Basic 3D-CAD: Adding Blades as a Pattern of Bodies

3D-CAD allows you to create a set of identical bodies in an ordered pattern. Here, you create a single fan blade and apply it in a pattern around the central axis.

To create the fan blade, first place a sketch on the large flat surface of the fan hub:

  1. Launch Simcenter STAR-CCM+ and load foundationTutorial_2.sim.

    You can either use the sim file that you saved from the previous tutorial, or load the sim file provided in the tutorials bundle. See Downloading the Tutorial Files from the Support Center Portal.

  2. Save the simulation as foundationTutorial_3.sim.
  3. Resume the 3D-CAD model.
  4. Sketch the outline of a single fan blade:
    1. Right-click the face shown below and select Create Sketch > On Face.


    2. In the toolbar at the top of the 3D-CAD View scene, click Model Visibility and activate the All Edges option.

      The edges on the geometry are displayed.
    3. In the Sketch panel, click (View Normal to Sketch Plane).
    4. Click (Create Line) and draw a horizontal line from the outer edge of the hub center that extends beyond the flat surface of the hub, and then press <Esc>.


    5. Multi-select the starting point of the created line and the outer circle of the hub center.
      Press and hold <CTRL> after the initial click to select additional entities.
    6. Right-click the selected corner and choose Apply Coincidence Constraint.


      When applying constraints, 3D-CAD allows you to reference entities from other bodies, such as the edges of the hub. 3D-CAD automatically projects these entities to the active sketch and applies the constraints.
    7. Multi-select the same outer circle on the hub and the sketch line.
    8. Right-click one of the edges and choose Apply Tangent Constraint.
    9. Right-click the line entity and apply a length dimension of 44 mm.


    10. Click OK.
    11. In the toolbar at the top of the 3D-CAD View scene, click Model Visibility and deactivate the All Edges option.
    12. Rename Features > Sketch 1 to Fan Blade Outline.
  5. Extrude the sketch to form the solid fan blade:
    1. Right-click Fan Blade Outline and select Extrude.
    2. In the Extrude panel, set Distance to 19 mm and click OK.


      The brown color of the blade body means it is a sheet body. Sheet bodies have zero thickness.

    3. Rename Features > Extrude 1 to Fan Blade.
  6. Thicken the blade body:
    1. In the 3D-CAD View scene, right-click the blade body and select Body Features > Thicken Sheet Bodies.
      If you cannot see the Thicken command due to the height of the right-click menu, in the Selection toolbar, click (Selection Filter) and deactivate the Faces option while keeping the Bodies option active. Then try accessing the Thicken command again.
    2. In the Thicken panel, set Direction to Backward, set Thickness to 1 mm and click OK.
    3. In the toolbar at the top of the 3D-CAD View scene, click Model Visibility and activate the All Edges option.


      The sheet body is converted to a solid body.

    4. Rename Features > ThickenSheetBodies 1 to Fan Blade Thicken.
  7. Slice the blade to remove the part of the fan blade that extends beyond the fan hub:
    1. Expand the Body Groups node, right-click Body 2 and select Boolean > Slice.
    2. In the Slice panel, set Keep Side to Back Side.
    3. Click inside the Cutting Tools group box to activate the selection mode for this property.
    4. In the 3D-CAD View scene, select the face on the side of the fan hub as shown below.


    5. Activate the Extend Cutting Tool to Intersect Target option to extend the selected face through the protruding fan blade.
    6. Click OK to slice the protrusion.
    7. Rename the Features > SliceBodies 1 to Fan Blade Slice.
Create the remaining fan blades around the fan hub using a pattern. You can pattern the existing fan blade about the axis of revolution.
  1. Create a reference axis:
    1. Right-click the neck of the fan hub and select Face > Reference Geometry > Axis From Revolved Entity.
      If within the (Selection Filter) you deactivated the Faces option, you must reactivate the option now. Then try accessing the Axis From Revolved Entity command again.


    2. In the Axis From Revolved Entity panel, click OK.
      An axis feature, Axis 1, is added to the Features node.
    3. Rename Features > Axis 1 to Axis of Revolution.
  2. Create a pattern about the axis of revolution:
    1. Right-click the Body Groups > Body 2 node and select Pattern > Circular Pattern.
    2. In the Body Circular Pattern panel, set Axis Type to Reference Axis.
    3. Click inside the Reference Axis field box to activate the selection for this feature, and then select the reference axis from the 3D-CAD View scene.
    4. Set Number of Instances to 30.
      This option controls the total number of fan blades in the pattern.
    5. Click (Expose Design Parameter) next to Number of Instances.
    6. In the Design Parameter dialog:
      1. Activate the Expose Parameter option.
      2. Set Name to Number of Fan Blades.
      3. Click OK.
      This option exposes the parameter that controls the number of fan blades in the pattern so that you can access it outside of 3D-CAD at the parts level.
    7. Click OK to create the pattern.
      A pattern feature, Circular Pattern 1, is added to the feature tree.

    8. Rename Features > Circular Pattern 1 to Fan Blade Pattern.
  3. Cut away a portion of the fan blades near the center of the hub to allow more air to flow into the fan as it spins:
    1. Right-click on the top face of the fan hub and select Create Sketch > On Face.


    2. In the sketch, right-click the outer edge on the hub center and select Project to sketch.
      Use the (Make Scene Transparent) tool to make it easier to visualize the sketch. Remember to deactivate this tool when done.


      The edge from the fan hub body is projected to the active sketch. Projected edges are displayed in orange in Sketch mode. Projected entities are linked to the underlying edge on the parent body, so that if the parent body changes, the projected edge changes as well.
    3. Right-click the projected edge and select Offset Sketch Primitive.
    4. In the Offset Sketch panel, set Offset Distance to 14 mm and click OK.
      Make sure Offset Options is set to Outward.
      A copy of the selected edge is offset by the specified amount.

    5. Click OK to exit sketch mode.
    6. Rename Features > Sketch 1 to Fan Blade Cut Outline.
    7. Right-click Fan Blade Cut Outline and select Extrude Cut.
    8. In the Extrude Cut panel, set Method to Up To Face.
    9. In the 3D-CAD View scene, select the face shown below.


    10. Click OK.
      The portion of the fan blades near the hub center are cut.
    11. Rename Features > Extrude Cut 1 to Fan Blade Cut.
  4. Expand the Body Groups node and rename Body 2 (2) to Fan.
  5. Save the simulation.
The finished fan is displayed below: