Creating the Backward Facing Step Geometry

You define the geometry for the backward facing step in relation to a set parameter for the step height. This approach allows for easy scaling of the model later.

To create the backward facing step geometry:
  1. Create a new simulation:
    1. Start up Simcenter STAR-CCM+ in a manner that is appropriate to your working environment and create a new simulation.
    2. Save the new simulation with the file name backwardFacingStep.sim
  2. Create a parameter for the step height to use when creating the geometry:
    1. Right-click the Automation > Parameters node and select New > Scalar.
    2. Rename the new parameter to StepHeight.
    3. Select the StepHeight node and set the following properties:
      Property Setting
      Value 1.0
      Dimensions > Length 1
  3. Create a 3D-CAD model:
    1. Right-click the Geometry > 3D-CAD Models node and select New.
    2. Select the 3D-CAD Model 1 node and rename it to Fluid Domain.
  4. Create the geometry of the backward facing step:
    1. Right-click the Fluid Domain > Features > XY node and select Create Sketch.
    2. In Display Options, click (Set Sketch Grid Spacing) and change Grid Spacing to 0.25 m.
    3. In Display Options, click (View Normal to Sketch Plane) to bring the sketch plane into view.
    4. In Create Sketch Entities, click (Create Line) to draw a line of length 1.0 m, starting at the origin (position [0, 0]) and extending in the positive y direction. After placing the end point, click [esc] to end the line.


  5. Apply constraints to the line:
    1. Right-click the vertex that lies on the origin and select Apply Fixation Constraint.
      This prevents the selected vertex on the line from moving.
    2. Right-click the line and select Apply Length Dimension, and in the Dimensions dialog, enter $StepHeight.
    3. Click OK.
  6. Draw the other lines in relation to the step height:
    1. Draw a line starting from the top of the step height and extending approximately 4.0 m in the negative x direction.
    2. Right-click the line and select Apply Length Dimension, and in the Dimensions dialog, enter 3.8*$StepHeight, then click OK.
    3. Using the same techniques, continue by creating the other lines, each in relation to the parameter $StepHeight, which corresponds to the step height H in the diagram below:


    4. Click OK in the Sketch: Sketch 1 dialog to complete the sketch.
  7. Extrude the sketch profile to obtain a solid body:
    1. Right-click the Fluid Domain > Features > Sketch 1 node and select Extrude.
    2. In the Extrude dialog, set Distance to 0.5 m and click OK to perform the extrusion.
      A new body, Body 1, is added below the Body Groups node.
    3. Select the Body Groups > Body 1 node and rename it to Backward Facing Step.
  8. Rename the geometry faces:
    1. Click in the toolbar and select Views > -X +Y +Z > Up +Y.
    2. Right-click the face shown below and select Rename. Rename the face to Inlet and click OK.


    3. Rename the other faces in the geometry to match those shown below:


    4. Click in the toolbar and select Views > -X +Y -Z > Up +Y.
    5. Rename the surface that lies on the Z = 0 plane to Surface for 2D Mesh, as shown below:


      This surface is used at a later stage to generate a 2D mesh.
  9. Create the shape to use as a volumetric refinement area:
    1. Right-click the Surface for 2D Mesh surface and select Create Sketch > On Face.
    2. In Sketch Mode, click the <T> key to change to the side view.
    3. Click (Create Rectangle) and draw a rough box around the bottom half of the geometry so that it covers the step, as shown below:


  10. Constrain the sketch so that the left, right and bottom edges are collinear with the corresponding edges of the backward facing step geometry:
    1. Select the bottom edge of the rectangle and the bottom edge of the solid part, then right-click the selection and select Apply Collinear Constraint.


    2. Repeat this for the left and right edges.
  11. Add a dimension for the height of the box, so that its height is twice the step height:
    1. Right-click the left edge of the sketch and select Apply Length Dimension.
    2. In the Dimension dialog, enter 2 * $StepHeight and click OK.


  12. Click OK to exit Sketch Mode.
  13. Create a solid body from the sketch:
    1. Right-click the Sketch 2 node and select Extrude.
    2. In the Extrude panel, set Method to Up to Face.
    3. Select the surface opposite the sketch plane.
      A preview of the box appears, and the Target Face property in the panel shows the name of the surface.

    4. In the Extrude panel, set the following properties:
      Property Setting
      Direction Type Reverse
      Body Interaction None
    5. Click OK.
      A new body is created. The body is associated with the shape of the backward facing step geometry. If the backward facing step domain changes, the box changes with it.
    6. Rename the Body Groups > Body 2 node to Refinement Box.
    7. Click Close 3D-CAD.
  14. Create a new geometry part using the 3D-CAD model:
    1. Right-click the Geometry > 3D-CAD Models > Fluid Domain node and select New Geometry Part.
    2. In the Parts Creation Options dialog, the default settings are acceptable so click OK to close the dialog.
    3. Expand the Parts > Backward Facing Step > Surfaces node to see the boundary faces specified in 3D-CAD as separate faces.
  15. Save the simulation.
The backwards facing step geometry is now complete.