2-D Scramjet Simulation
 

Hi All,

I am trying to perform a 2-D simulation on a Scramjet Combustor and I guess the back pressure increase due to combustion is getting so high that its pushing out the oblique shock wave out of the combustor. If I decrease the back flow pressure will that solve my problem ?

Thanks,
CPT

Could you please furnish some more details about the problem you are simulating???

1) What part of scramjet you are simulating?? Inlet with forebody ramps?? or just inlet???

2) Which shock you are talking about?? Ramp shock or tip shock???

3) What are flow conditions? Geom details??

4) is the inlet chocked? meaning are you getting a bow shock???

Hi Nilesh,

Thanks for getting back concerning my post.

Actually the problem I was facing before has been solved but now another error has been occurring.

I am performing 2-D simulation of a wall injected scram combustor using FLUENT with reduced reaction mechanism (7-step). The turbulence model used is k-epsilon realizable and combustion model being used is EDC (eddy dissipation concept). I am not using CHEMKIN to feed in the reaction mechanism, rather I am feeding the reactions and all the rate parameters directly in FLUENT reactions page. The cold flow with h2 injection has already been established and then I am switching on the reaction chemistry but the cold flow with injection and no combustion was simulated using the laminar finite rate model without the reaction mechanism fed into the FLUENT.

Now its been 4000 iterations and the max temperature in the duct as found in 3-D Numerical Simulations is around 2200 K as compared to mine being 8000 K. I was thinking that are these the transients which eventually will die out and slowly the flow and the flame will spread over as the simulation proceeds.

Kindly lemme know if there is any other detailed information you need.

Thanks,
CPT

Guess m bit late now...I could have helped with inlet aerodynamics part, but combustion is not my area of expertise.:(

Hey Nilesh,

Thats completely fine ! Thanks for your concern though :)

CPT

Not sure as how Setting up mesh and flow setup is done?
 

Hi Nilesh i am working on simulating flow around the inlet of the scramjet, but i am not sure as to how i am supposed to apply hybrid mesh?
to clarify more on the problem i am trying to simulate

1) i am trying to simulate the scramjet inlet
2) i need to look into the ramp shock
3)the flow conditions are:-
Altitude = sea level
M=5
T=288.2 K
P= 1.0133*10^5 Pa
Density= 1.2252 kg/m^3
Reynolds Number= 1.71*10^5

^^^ @stanp_

Well what kind of hybrid mesh you are looking for exactly?? is it unstructured tet+prism layer?? Or hex + tet

I am not sure what you really need. A little more specific question would help.:confused:

I am looking to make the mesh unstructured tet+prism layer.

The task i am looking into is shock-viscous interactions in the scramjet inlet.
looking to obtain results-

-Velocity, Pressure and temperature contour
-phenomena of shock-waves with sudden pressure changes

I have attached a few image of my work done so far
1) Inlet Geometry
2) Mesh
3)Sphere of influence around the inlet (finer mesh for regions of expected shockwaves)

I hate to say it but your mesh quality is terrible. Your mesh on the surfaces is so coarse it has lost all detail of the curvature and changed the shape dramatically. The mesh has not even resolved the sharp point and has made it a blunt stub. Then you combine this with a much finer volume mesh which results in a horrible transition from the inflation layers to the volume mesh.

I can safely say this simulation will never converge with a mesh that bad. You need to dramatically improve the mesh quality.

OK...

1. Why you have so big domain upstream of the inlet?? Which shock wave you are expecting in the shown sphere of influence. If your area of interest in inside the ramp, then you need mesh only inside the scramjet inlet. In any case the computational domain needs to be only a little ahead of the 1st shock you would get, which would be at the tip of the ramp. Everything upstream is uniform supersonic flow at free-stream conditions.

2. Well, @ghorrocks has said it all about the mesh. Its not gonna work. There will be bow shock with such blunt tips.

3. All the simulations I have done for scramjet inlet have been structured hex grids. I never tried hybrid mesh. But I can tell you this much that you need to resolve all shocks and the boundary layer region adequately to get good results.

I am attaching a pic of the mesh we (@IITB) used when we simulated Shock-Turbulent BL interaction in scramjet inlet. Its a 3D mesh but nevertheless it will give you some idea about the domain size required and all. The contour planes show full mesh cross section. And the mesh starts just ahead of the ramp tip. I cannot find image of 2D sims I have done in past.

You work on the domain size first and then refine mesh along the boundary layer region and along the ramp shocks. Inviscid shock calculations will tell you where to expect at-least the primary shocks.


Questions:

1. which code/software you are planning to use??
2. Turbulence model??
3. steady/unsteady??
4. when u say "phenomena of shock-waves with sudden pressure changes", what pressure change you are referring to?? Free stream??

Thank you for replying back so quickly, i will look into working on the domain size first and then refining the mesh.

to answer your questions:-

1) The code/software i am using is ANSYS-CFX
2) Shear Stress Transport (SST) model

Thank you for your feedback, i will look to improve the domain sizing and mesh quality.

Thank you for replying back so quickly, i will look into working on the domain size first and then refining the mesh.

to answer your questions:-

My area of interest was inside the ramp so i have changed the mesh inside the scramjet inlet
1) The code/software i am using is ANSYS-CFX
2) Shear Stress Transport (SST) model
3) Steady
4)Free stream pressure

If I was you, I would do a benchmark simulation (such as a convergent-divergent nozzle) so you get some experience in modelling shock waves in flows with good benchmark simulations. Once you can get known flows modelled accurately then you can move to your geometry.

i have once meshed a supersonic inlet in icem cfd :
http://www.youtube.com/watch?v=7WF8niG1suM