HV-3095: Generate CFD Plots/Streamlines

Learn how to generate cross sections for contour plotting of flow variables (for example, velocity or pressure) and generate streamlines starting from a surface or line.

This exercise uses the ensightb.case results file located in the animation folder.
To access the Streamlines panel:
  • Click the Streamlines panel button on the Result toolbar.


  • Select Results > Plot > Streamlines from the menu bar.

Figure 1.

The Streamlines panel allows you to generate streamlines using any available nodal vector field (typically a velocity field). Velocity fields are directly written to H3D files by many solvers such as: Radioss, HyperXtrude, Moldflow, etc. Velocity fields and other scalar and vector data fields are also saved in EnSight format by most CFD solvers.

Create Multiple Section Cuts and Contour the Model

  1. Load the ensightb.case file, located in the animation folder, as both the model and results files.
    Figure 2.
  2. Right-click within the Results Browser and select Create > Section Cut > Planar. Then right-click on Section 1 and select Edit.
    A section cut is automatically applied to the model, and the Section Cut panel is displayed.
  3. Verify that Define plane is set to Y Axis.
  4. Under Display Options, turn on the Cross section option and verify that the Width is set to the lowest value.
    Figure 3.
    Note: You can use the Define plane slider bar (located under the Y Axis button) to move the position of the section cut.
  5. Click the Contour panel button on the Result toolbar.
  6. Select UVW(v) as the Result type and click Apply.
    Figure 4.
  7. Within the Results Browser, expand the Section Cuts folder, right-click on Section 1, and select Edit.
    You are returned to the Section Cut panel.
  8. Click the Add button.
  9. Select Z Axis for the plane and click Apply.
    Figure 5.
  10. Deactivate the section cuts by removing the check marks from their respective check boxes.
    Note: If the section cuts are not deactivated, the streamlines will also be cut and you would only be able to see the points where the streamlines hit the cross section.
  11. Return to the Contour panel .
  12. Click the Clear Contour button.
    Note: If the contours are not cleared, all of the streamlines would appear gray and they would not be colored according to the contour variable.

Create a 'Line' Streamline

  1. Using the Results Browser, turn off the display of the following components: BC3_wall (ID 7), cells of cell type 1 (ID 1), and cells of cell type 2 (ID 2), so that the inside of the flow domain is displayed in the graphics area.
    Figure 6.
  2. Click the Streamlines panel button from the Result toolbar to enter the Streamlines panel.
  3. Click Add, to add a new set of streamlines.
  4. Select Line as the Rake type.
  5. Specify N1 and N2 by picking two nodes on the BC1_inlet (ID 4) component on the model.
  6. Select Downstream from the Integration mode drop-down menu.
  7. Enter 10 into the Number of seeds text box.
  8. Click the Create Streamlines button (located within the Streamlines tab on the right side of the panel).
    Figure 7.
  9. From the Streamlines tab, activate the Draw as tube option.
  10. Select Streamline from the Size drop-down menu and change the value in the text box from 1 to 7.
  11. Click the Create Streamlines button.
    Figure 8.

Create an 'Area' Streamline

  1. Add another streamline.
  2. Select Area as the Rake type.
  3. Select the BC1_inlet (ID 4) component on the model.
  4. Select Downstream for the Integration mode.
  5. Specify the Number of seeds as 40.
  6. Click Create Streamlines.
    Figure 9.
  7. Click the Contour panel button on the Result toolbar.
  8. Select UVW(v) as the Result type and click Apply.
  9. Rotate the model and view the streamlines with the contour applied.
    Figure 10.