Basic 3D-CAD: Creating the Enclosure Solid Shell

In cases where you create the wetted volume first, Simcenter STAR-CCM+ allows you to surround the volume with a solid shell of specified thickness. This additional solid is then available for simulations that model phenomena in both solid and fluid materials.

Create the solid body for the graphics card enclosure and thereafter expose the fan within the enclosure.

  1. Launch Simcenter STAR-CCM+ and load foundationTutorial_4.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_5.sim.
  3. Resume the 3D-CAD model.
  4. Extrude the enclosure sketch to form a solid body:
    1. Right-click Enclosure Sketch and select Extrude.
    2. In the Extrude panel, set Direction Type to Reverse.
      This option reverses the direction of the extrusion so that the solid encloses the fan.
    3. Set Method to Up To Face and select the top face on the graphics card fan hub.


    4. To keep the fan separate from the surrounding body, set Body Interaction to None.
    5. Click OK.


    6. Rename Features > Extrude 1 to Enclosure Extrusion.
  5. Add a fillet to the top edge of the enclosure:
    1. In the 3D-CAD View, multi-select the side and circular edges around the top of the enclosure.
    2. Right-click the selection and choose 4 Edges > Create Fillet.
    3. In the Fillet panel, set Radius to 3 mm.
    4. Click OK.


    5. Rename Features > Fillet 1 to Enclosure Fillet.
  6. Shell the enclosure:
    1. In the 3D-CAD View, right-click the enclosure body and select Body Features > Shell.
    2. In the Shell panel, set Thickness to 2 mm.
    3. Click inside the Faces to Remove group box to activate face selection.
    4. In the 3D-CAD View scene, select the face that corresponds to the exhaust of the enclosure.


      This face is removed from the shelling operation so that the enclosure has an opening.
    5. Click OK.


    6. Rename Features > Shell 1 to Enclosure Shell.
  7. Draw a sketch for the fan opening:
    1. Right-click the top surface of the enclosure and select Face > Create Sketch > On Face.
    2. Draw a circle about the fan axis that has a radius of 35 mm.
      Activate scene transparency so that you can see the fan.


    3. Click OK.
    4. Rename Features > Sketch 1 to Fan Opening Outline.
  8. Cut out the opening for the fan:
    1. Right-click Fan Opening Outline and select Extrude Cut.
    2. In the Extrude Cut panel, set Method to Through Body First Segment.
      As the enclosure is a shell, this option cuts through the top layer of the shell, but not through the bottom layer.
    3. Click the Through Body field and select the enclosure body in the 3D-CAD View scene.
    4. Set Bodies to Cut to Selected.
      By default the operation cuts all bodies in its path. Here, you only want to cut the enclosure, not the fan.
    5. Click the Cut Bodies group box, and select the enclosure body in the 3D-CAD View scene.
    6. Click OK.
    7. Rename Features > Extrude Cut 1 to Fan Opening.
  9. Expand the Body Groups node and rename the new body to Enclosure.
  10. Save the simulation.
The completed enclosure is displayed below.