Now that you have a computational mesh for the Piper Cherokee, set up and run a simulation on it.
General Settings
To start, define the overall type of simulation that you wish to run. Do this in the General section at the top of the control panel.
For the Piper Cherokee, stick with the defaults, which are:
Time set to Steady: Solving for a snapshot of the flow field at a single point in time, rather than a flow that changes with time.
Gravity set to Off: Ignoring the effect of gravity.
Create a Material
Next, pick the material to simulate in the Material section. To simulate air flow around the airplane, you'll need to create a fluid.
Click the + icon next to Material.
Select Fluid.
In the properties panel below, set Material to Standard Air.
Now assign a volume to this material. Click in the box and select Volume 1 from the Geometry panel.
Create Physics
Now assign physics to the fluid material. To create fluid flow physics, select volumes, define boundary conditions, and other settings.
Click the + icon next to Physics.
Select Fluid Flow. This will create a new Fluid Flow item in the control panel and open settings in the properties panel.
Ensure that Viscous Model is set to RANS and Turbulence is set to Spalart-Allmaras.
Next, specify which volumes will be assigned these physics:
Click Volume Selection.
Click in the box and select Volume 1 from the Geometry panel.
Set Boundary Conditions
The next major step is to define the boundary conditions. Start with the boundary condition for the far-field, which represent the flight conditions of the airplane. It will be flying at a subsonic speed at an altitude of around 3,000 meters and an angle of attack of 2°.
Click the + icon next to Boundary Conditions.
Select Far-Field and set the following properties:
Static Pressure: 70,100 Pa
Mach Number: 0.216
Temperature: 288.15 K
Flow Direction: Choose Flow Angles
Angle of Attack: 2°
Scroll down and click inside the box to select the Far-Field surface group from the Geometry panel, then click outside the box to save.
Now create one on the airplane. Set this up as a no-slip wall, meaning that the air particles directly next to the wall are not moving
Select Boundary Conditions. You’ll see a list of undefined boundaries in the properties panel.
Click Define All and select Wall. This will create a new wall boundary condition, opening the settings for this boundary condition in the properties panel.
Make sure that Momentum is set to No-Slip.
Define Initial Conditions
Next, define the initial conditions. These are the initial values assigned to control volumes before running a simulation, and setting reasonable values can help a simulation converge quicker. In some cases they can also affect the final result.
Click Initialization.
In the properties panel, ensure Initialization is set to Far-field Values.
Create Outputs
By default, a simulation will output the solution residuals at each iteration. These should gradually trend downwards as the simulation converges towards a solution, and tracking them can help understand how well the simulation process is performing.
You can also define many different custom outputs that may be quantities of interest for different cases. For this simulation, define outputs for the lift and the drag of the airplane at its current flight conditions.
To define lift as an output variable:
Click on + symbol next to the Outputs section in the control panel.
Select Surface.
Set Quantity to Lift (N).
Set Reference Frame to Body Frame.
Scroll to the bottom of the properties panel and click in the box to choose which surfaces to calculate lift over. Select the Airplane surface from the 3D Viewer or Geometry panel and then click outside the box to save.
To define drag as an output variable, follow the same overall process, but ensure that Quantity is set to Drag (N).
Set Stopping Conditions
Stopping Conditions are used to determine when a simulation exits and saves results. In the case of the Piper Cherokee, use stopping conditions based on the number of iterations and one of our custom output quantities:
Click on Stopping Conditions in the control panel.
Set Max Iterations to 2,000. This means that if the simulation hasn't met the other stopping conditions criteria by the time it has run 2,000 iterations, it will save and exit then.
Next, under Conditions, set Stop If to ALL Conditions are met. This means all the following stopping conditions must be met for the solution to save and exit early.
Click + Add Stopping Condition.
Set Output Name in the new stopping condition to be Lift.
Set the following:
Tolerance: 0.01%
Start at Iteration: 500
Averaging Iterations: 10
Iterations to Consider: 5.
This means that starting from the 500th iteration, the platform will calculate an average value of lift based on the last 10 iterations, inclusive. It will then compare the variation of this trailing average over the last five iterations, inclusive. If this varies by less that 0.01%, the stopping condition will have been met.
You should see that there are no red dots alongside any sections in the control panel (all required settings have been assigned), and the Run Simulation button at the top is active.
Run Simulation
If everything is set up correctly in the control panel, the Run Simulation button at the top will become active.
Clicking this button will launch a new simulation and open a Simulation tab showing you the current status of the run. Once the simulation has finished, this new tab can also be used to analyze the results and create visualizations.
On the left of the 3D Viewer, you will see a collapsible Run Status summary. The Output monitors at the bottom will, once the simulation starts, show a graph of the residuals or other chosen output quantities. By watching these three components you can see the current status of the simulation and track its progress.
This sample project will run for 2,000 iterations. At this point it will stop, saving all of the data for the last iteration.
To run this simulation for additional iterations:
Click on Post-processing at the top of the control panel.
Select Setup Details.
Click the Copy to Setup icon at the top of the control panel. This will copy all the settings used in this simulation to the Setup tab, and set the initial conditions for a new run to be the values from the final iteration of the previous run.
Next Steps
Now that you've run a simulation, you can move on to:
Analyze the results
Visualize flow movement with Visualization Tools
Use the buttons below to choose.