Geometry Parts: Creating the Main Fluid Volume and Subtracting the Enclosure and Fan

Although you can create the main fluid volume using 3D-CAD, Simcenter STAR-CCM+ provides additional tools at the geometry parts level with which you can achieve the same goal. Using the part-level tools helps you differentiate between detailed and bulk geometry creation.

Here, you first create parts from the 3D-CAD model before creating a part shape that defines the outer fluid volume:

  1. Launch Simcenter STAR-CCM+ and load foundationTutorial_6.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_7.sim.
  3. Create geometry parts from the 3D-CAD model:
    1. Expand the Geometry > 3D-CAD Models node.
      The 3D-CAD model of your geometry is stored here.
    2. Right-click 3D-CAD Model 1 and select New Geometry Part.
    3. In the Part Creation Options dialog, click OK to accept the default settings.
    The solid bodies from the 3D-CAD model are added as geometry parts.
  4. Right-click the Scenes node and select New > 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.
  5. Create a part shape for the surrounding 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 [-0.250, -0.025, -0.200] m
      Corner 2 [0.150, 0.150, 0.200] m


    3. Click Create followed by Close.
      A shape part, Block, is created and added to the Parts node.
  6. Split the surfaces of the block in preparation for the extruder mesher that you will set up in a later tutorial:
    1. Right-click the Block > Surfaces > Block Surface node and select Split by Patch.
    2. In Geometry Scene 1, select the face that is upstream of the flow.


      To help you identify the correct face to select, pay attention to the orientation of the direction axes in the scene. Select the face that lies on the plane with the largest X value.
    3. In the Part Surface Name field, enter Upstream and click Create.
      The selected patch is removed from the scene.
    4. In the same scene, select the surface that is downstream of the flow.


      To help you identify the correct face to select, pay attention to the orientation of the direction axes in the scene. Select the face that lies on the plane with the smallest X value.
    5. In the Part Surface Name field, enter Downstream and click Create.
    6. Click Close.
    The selected patches are split and added to the Geometry > Parts > Block > Surfaces node.
  7. Subtract the graphics card and disc from the static region:
    1. Right-click the Geometry > Operations node and select New > Boolean > Subtract.
    2. In the Create Subtract Operation dialog, set the following parameters:
      Parameter Setting
      Input Parts Block
      Disc
      Enclosure
      Target Part Block
      Perform CAD Boolean Activated
    3. Click OK.
      A subtract operation is added to the Operations node. A subtract placeholder for the operation is also added to the Parts node.
    4. Rename the Parts > Subtract node to Static Region.
    5. Rename the Operations > Subtract node to Subtract Block.
    6. Right-click the Operations > Subtract Block node and select Execute.
  8. Modify the geometry scene to display only the parts that correspond to the simulation domain:
    1. Click Scene/Plot above the simulation object tree.
      The object tree displays only the properties of the active scene, Geometry Scene 1.
    2. Select the Geometry Scene 1 > Surface 1 > Parts node.
    3. In the Properties window, click (Custom Editor) next to Parts.
    4. In the Parts dialog, right-click on a blank area of the dialog and select Deselect All to clear the selection.
    5. In the same dialog, select the Rotating Region and Static Region and click OK.
    6. Click (Make Scene Transparent) to get a better view of the static region.


  9. To create a part contact between the static region and the rotating region, imprint these two parts together:
    Part contacts define the connection between two part surfaces. The meshers aim to generate a conformal mesh at the contact, which then becomes an interface in the physics region.
    1. Click Simulation above the simulation object tree.
    2. Right-click Geometry > Operations and select New > Boolean > Imprint
    3. In the Create Imprint Operation dialog, select Rotating Region and Static Region.
    4. Activate the Perform CAD Imprint option.
    5. Click OK.
      An imprint operation is added to the Operations node.
    6. Right-click the Operations > Imprint node and select Execute.
    The two parts are imprinted together and a part contact is created between the two parts.
  10. Save the simulation.