Z direction. Use the top arc center as the Stationary Plane.

Step 36:

Select Home tab > Feature group > More > Trim gallery > Trim and Extend to trim away the overlapping surfaces using the Make Corner type. Keep the outside portion of the parting surface and the top portion of the cylindrical surface. Choose the Parting Surface as the Target.

Step 37:

The last command automatically combined the surfaces together. Change the color of this surface to green.

Step 38:

Another surface representing the bottom half needs to be created. A copy of Parting Surface must be created. Start by making the feature group named 'Parting Surface' the Current Feature.

Extract the entire sheet body using the Body method.

Make the last feature Current and Hide the Parting Surface.

Step 39:

Perform the same steps as before. Show the cylinder solid. Extract the cylindrical face, Draft the face 2 degrees in the negative Z direction using the bottom arc center as the Stationary Plane, and Trim and Extend keeping the outside and bottom half.

Change the color of the surface to yellow.

Step 40:

Use Show and Hide to only show the Cylinder and Yellow/Green surfaces.

Step 41:

Using Trim Body is the ultimate command we will use to create the draft on the cylinder. Before this can be done though, the cylinder needs to have enough material to shave off. Create an Offset Face of 5 on the outside face to make the diameter larger.

Step 42:

Perform two Trim Body operations to trim away the solid using the surfaces created.

Hide the surfaces.

Step 43:

Show and Unite the blade solids to the cylinder.

Step 44:

Examine the previous problem areas.

No geometrical problems at the connections of the blade solids should exist.

Even though more work was required, a more accurate result was achieved. 

Step 45:

 Extrude an embedded sketch comprising of a circle with a diameter of 34.5 centered on the bottom of the cylinder base in to the solid. Use an end Distance of 19.25 and a draft Angle of 1 from the start limit. Subtract the tool then add a blend to the bottom edge of the pocket with a radius of 1.25.

Step 46:

 Blend the top edge of the cylinder using a radius of 3.5.