Guide to ANSYS Fluent

• For ANSYS installation, please refer to Nathan’s video: https://utexas.sharepoint.com/sites/ENGR-LonghornRacing/_layouts/15/stream.aspx?id=%2Fsites%2FENGR-LonghornRacing%2FLHR Solar%2FMechanical%2FMechanical Resources%2FHow to Install ANSYS.mp4&referrer=StreamWebApp.Web&referrerScenario=AddressBarCopied.view.49a1d015-f6b6-4e68-a8f6-a5a5b5c42740

• When downloading ANSYS, download it from the LHR Solar Sharepoint, not the general

• Make sure to do EVERYTHING in the video, including the VPN and editing your hosts file

How to run a simulation:

Workbench 

1. Geometry 

2. Import file 

3. Edit in space claim 

Space claim 

1. Repair 

   1. Stitch 

   2. Gaps 

   3. Missing faces 

   4. Split edges 

   5. Extra edges 

   6. Duplicates 

   7. Small faces 

2. Design → Planes 

   1. 10 cm below car 

3. Prepare → enclosure 

   1. Uncheck symmetric dimensions 

   2. Front: 4 x length 

   3. Back: 7 x length 

   4. top / bottom: 3 x height 

   5. Left / right: 3 x width  

   6. Check mark 

4. Structure tab (left)

   1. Suppress for physics (car file)

5. Hide enclosure 

6. Sketch 

   1. Rectangle around car (positive axis)

   2. No merge 

   3. Pull from both sides 

   4. Width + 500mm

   5. Taller Rectangle behind 

   6. No merge 

   7. Pull from both sides 

   8. Width + 1m

7. Select face of back boi, extend up to back face of enclosure 

8. Design → split body

   1. Hide car

   2. Split along both planes (keep positive axis)

9. Groups → create ns 

   1. Inlet 

   2. Outlet 

   3. Side

   4. Sky 

   5. Ground 

   6. Symmetry 

   7. Boinear 

   8. Boiwake 

   9. Fine 

   10. Mediumfine 

10. Hide groups 

11. Save file (ctrl+s)

12. Close space claim 

Workbench 

1. Duplicate geometry 

2. Edit in design modeler 

Design Modeler 

1. Right click import  

2. Generate 

3. Change 3 body types to fluid 

4. Change name → boinear / boiwake 

5. Save and close 

Workbench 

1. Fluent with fluent meshing 

2. Drag duplicate geometry to mesh 

3. Properties → m to mm 

4. Mesh → edit 

5. Double precision 

6. 8 processes when launching

Fluent meshing 

1. Import geometry 

2. Add local sizing 

   1. Body of influence x 2 

      1. Rename 

      2. Select option 

      3. Target mesh 

         1. Boinear 60mm 

         2. Boiwake 100mm 

   2. Curvature x 2 

      1. Rename 

      2. Select option 

         1. Fine 

            1. Local 1

            2. Max 8 

            3. Angle 14

         2. Mediumfine 

            1. Local 1

            2. Max 10

            3. Angle 16 

3. Generate surface mesh 

   1. Min 1

   2. Max 250

   3. Cells per gap 3 

   4. Generate mesh 

4. Geometry types 

   1. Consist of only fluid regions with no voids

   2. Describe geometry 

5. Update boundaries 

   1. Side and sky → symmetry  

   2. Update boundaries 

6. Update regions 

   1. Update regions 

7. Add boundary regions 

   1. Offset → last-ratio

   2. Layers 8 

   3. CFD - First cell height estimator  

      1. Target y+ 1

      2. Velocity 9 

      3. Length of car (check units)

      4. Calculate 

      5. Copy mm number 

   4. First height: calculated 

   5. Add boundary layers 

8. Generate volume mesh 

   1. Fill with: poly-hexcore

   2. Generate volume mesh 

9. Save and quit 

Workbench 

1. Setup 

2. Edit 

Fluent meshing 

1. Models → viscous → check curvature correction

2. Boundary conditions → inlet → inlet 

   1. Velocity 9 

   2. Turbulent intensity 3 

3. Boundary conditions → outlet → outlet

   1. turbulent intensity 1 

4. Wall → ground→ moving wall 

   1. Check direction of airflow (blue strings)

   2. Z → -1

5. Open reference values 

6. Reports → projected areas 

   1. Select fine and mediumfine 

   2. Min size 0.001

   3. Projection direction → Z

   4. Compute 

   5. Put in reference value area 

   6. Length of car 

   7. Temperature 303 

   8. Velocity 9 

7. Monitors → residual → show advanced options → convergence criterion → none 

8. Report definitions 

   1. New → force report → drag 

      1. Name: cd

      2. Direction: same as airflow 

      3. Select fine and mediumfine

      4. Print to console 

   2. New → force report → drag 

      1. Name: dragforce

      2. Direction: same as airflow 

      3. Output type: Drag force 

      4. Select fine and mediumfine

      5. Print to console 

   3. New → force report → lift

      1. Name: cl

      2. Direction: (0,1,0)

      3. Select fine and mediumfine

      4. Print to console 

9. Initialization 

   1. Hybrid initialization 

   2. Initialize 

10. Run calculations 

    1. Iterations 500 

    2. Calculate 

11. TACC Video: TACC Video