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