Blended Wing Body



The Blended Wing Body shape allows unique interior designs. Cargo can be loaded or passengers can board from the front or rear of the aircraft. But this kind of the wing used in military aircraft only. So, this project is about the flow visualization of the aircraft with blended wing body which provide diagnostic information about the flow around the Aircraft.

The Blended Wing Body Aircraft been made with all the Designing Parameters in SolidWorks as shown in Fig.1 below.

Fig.1: CAD Model of the Blended Wing Body Aircraft


For the Project compressible flow simulation type has been chosen because this type of aircraft moves at high Mach Number. Along with the K-omega SST turbulence Model which tells about the turbulence energy and scale. and the steady state is chosen as time dependency because this kind of simulation is been done under ISA (International Standard Atmosphere) So the values does not change with time.


Meshing is an important part of any kind of simulation. Hex-dominant is used as the algorithm of the Mesh. Along with the External meshing mode. As the accuracy of the result is depend on the Fineness of the Meshing.So, here Mesh Refinement is also used at the edges of Aircraft and Moderate Mesh is been used as the fineness of the Meshing with 16 number of processor. For external meshing mode two Geometric Primitives been used inner and outer box around the aircraft as shown in the Fig.2 & Fig.3 below.


Fig.2: Inner Mesh Box around the Aircraft


Fig.3: Outer Mesh Box around the Aircraft

After a Mesh operation of around 18 minutes here we got 1.3 M cells and 1.7 M nodes for this Meshed Blended Wing Body Aircraft as shown in Fig.4 below.

Fig.4: Meshed Blended Wing Body Aircraft


For this simulation AIR material is used from the material library of the SimScale. Air is applied over the complete volume of the aircraft as shown in Fig.5 below.

Fig.5: AIR applied over the complete volume of the aircraft


Initial conditions velocity for this simulation is given 500 m/s in Z-Direction.


For this simulation total five number of the boundary conditions been used

  • Velocity Inlet: velocity is applied at the inlet of the body with 500 m/s in positive Z direction as shown in the Fig.6 below.

Fig.6: Applied Inlet Velocity Boundary Condition on the aircraft

  • Pressure Outlet: Pressure is applied at the outlet of the aircraft body as shown in Fig.7 below


Fig.7: Applied Pressure outlet Boundary Conditions on the aircraft

Walls: The whole aircraft body along with the Geometric Primitives has been chosen as wall instead of inlet and outlet side of Geometric Primitives as shown in Fig.8 below


Fig.8: Walls Boundary Condition on the Aircraft

After completing the simulation setup simulation run 1 has been started which took around 184 minutes of time to get done and we got the Following result as shown in the Figure below.

Fig.9: Pressure changes at aircraft surface.

Fig.10: Pressure SIde view on the airfoil.

Fig.11: Energy of the Turbulence Produced during analysis

Fig.12: Scaling of the Turbulence

Fig.13; Velocity of the Fluid Flow


From all of the simulation result we can easily Visualize the Fluid Flow around the Aircraft which can help us in design optimization of the Blended Wing Body Aircraft.

Thank you:slightly_smiling_face:

1 Like

Really cool simulation but I would be a little concerned about what looks like negative temperatures as well as velocities that are much higher than the 500 m/s that you defined. Having looked at your simulation, a couple of thoughts;

  • You use a very coarse mesh, but it should be much finer, especially near the surface of the airplane. In your mesh log I see 100’s of elements have errors.

  • You did not set your velocity initial condition to 500 m/s. It’s not essential but it helps convergence

  • you set a Poutlet = 1 atm boundary just behind the airplane but I feel it may be too close to the airplane and that you should extend your air region as the area near your outlet boundary will still be heavily influenced by the airplane.

  • I don’t understand the purpose of the symmetry boundaries that you have set. It looks like you are trying to multiply the number of airplanes. I don’t think you should have these but you could cut the airplane and air volume in half across the plane of symmetry of the airplane and put a symmetry boundary in there to reduce runtime.

  • Under numerics you use the default min and max density of 0.5 and 2 kg/m3. I’m not certain that this density range is large enough for your study

  • Under simulation control you keep the default values of 0 to 1000 s and 1 s delta t. You don’t need 1000s to model these flow phenomenon but what you do need is a much much smaller delta t. Try for example simulating 0 to 10 seconds with delta t of 0.01 or even 0.001

Keep in mind that this is all general advice, I don’t have experience in supersonic flows


hi @roy_g
thanks for your advice and I think it would be better if I just try this simulation again with keep all these idea you have given me in mind.:slightly_smiling_face: because it is having errors in mesh.

Can you please tell me about this? because I tried this a lot of time with many project but every time I am facing these issue other issue is with particle traces which I never get.

The purpose of the symmetry boundary is that if there is a plane of symmetry in your model and you therefore expect the results to also be symmetrical about this plane, you can create a ‘half model’ and the define a symmetry boundary. This means you are only simulating half your model and it therefore reduces run-time. To do this you need to cut your airplane in half across its plane of symmetry (in your cad program) and then once you mesh your model in simscale you define a symmetry boundary on the cut surface.

For your mesh, try using a coarse mesh + inflate the boundary layer then send some pictures of it including cross sections and we can see if it looks reasonable.