Repairing the Exhaust Tip

One of the exhaust tips is a sheet body with internal parts. Some of the surfaces are missing from this part which prevents 3D-CAD from using it as a solid body. In order to use this body in meshing, you must reconstruct the internal parts before converting it to a solid body.

To convert the exhaust tip to a solid body:
  1. First isolate the part for repair:
    1. Under the Body Groups node, multi-select the Exhaust Tip 1, Exhaust Tip 1 2, Exhaust Tip 1 3, and Exhaust Tip 1 4 nodes.
    2. Right-click one of the selected body nodes and select Show Only.


Before reconstructing the interior, you create a sketch plane onto which you project one of the perforation holes. You can then use the projected sketch to recreate the perforation holes once the interior of the exhaust tip is fixed.
  1. To create a sketch plane for the sketch of the perforation hole:
    1. In the graphics window, rotate the part and select the edge that connects the exhaust tip to the tail pipe as shown in the image below.


    2. Right-click the edge and select Reference Geometry > Plane from Curve.
    3. In the Plane from Curve panel, click OK to create the plane.
      A sketch plane feature, Plane 2, is added to the Features node.
    4. In the 3D-CAD View scene, right-click the plane and select Reference Geometry > Plane by Transformation.
    5. In the Plane By Transformation panel, set Translation Vector to [0.0, 0.0, -0.01]m and click OK.
    6. In the toolbar at the top of the 3D-CAD View scene, click Display Cut Parts using Multiple Planes.


    7. In the Dynamic Sectioning panel, within Section 1, first select (ZX Plane), which activates a slice through the middle of the exhaust tip.
    8. In the graphics window, orient the exhaust tip so that reference Plane 3 is closer to you than the middle plane.
    9. In the Dynamic Sectioning dialog, now select (Reference Plane) and then, in the graphics window, select Plane 3. Confirm that you have selected the correct slicing plane by moving the exhaust tip around in the graphics window.
    10. Click Close.
    11. In the Vis toolbar, click (Save-Restore-Select Views) and select Views > -Y > Up +Z.
    12. In the feature tree, right-click the Plane 3 node and select Create Sketch.
    13. In the graphics window, zoom in closely and right-click the edge of the hole as shown in the image below and select Project to sketch.


    14. In the Sketch panel, click OK.
    15. Under the Features node, multi-select Plane 2 and Plane 3, right-click and select Hide.
The projected perforation hole is used in a later step for recreating all of the channel holes. Before then, you use the Search Tool to find the existing channel holes in order to delete them.
  1. To create a design filter that finds all the channel faces:
    1. To open the Search Tool panel, on the right side of the 3D-CAD View scene, click (Show Filter).
    2. In the Design Filter 1: Input panel, set Selection Mode to (Selected Entities).
    3. For Object Type, select Bodies .
    4. To the right of the Object Type Selection box, click the (Object Selector) and select Exhaust Tip 1. Close the object selector by clicking the same button as you did when opening it.
    5. For Input Type, select Faces .
    6. Under the Search Criteria tab, select the Find Similar option.
    7. In the 3D-CAD View scene, rotate the part and zoom in closely to select a channel face, as shown in the example below.


    8. Once you have selected the face, click Search to locate all the similar faces in the body.
      All the channel faces are identified and selected in the geometry. In total 84 faces are found by the Search Tool.

    9. At the bottom of the Filter panel, click OK.
      This action creates Design Filter 1 under the Design Filters node in the simulation tree.
    10. Rename the Design Filter 1 node to Channel Faces.
  2. Use the results from the Search Tool as inputs to the Delete Faces operation:
    1. Under the Design Filters node, right click the Channel Faces node and select Delete.
    2. In the Delete Faces panel, click OK.
  3. Use the Fill Holes operation to fill the perforation holes:
    1. Under the Body Groups node, right-click the Exhaust Tip 1 node and select Repair Tools > Fill Holes.
      The operation preview shows that two edges at the entrance to the exhaust tip are included which are not among the small channel holes. These edges must be excluded from the fill holes operation.
    2. In the Fill Holes panel, click within the Exclude Holes box and then, in the graphics window, multi-select the two edges as shown below.


    3. In the Fill Holes panel, click OK to fill the holes.
Due to missing faces, the inner cavity within the Resonator cannot be formed correctly. To overcome this problem, you first move redundant surfaces and then recreate the faces that surround the inner cavity.
  1. Use the Imprint tool to split the faces where the Exhaust Tip 1 and Exhaust Tip 1 2 bodies intersect:
    1. Within the Body Groups node, multi-select the Exhaust Tip 1 and Exhaust Tip 1 2 nodes, right-click and select Boolean > Imprint.
    2. In the Imprint Bodies panel, click OK.
  2. Use the Delete Faces operation to remove unwanted faces inside the exhaust tip:
    1. In the toolbar at the top of the 3D-CAD View scene, change Color Mode to (Distinguish Bodies).
    2. In the 3D-CAD View scene, multi-select the faces as shown in the images below.


    3. Right-click on the faces and select Delete Faces.
    4. In the Delete Faces panel, click OK.
  3. To help in selecting the right portion of the inner surface:
    1. Multi-select the inner face at the entrance to the tip and the leading edge of the floating inner surface as shown below.


    2. Right-click the edge or face and choose Repair Tools > Split Faces By Edge Projection.
    3. In the Split Faces dialog, set Max Project Distance to 5.0 mm.


    4. Click OK.
  4. Select the inner surface and create a shell body as follows:
    1. Double-click one of the inner faces of the exhaust tip. This action selects all the faces.
    2. While pressing <CTRL>, click the first inner (selected) face at the entrance to the tip; this action deselects this first face.


    3. Right-click one of the remaining selected faces and select Create Sheet Bodies. In the Create Sheet Bodies panel, click OK.
      Exhaust Tip 1 3 is added within Body Groups.
    4. Right-click Body Groups > Exhaust Tip 1 3 and select Thicken.
    5. In the Thicken panel, set Direction to Backward, enter 0.0012m for Thickness and click OK.
  5. Only the upper surface of the thickened body is required. To delete the other surfaces:
    1. Multi-select the thin faces at each end of the thin body as shown below.


    2. Right-click one of the faces and select Delete Faces.
    3. In the Delete Faces panel, click OK.
      As the single body is now divided, an additional sheet body, Exhaust Tip 1 5 appears. This body is the one that you want to keep.
    4. Right-click Body Groups > Exhaust Tip 1 3 and select Delete. In the Delete Bodies panel, click OK.
  6. To provide a consistent set of edges for a bridging surface near the outlet of the tip, create a plane and use it in a boolean slice:
    1. Select the face as shown in the image below.


    2. Right-click on the face and select Reference Geometry > Plane by Transformation.
    3. In the Plane By Transformation panel, enter -0.008925 for the Z component of the Translation Vector and click OK.
    4. Expand the Body Groups node, multi-select Exhaust Tip 1 4 and Exhaust Tip 1 5 nodes, right-click and select Boolean > Slice.
    5. In the Slice Panel, set the following parameters:
      Parameter Setting
      Keep Side Back Side
      Sketch Planes Plane 4
    6. Click OK.
  7. Create bridging surfaces at the start and end of the inner volume that you are forming:
    1. Rotate the exhaust tip and multi-select the free edges above the projected edge that was created from the Split Faces By Edge Projection tool.


    2. Right-click on the edges and select Bridge Surface.
    3. In the Bridge Surface panel, activate Sew Bodies and click OK.
    4. For the bridging surface near the end of the tip, multi-select the free edges as shown in the image below.


    5. Right-click on the selected edges and select Bridge Surface.
    6. In the Bridge Surface panel, activate Sew Bodies and click OK.
    7. Under the Features node, right-click on the Plane 4 node and select Hide.
    8. In the toolbar at the top of the 3D-CAD View scene, select the (Toggle Section View) icon to deactivate the dynamic sectioning scene.
    Exhaust Tip 1 4 is now a solid body that represents the inner volume of the exhaust tip.
  8. Under the Body Groups node, multi-select Exhaust Tip 1 and Exhaust Tip 1 2, right-click on the nodes and select Sew.
  9. In the Sew Sheet Bodies panel, click OK.
  10. Multi-select Exhaust Tip 1 and Exhaust Tip 1 4, right-click and select Boolean > Subtract.
  11. In the Subtract Bodies panel, click OK.
  12. Reconstruct the perforation holes:
    1. Rotate the part and select the face inside the exhaust tip as shown below.


    2. Right-click the selected face and select Reference Geometry > Axis from Resolved Entity.
    3. In the Axis From Resolved Entity panel, click OK.
    4. In the graphics window, right-click the axis and select Hide.
    5. In the features tree, right-click the Sketch 1 node and select Extrude.
    6. In the Extrude panel, set the following properties:
      Parameter Setting
      Direction Type Reverse
      Distance 0.02973 m
      Body Interaction None
    7. Click OK.
    8. Under Body Groups, rename the new body to Perforation Body
    9. Right-click the Perforation Body node and select Pattern > Linear Pattern.
    10. In the Body Linear Pattern panel, set the following properties:
      Parameter Setting
      Direction (1) - Distance 0.012m
      Direction (1) - Number of Instances 5
      Body Interaction None
      Create Body Group Activate
    11. Click OK.
    12. Under Body Groups, rename Body Group 1 node to Perforation Holes.
    13. Right-click the Perforation Holes node and select Pattern > Circular Pattern Cut.
    14. In the Body Circular Pattern Cut panel, set the following properties:
      Parameter Setting
      Axis Type Set to Reference Axis and select Axis 1
      Number of Instances 20
    15. Click OK.
  13. Multi-select all the feature nodes from Plane 2 to Circular Pattern Cut 1, right-click on the selected features and select Group.
  14. Rename the feature group to Repairing the Exhaust Tip.
  15. Save the simulation.