Exercise: Meshing in Simulation CFD for AEC projects

The impact of meshing on results fidelity will be demonstrated by first running an office space with a default mesh and then running the same space again with a more refined mesh.

Learning Objectives

  • Provide experience working with multiple mesh refinement techniques.
  • Observe how mesh quality can directly affect the results.

Assumptions

The simulation will have several simplifying assumptions to reduce overall complexity and expedite completion of this tutorial.

  • Flow only analysis to observe impact of mesh refinement on flow velocity results.

NOTE:  The tutorial will begin from a support share file where all setup tasks, except meshing, have already been defined to keep the focus of this tutorial on meshing. 

Simulation Parameters

Total flow rate:158 cfm (~4 air exchanges per hour)

Simulation Process

1. Download the Exercise 4.cfz share file to a local hard drive folder.

2. Load support share file

a. Start the Simulation CFD interface and click Open in the upper left ribbon, then navigate to and open the Exercise 4.cfz share file.

3. Define a default mesh

a. Select the Mesh Sizing icon from the Setup Task section of the Ribbon menu.

b. Click the Autosize button in the ribbon.

A clone of this scenario will now be created and run in order to make a side by side comparison of the effects of mesh adjustments to the model.  These iterative mesh refinements are in accordance with the mesh convergence process and strategic refinement practices discussed previously in this module.

4. Clone Scenario

a. Right Click on the DefaultMesh scenario node  in the Design Study Bar and select Clone.

b. Type in RefinedMesh for the new scenario name.

5. Refine the mesh on the outlet, using mesh size adjustment, to improve the ability to accurately capture the outlet flow profiles.

a. Click on the small air volume representing the outlet extension and click on Edit in the ribbon. 

b. Move the Size Adjustment slider to the left to approximately 0.25 ( this will specify roughly 6 elements across the width of the outlet, a much improved mesh to capture the flow profile than the original 2 elements).

c. Click the Apply button.


The default mesh (left) has only 1 mesh seed spanning the width of the outlet extension.  After mesh size adjustment, there are now 5 or 6 mesh seeds.

6. Refine the mesh at the inlets, using Refinement Regions, to better capture the flow  characteristics in these local regions of high velocity air.

a. Click on Regions in the ribbon.

b. Click the Add button the the Mesh Refinement dialog box (a box will be surrounding the model).

TIP:  The view navigation cube can be used to quickly orient the model orthogonally to more easily position and size the region shape.  Also, changing the visual style to wireframe mode before adding regions will help to locate the region shape on internal features that would be hidden from view in shaded mode.

c. Use the Regions handles (blue arrows with red cylinders on the side opposite of arrow) to shrink, stretch, or move the region by left clicking and dragging over an actively selected handle. [Use handles to create a region similar to the one shown (size and location)].


Refinement Region sizing depicted from three orthogonal and one isometric view for clarification. 

d. Click the Get local mesh size button.

e. Change the value next to the slider to .03 and then hit Enter. (This number is the approximate uniform length of each element in the region.  The narrowest width of the inlet is 0.102 meters.  Dividing this number by 0.03 results in 3-4 elements across the width, not counting the mesh enhancement layers. )

f. Click Add to create another region for the other inlet.

g. Explicitly define this region's location and size (an alternate and more precise method compared to region handles). Fill in the Define region parameters as below (hit Enter after each entry):

X Offset -1.75
Y Offset 1.3
Z Offset 0.6
X Length 0.7
Y Length 1.2
Z Length 1.5

h. Click Get local mesh size.

i. Change the value next to the slider to .03 and hit Enter.

j. Click OK.

7. Solve the RefinedMesh analysis

a. Click on Solve in the Ribbon.

b. Click on the Solve button

8. Solve the DefaultMesh analysis

a. Double Click on the DefaultMesh node in the Design Study Bar to activate the scenario.

b. Click on Solve in the Ribbon.

c. Click on the Solve button.

The mesh and results will be evaluated at 2 locations; one of the inlets and the single outlet.  To directly compare the results between the different mesh versions, the Decision Center, will be used.  Several View Settings have been previously created and saved to expedite the comparison of results.

9. Apply view settings to get a visualization of the shaded mesh at the outlet and create a summary image.

a. While in Results mode, click on the View tab at the upper left of the interface and click on Apply View.

b. Select the file shadedmesh.xvs and then click the Open button.

c. Click on the Results tab.

d. Click on the Summary Image icon at the left of the Ribbon.

10.   Apply view settings to get a visualization of the shaded mesh on a plane slicing through an inlet and create a summary image.

a. While in Results mode, click on the View tab at the upper left of the interface and click on Apply View.

b. Select the file planemesh.xvs and then click Open.

c. Click on the Results tab.

d. Click on the Summary Image icon at the left of the Ribbon.

11.   Compare results using the Decision Center.

NOTE:  The next steps will require waiting until both simulations have completely finished solving; the Decision Center is not accessible while a simulation in the active study is running.

a. Click on Decision Center in the Results ribbon; the Decision Center will appear in the bottom left corner of the interface below the Design Study Bar.

b. Right click on the Design Review Center node in the Decision Center and select Update all images.

c. Now click on the View tab of the Ribbon

d. Change the viewports from a single port to two vertically split ports using the Viewports dropdown in the Window ribbon menu.

12. Review images

a. Click on the Image 01 node in the Decision Center

b. Click and drag the RefinedMesh scenario thumbnail image, located in the Output Bar at the bottom, into the viewport on the right.  Your screen should look similar to the one depicted below:


Decision Center comparison of the mesh at the outlet for DefaultMesh (left) and RefinedMesh (right).

To more clearly see the difference in these results, the resolution of the velocity legend range will be modified. 

c. Right Click directly on the vertical colored bar of the velocity legend and select Options … .

d. In the Legend Option dialog, type in 1.0 for the Max value and then click on the Close button.  The results should now appear similar to those depicted below.  Note that the modified legend range is now interpreted as “all areas colored RED are a value of 1.0 and higher”.


With the legend scale adjusted, there is now more contrast for the velocity values at the outlet.

e. Repeat  steps “a.” and “b.” for Image 02 which is the plane placed at one of the inlets.

f.  Zoom in on the inlet region to get the images below.


Decision Center comparison of the internal mesh at an inlet for DefaultMesh (left) and RefinedMesh (right).

 

OPTIONAL - Continue the mesh convergence process by running another incremental mesh refinement.

a. Clone the RefinedMesh scenario.

b. Adjust the mesh refinements to add more elements (e.g., change the mesh region values from 0.03 to 0.02).

c. Run the solution and compare the results again using the Decision Center.

Conclusion

The primary takeaway from this exercise is that the quality of the mesh will directly impact the quality of the results.   The default mesh, with less elements, was not able to capture the complex flow profiles.  Strategic refinement of the mesh improves the accuracy of the solution with the implication of taking a longer time to complete the solution.  The mesh convergence process, which employs multiple iterations of incremental mesh refinement, is the only way to validate the accuracy of the mesh.


1 This small area of high velocity flow at the outlet in the default mesh is removed in the refined mesh.
2 Notice the difference between the flow profile between the default and refined meshes.  Only having 1-2 elements spanning the outlet is not sufficient to resolve the flow profile.
3 With only 1-2 elements across the inlet in the default mesh, the flow profile cannot be resolved accurately which also impacts the ability the capture the plume of higher velocity air entering the space.
4

These nonuniform results in the default mesh, which appear to follow the element edges, are a clear sign of the need to refine the mesh in this area.  Notice the smoother velocity profiles in the refined mesh.

NOTE: Although this exercise focused on flow velocity profiles, other performance criteria such as pressure drop, flow recirculation and vertical thermal stratification, which are covered later, would also need to be evaluated to ultimately determine the quality of the mesh.

AttachmentSize
Package icon cfd-aec_exercise4_meshing.zip4.86 MB