AAE 450
A.4.1.2.5 4
As computer technology has greatly advanced, it has become an industry standard to use Computational Fluid Dynamics, CFD, as a preliminary form of aerothermodynamic analysis. A cheaper alternative to wind tunnel testing, CFD allows engineers to obtain accurate solutions to a variety of aerothermodynamic concerns. Because most aerodynamic theory falls apart in the transonic regime, it is hard to get accurate results using basic equations and analytical solutions. It is much more accurate to create a mock up of the launch vehicle and place it in a wind tunnel to retrieve physical results.
Creating a mock up of the launch vehicle becomes a very time consuming and costly task however, when the design begins to advance. As the design progresses, the launch vehicle geometry begins to change; since most aerothermodynamic loads are based on geometry, they are constantly changing as well. Every time the geometry of the launch vehicle changes, a new launch vehicle mock up needs to be built, and more wind tunnel tests need to occur. The alternative to these costly wind tunnel tests is CFD.
A CFD analysis can output the same type of information as a wind tunnel test in a timelier, more cost effective manner. Instead of paying for new launch vehicle mock ups to be created with each change in geometry, changes can simply be made in a CAD software program such as CATIA, ProEngineer, or SolidWorks. CFD can then be completed for each phase of the design, and costs associated with wind tunnel testing become obsolete.
Completing a CFD analysis on a launch vehicle can be broken down into a four step process:
1. Create a model of the launch vehicle in a CAD software program.
2. Import the launch vehicle geometry into a meshing program, such as Gambit or StarCCM+, and mesh the geometry.
3. Import the meshed geometry into a CFD program such as Fluent or Stardesign, set design parameters and environmental conditions, and run the program.
4. Post-process the output and analyze the results.
The results can then be used to determine whether or not the aerothermodynmic loads exceed tolerable values. If they do, a new design will need to account for these loads, and if not, more analysis can be done on other components of the launch vehicle design.
What makes CFD nearly as accurate as wind tunnel testing are the numerical methods imbedded internally within the CFD program. By meshing the CAD model first, the launch vehicle is broken down into small pieces. When placed into the CFD program, solutions to Navier-Stokes equations are integrated across each of these small pieces, and summed in order to solve for a multitude of aerodynamic loads. Outputs can range from pressure, temperature, and velocity distributions to coefficient of drag, coefficient of pressure, and moment coefficient acting on the launch vehicle.
CFD is an incredibly advantageous tool because it allows for geometry changes as well as environmental changes to be taken into consideration. By specifying the appropriate boundary conditions one can change the speed and angle of attack of the launch vehicle, account for changes in temperature, density, and pressure of the surrounding atmosphere, and even include viscous effects and shock waves.
Due to the cost, time, and inaccessibility of a wind tunnel, we decided to use CFD as a means of determining aerothermodynamic loads at designated intervals throughout the launch. In order to exploit Fluent’s symmetry capability we created a model of half of the 1 Kg launch vehicle using CATIA. Splitting the launch vehicle in half reduces the complexity along with the amount of time to needed to solve the problem. We then saved this model as a “.igs” file, and imported into GAMBIT.
Once in GAMBIT, the model was nearly ready to be meshed. In order to account for the fact that air flows around the launch vehicle and not through it, the area surrounding the launch vehicle model needed to be meshed, rather than the launch vehicle itself. To do this, we created a large rectangular prism surrounding the launch vehicle. The launch vehicle geometry was then subtracted from this rectangular prism leaving only the area surrounding the launch vehicle to be meshed.
To begin, we meshed the edges of the rectangular prism with a spacing of 0.8. Next, the longest symmetry plane edges of the launch vehicle were meshed with a spacing of 0.13, and the smallest symmetry plane edges of the launch vehicle were meshed with a spacing of 0.05. Using the edge mesh sizes as guides, we meshed the faces of the launch vehicle and the faces of the rectangular prism next. We created both of these face meshes using a triangular mapping pattern. Finally, the volume surrounding the launch vehicle was meshed using a tetrahedral hex-core pattern. The results of the mesh can be seen in Fig. A.4.1.2.5.1 below.
Fig A.4.1.2.5.1: Mesh of 1Kg launch vehicle in GAMBIT
(Jayme Zott, Chris Strauss, Brian Budzinski)
After meshing was complete, we broke up the launch vehicle into zones. We designated the face of the rectangular prism in front of the launch vehicle as a pressure inlet, and the face behind the launch vehicle as a pressure outlet. We designated the face aligned with the symmetry plane of the launch vehicle as symmetry, and the remaining faces as walls.
Once meshing was complete and the launch vehicle had been broken up into zones, we exported the mesh into Fluent. Table A.4.1.2.5.1 describes the settings and boundary conditions we chose within Fluent.
Table A.4.1.2.5 Summary of Fluent settings and boundary conditions for 1 Kg launch vehicle at 350 m/s.Setting/Boundary Condition / Value
Solver / --
Pressure based
GG node based
Implicit
Steady / --
--
--
--
Energy
On
Viscosity
Inviscid
Materials
Ideal Gas
Operating Conditions
Pressure Inlet Boundary Conditions
Total Pressure
Supersonic
Pressure Outlet Boundary Conditions
Outlet Pressure
Solution Controls
Pressure/Velocity
Pressure Model
Pressure Accuracy
Courant Number
Relaxation factor / --
--
--
--
--
--
0 [atm]
1.3 [atm]
0.65 [atm]
0.65 [atm]
Coupled
Standard
2nd order upwind
5
0.5 /
We based our choices for the settings and boundary conditions shown in table A.4.1.2.5.1 on Fluent tutorials1, Fluent webinars2, conversations with graduate students and professors3, and trial and error. The solver was chosen to be pressure based because pressure based is most accurate for supersonic flows. The energy equation was turned on as a requirement for incompressible flow. The viscosity was chosen to be inviscid, because viscous forces are negligible at zero angle of attack. The boundary conditions for the pressure inlet and outlet were chosen based on the desired launch vehicle velocity. The remaining settings and boundary conditions were based more on trial and error than anything else. Overall, we attempted many different solution possibilities, from adapting the gradient of the grid to account for the formation of shock waves, to testing out a density based solver, to reducing the Courant number all the way to 0.01. There were many different options tested, and while our output seems intuitively reasonable, it is hard to say whether or not the settings displayed in table A.4.1.2.5.1 are the best for analyzing the supersonic flow of air around our launch vehicle.
The results for the pressure distribution of the 1Kg launch vehicle traveling 350 m/s at zero angle of attack can be seen in Fig. A.4.1.2.5.2. The scale on the left displays a color schematic representing the range of pressures distributed across the launch vehicle. The lowest pressure, colored blue, begins at 0.37 atm, and the greatest pressure, colored red, stops at 1.56 atm. The pressure is highest at the locations where a sharp edge occurs, and lowest in the areas immediately after them. Based on our initial boundary conditions, and the high probability that the flow is separating near the base of each skirt, these results seem reasonably accurate.
Figure A.4.2.1.5.2 Pressure distribution of 1 Kg launch vehicle
(Jayme Zott)
The results for the velocity distribution of air surrounding the 1Kg launch vehicle traveling 350 m/s at zero angle of attack can be seen in Fig. A.4.1.2.5.3. The scale on the left begins in blue at 5.89 m/s, and ends in red at 411 m/s.
Figure A.4.2.1.5.3 Velocity distribution of air surrounding 1 Kg launch vehicle traveling 350 m/s
(Jayme Zott)
The velocity is greatest at the locations where the skirts end, and lowest slightly after that location. Shocks are most likely forming at the base of the skits where a significant change in the launch vehicle geometry occurs. These probable shock locations correlate well with the velocity distribution, and the velocity magnitudes correlate well with our initial boundary conditions. We therefore assume that the results are reasonably accurate for use in our aerodynamic analysis.
Since the bottom line aerodynamic analysis for the launch vehicle design was completed using call_aerodynamics.m, we used CFD as a sanity check for the linear perturbation theory output. With both of these methods working together, we were able to get a solid idea of the type of aerodynamic loading the launch vehicle was likely to experience throughout its flight.
Author: Jayme Zott