Creating Attached Shell Parts

To create shell parts form the exhaust pipe parts, you can use the Attached Shells Creator operation.

A shell part has two part surfaces—a front surface and a back surface. You can apply boundary conditions on the part surfaces respectively.

  1. Right-click the Geometry > 3D-CAD Models > Exhaust Pipe node and select New Geometry Part.
  2. In the Parts Creation Options dialog, click OK.
Some of the exhaust surfaces are used for flow boundary conditions in the final simulation. These surfaces must be converted to regular parts (rather than shell parts).
  1. To separate the inlets and outlets into individual regular (solid) parts:
    1. Expand the Geometry > Parts > Body 1 > Surfaces node and select Inlet 1.
    2. Right-click on the selection and select Create New Part From Surfaces.
      A new part is created and added to the Parts node.
    3. Rename the newly created Part to Inlet 1.
    4. In the same way, convert the remaining inlet and outlets to solid parts. The table below specifies the location of each inlet and outlet.
      Location Inlet and Outlet Surfaces
      Body 4 Outlet 1
      Outlet 2
      Body 8 Inlet 2
      Body 12 Outlet 3
      Outlet 4
    The solid bodies are listed in the Geometry > Parts node, as shown below.

To create the attached shell parts:
  1. Right-click the Geometry > Operations node and select New > Surface Preparation > Attached Shells Creator.
  2. In the Create Attached Shells Creator Operation window set the following properties and click OK:
    Property Setting
    Input Parts All [Body] parts
    Part Surfaces All Surfaces
    Execute Operation Upon Creation Activated
  3. Right-click the Scenes node and select New Scenes > Geometry.
    A new geometry scene, Geometry Scene 1, is added to the Scenes node. This scene automatically displays all parts that are listed under the Geometry > Parts node.
  4. Create a part shape for the fluid volume:
    1. Right-click the Geometry > Parts node and select New Shape Part > Block.
    2. In the Create Block Part panel, set the following parameters:
      Parameter Setting
      Corner 1 [-2, -1, -1] m
      Corner 2 [4, 1, 1] m
    3. Click Create followed by Close.
      A shape part, Block, is created and added to the Parts node.
    4. Rename the Geometry > Parts > Block node to Fluid Volume.
  5. Split the Fluid Volume surfaces so that boundaries can be identified:
    1. Right-click the Geometry > Parts > Fluid Volume > Surfaces > Block Surface node and select Split by Angle.
    2. In the Split Part Surfaces by Angle dialog, click OK.
    3. Rename Block Surface 3 to Inlet and Block Surface 6 to Outlet.


  6. Save the simulation.