## StarCCM Instructions This is a set of instructions our team has developed over time to make sure all CFD simulations are always run the same way. Based off Gator Motorsports' Instructions. Definitions come from a variety of tutorials on theansweris27.com ***(text) represents annotation to explain the instructions or definitions*** **Note: Save work often**
**1. Startup *(Create the simulation file)*** Click File -> New Simulation Select Parallel on Local Host Compute Processes: Use your logical processor count Select Power Session and Power-On- Demand Power-On-Demand Key: ***Ask team lead for this*** *Note: Save configuration for future use*
Click File -> Import -> Import Surface Mesh *Note: Make sure the file is a parasolid (.x_t file)* Select Ok
**2. Adding Wind Tunnel *(Defining the size of the wind tunnel. The size should be large enough so that the air on the outsides of the tunnel are unaffected by the part being tested, however too large of a volume will require more computer power)*** Open Geometry -> Right Click Parts Select new shape part -> select block Corner 1 Dimensions X = -5 m Y = -0.03 m Z = -5 m Corner 2 Dimensions X = 5 m Y = 6 m Z = 25 m *(To accommodate for the vortices from the car)* Click Create and then Close Rename Block to Wind Tunnel
Open Wind Tunnel (new block) Open Surfaces -> Right click Block Surface -> split by patch Select front of block -> Change Part Surface Name to Inlet -> Click Create Select back of block -> Change Part Surface Name to Outlet -> Click Create Select bottom of blcok -> Change Part Surface Name to Ground -> Click Create Close *Note: The front of the block would be where the front of the car is facing*
**3. Surface Wrapper *(Wraps the initial surface to provide a closed and manifold surfface mesh from a complex geometry)*** Right Click Operations (under geometry) -> New -> Surface wrapper Select the car body Open surface wrapper folder -> Open Defualt Controls Select volume of interest Under properties change Method to External Select Base Size Under properties change Base Size Value to 0.002 m Whichever value you're told for surface wrapper; one that
provides a clean surface (i.e. no bumps) *(Used 0.002)* Right click Surface Wrapper -> Execute
**4. Subtract Operation *(Removes the surface wrapper volume from the wind tunnel volume)*** Right Click Operation -> New -> Subtract Input Parts -> Select -> Surface Wrapper and Wind Tunnel Target Parts -> Select -> Wind Tunnel Select Execture operator upon creation Click Ok
Open Scenes -> Open Geometry 1 -> Open Displayers -> Open Geometry 1 Double click Parts Only have Subtract selected *Note: The holes where the wheels intersect with the block should be visible from the bottom*
**5. Physics Model** Right click Continua -> New -> Physics Continuum Double click Models Select: 3D, Constant Density, Steady, Turbulent, Gas, K-Epsilon
Turbulence, Segregated Flow, Cell Quality Remediation
Open Initial Conditions Select velocity Under properties change velocity value in the firection the wind
will be moving (15 m/s unless decifed otherwise)
Under Geometry -> Open Parts Right click Subtract and add "Assign Parts to Region" On the bottom open the second scroll down option Change to "Create a boundary for each part surface"
Open Regions Open Region -> Open Boundaries Select Inlet Under properties change Type to Velocity Inlet Open Inlet -> Open Physics -> Select Velocity Magnitude Change value to 15 m/s (same as the car's velocity Select Outlet Under Properties change Type to Pressure Outlet **
6. Creating Mesh** Right Click Operation -> New -> Automated Mesh Select Subtract At the bottom select: Surface Remsher: *(Remeshes the initial surface to provide a quality discretized mesh that is suitable for CFD. It is used to retriangulate the surface based on a target edge length supplied and can also omit specific surfaces or boundaries preserving the original triangulation from the imported mesh.)* Trimmed Cell Mesher: *(Generates a volume mesh by cutting a gexahedral template mesh with the geometry surface. It is recommended when an underlying custom mesh needs to be used or if the surface quality is not good enough for a polyhedral mesh. Besides, it is useful in modeling external aerodyanic flow due to its ability to refine cell in a wake region - unsteady and turbulent fluid caused by boundary layer seperation.)* Prism Layer Mesher: *(Adds prismatic cell layers next to the wall boundaries. The mesher projects the core mesh back to the wall boundaries to create prismatic cells.)* Automatic Surface Repair Click Ok
Open Automated Mesh -> Open Default Control Under Properties change Base Size value to 0.5m
Creating Surface Control Open Automated Mesh -> Right click Custom Controls -> Surface Control Open Custom Controls -> Select the new Surface Control Under properties in Part Surfaces click the three dots or the empty bracket Open Subtract -> Select Surface Wrapper
Open Surface Control -> Open Controls Select Target Surface Size Under Properties convert to Custom Select Minimum Surface size Under Properties convert to Custom Select Prism Layers Under Properties convert to Custom Open Prism Layers -> Select Customize Select Number of Layer Select Total Thickness Open Balues Select Target Surface Size Under Properties change to Absolute Open Target Surface Size -> Select Absolute Size Change Value to 0.003 Open Custom Prism Values Select Number of Prism Layers Change value to 12 Select Prism Layer Total Thickness -> Change to Absolute Open folder -> Select Absolute Size Change Value to 0.03m Select Minimum Surface Size Change to Absolute Open folder -> Select Absolute Size Change Value to 0.001 The larger the range between the two values the less errors
should occur along with a shorter mesh execution time *Note: The wider range between target size and minimum size might make the mesh run faster*
Creating Wall Control Open Automated Mesh -> Right click Custom Controls -> Surface Control Select the new surface control (Rename Wall Control) Click on the 3 dots next to Part Surfaces Open Subtract -> Open Wind Tunnel -> Select Block Surface Open the surface control (wall control) -> Open Controls Select Prism Layers Under properties change to Prism Layers to Disable
Right Click Automated Mesh -> Execute
**7. Reports** Right Click Reports -> New Report -> Force Select Force (Rename Drag Force) Under Properties Open Parts -> Open Regions -> Open Region -> Open Boundaries Select subtract.surface wrapper.body (select all faces corresponding to the car body) In Direction - adjust values to correct direction with value of 1 (In this case, only the z value would be used with a value of -1)
Right click Drag Force Create Monitor and Plot from Report
Frontal Area Create a new report Under Properties Open Parts -> Open Regions -> Open Region -> Open Boundaries Select subtract.surface wrapper.body (select all faces corresponding to the car body) (make sure the normal direction is the same firection as the
force report)
Drag Force Coefficient Create a new report Under Properties Open Parts -> Open Regions -> Open Region -> Open Boundaries Select subtract.surface wrapper.body (select all faces corresponding to the car body) In Direction - adjust values to correct direction with value of 1 (In this case, only the z value would be used with a value of -1) Reference Density - 1.225 kg/m^3 Reference Velocity - 15 m/s (same as car velocity) Reference Area - Frontal Area value
*Note Double click the report to show final value*
**8. Stopping Criteria** Different options: Disable maximum steps *(So the simulation does not stop when not complete) Open stopping criteria -> click Maximum Steps -> uncheck box
next to "Enabled"
Set up standard deviation Right click Stopping Criteria -> create new criterion -> from monitor Select Drag Force Monitor -> Ok Click Drag Force Monitor Criterion -> under properties drop
down Criterion Option -> Standard Deviation Open Drag Force Monitor Criterion -> click standard deviation Standard Deviation: 0.02N Number of samples: 100
Open Stopping Criteria Click Maximum Steps -> Change Maximum Steps to include 1000
more steps
**9. Run Simulation** Click the running man at the top *Note: On the Drag Force Plot the line should be leveling off as more iterations pass by.*
**10. After Simulation** Pressure Scenes Right click Scene -> New Scene -> Scalar Expand Scalar Scene 1 -> Expand Displayers -> Expand Scalar 1 Double click Parts Expand Regions -> Select subtract.surface wapper.body
(all faces corresponding to the car body) Double click Scalar Field For Function -> Click the three dots Select Absolute Pressure
Steamline Open Pressure Scalar Scene Right Click Derived Parts -> New Part -> Streamline For Seed Parts -> Click Select Open Region -> Wind Tunnel Inlet Select Part U and Part V resolution to 10 Click Create then Close
Expand Pressure Scalar Scene -> Expand Displayers -> Espand
Streamline Streamline Double click Scalar Field For Function -> Click the three dots Expand Velocity -> Select Magnitude
Vector Right click Scene -> New Scene -> Vector Expand Scalar Scene 1 -> Expand Displayers -> Expand Scalar 1 Double click Parts -> Expand Regions -> Select subtract.surface wapper.body
(all faces corresponding to the car body) Right click Displayer -> New Displayer -> Vector Expand Vector -> double click Parts Expand derived parts -> select Plane Section Plane Section Right-click derived part -> derived part -> section -> plane Select correct orientation (cutting through the profile of car)
**11. Rerun a simulation** To rerun a simulation and avoid setting it up from the beginning: At the top click Solutions and Clear Solutions With the given setting click OK