[Abhinand]

Hello guys,
I have been trying to simulate supersonic flow over a flat plate in inviscid flow.
But however I change my relaxation factor my residuals start to shoot up after some 600 iterations.
I have checked the mesh and it has low skewness and good quality structured mesh
Can you ease suggest ways to improve the convergence and solution controls if I have to change anything new

Thanks very much

[Kirill-MIPT]

Originally Posted by Abhinand

Hello guys,
I have been trying to simulate supersonic flow over a flat plate in inviscid flow.
But however I change my relaxation factor my residuals start to shoot up after some 600 iterations.
I have checked the mesh and it has low skewness and good quality structured mesh
Can you ease suggest ways to improve the convergence and solution controls if I have to change anything new

Thanks very much

Hello!

Can you please show the mesh and geometry?

Which boundary conditions do you use?

Did you turn on the energy equation?

What EOS do you use?

Sent from my Redmi Note 3 using CFD Online Forum mobile app

[Abhinand]

Thanks for the reply,
My geometry is just a plain structured rectangular mesh
BCS
Inlet -pres inlet
Outlet -farfield
Plate - wall
Other surfaces - symmetry

Yes the energy equation is on
I used pressure based solver since density based is going too much divergent

Solution controls is all default intially with lower order scheme then higher order

[Kirill-MIPT]

Originally Posted by Abhinand

Thanks for the reply,
My geometry is just a plain structured rectangular mesh
BCS
Inlet -pres inlet
Outlet -farfield
Plate - wall
Other surfaces - symmetry

Yes the energy equation is on
I used pressure based solver since density based is going too much divergent

Solution controls is all default intially with lower order scheme then higher order

Please describe the mesh and geometry more throughly. The best for me in this case is to see the picture of the mesh

OK, and what about the freestream parameters?

You didn't answer the question about the equation of state

For compressible cases (and your case is compressible) use density based solver, implicit scheme, ausm, Courant number ~ 1, green-gauss node-based and 1st order of approximation. Try this and don't forget to let me know about what I asked

By the way, how do you initialize the problem? For initial values of flow parameters you should use the freestream values

Sent from my Redmi Note 3 using CFD Online Forum mobile app

[Abhinand]

Hello,
Thank you very much for your reply. My free stream parameters are set to Mach 2.56 and gauge pressure of 1atm with operating conditions of 0Pa.

Sorry I could not understand what you wanted to know my EOS. Can you explain a bit.

I have used standard initialization and yes I initialized with freestream parameters only. (P_inlet)

Here is a picture of my mesh. The middle domain is the portion where an injector is employed to inject into supersonic flow

[Kirill-MIPT]

Originally Posted by Abhinand

Hello,
Thank you very much for your reply. My free stream parameters are set to Mach 2.56 and gauge pressure of 1atm with operating conditions of 0Pa.

Sorry I could not understand what you wanted to know my EOS. Can you explain a bit.

I have used standard initialization and yes I initialized with freestream parameters only. (P_inlet)

Here is a picture of my mesh. The middle domain is the portion where an injector is employed to inject into supersonic flow

Eos is equation of state. Did you use ideal gas eos or something else?

Can you send the case file for me?


Sent from my Redmi Note 3 using CFD Online Forum mobile app

[Abhinand]

Yes, I used ideal gas only.
Can u tell me how to select solution controls depending on the problem.
I tried with the settings yous said, the residuals keep on decreasing. What should I do to converge them

[Kirill-MIPT]

Originally Posted by Abhinand

Yes, I used ideal gas only.
Can u tell me how to select solution controls depending on the problem.
I tried with the settings yous said, the residuals keep on decreasing. What should I do to converge them

For supersonic problems it's enough to use solutions controls that I listed above. Even flows over bodies with complicated forms can be calculated under these conditions. The last thing that can be useful at the beginning of calculation is reducing Courant number to about 0.1.

Looking through your case file can be useful. There is possibly a problem with mesh or boundary conditions. But I have 15th version of fluent

Did you create your mesh via Pointwise?

Sent from my Redmi Note 3 using CFD Online Forum mobile app

[Abhinand]

Yes, I created the mesh with pointwise. I have just a plain refined structural mesh. What could be the problems with the mesh that can happen?

BTW thank you, my solution converged. But isnt it advisable to move to higher order scheme to get better results?

Can you tell me how to vary courant number as the solution progresses, what should we do if residuals starts to increase suddenly. What to do if it goes on a straight line? How do we proceed such situations

Thank you very much for your timely help

[Kirill-MIPT]

If you had no symmetry conditions, there would be problems in the stagnation point

You are welcome! Maybe it has sense in case of viscid flow for your problem. Higher orders are good for complicated geometries with separate flows

You can increase it to
accelerate convergence, but don't forget to save case and data. For each problem there is its own highest Courant number, and the precise value of it isn't obvious at all

Sudden growth is OK when one changes a turbulence model or approximation order (in this case residuals level quickly reduces to the value it used to have before). But for a case when they jump several orders up high and the solution breaks down, then one should consider calculation control problems or mesh/geometry problems and even physical models that are used in the problem

Sent from my Redmi Note 3 using CFD Online Forum mobile app

[Abhinand]

thanks for your reply.
I just have a small doubt. How do we be certain about the type of solver and scheme if we are solving a viscid flow. If the residuals are not decreasing as we think, how should we change the solver?
For example, may I ask how did you know that Green gauss node based would work with implcit solver?. How do we determine that

Many thanks

[Kirill-MIPT]

Ausm gives precise solution of Riemann problem. Green-Gauss theorem calculates gradients of pointwise defined functions much better than least square method (the latter needs many points to achieve accuracy). Implicit scheme turns to be stable more often than explicit. That's why me and my colleagues use these parameters for hypersonic flows calculation

Sent from my Redmi Note 3 using CFD Online Forum mobile app

[Abhinand]

Thanks a lot. The problem is Im continuing the same problem in viscous flow with a grid spacing according to y+ value and the free stream parameters. But when I run it, I find it very difficult to converge and changing none of the parameters seem to be changing the status of the residuals.
So for a start if I have used AUSM Implicit, Green gauss node based with courant number 0.96
after some 1000 iterations its starts to increase rather than oscillate between values.
What should be my first step to make the residuals decrease and converge?

Many thanks for your time

[Kirill-MIPT]

For different problems residuals change in very different ways. Maybe for your problem a permanent growth is OK. Often in case of flow over blunt bodies residuals fall down very slowly. Play with Courant number - try increasing it by two or more times

Sent from my Redmi Note 3 using CFD Online Forum mobile app

[Abhinand]

Yes I tried playing with the Courant numbers, initially I increased it and after sometime it started to detect divergence, so I reduced it back again.
If the residuals are exactly oscillating in a continuous fashion however you change your Courant numbers are they considered to be converged??
Thanks a ton for your help

[Kirill-MIPT]

So find highest Courant number since which divergence doesn't take place

In case of hypersonic viscid flows residuals sometimes oscillate around a line that decreases very slowly (so the residuals also reduce in general). Try waiting for 10000 or more iterations

Sent from my Redmi Note 3 using CFD Online Forum mobile app

[paragmangave]

Originally Posted by Kirill-MIPT

Please describe the mesh and geometry more throughly. The best for me in this case is to see the picture of the mesh

OK, and what about the freestream parameters?

You didn't answer the question about the equation of state

For compressible cases (and your case is compressible) use density based solver, implicit scheme, ausm, Courant number ~ 1, green-gauss node-based and 1st order of approximation. Try this and don't forget to let me know about what I asked

By the way, how do you initialize the problem? For initial values of flow parameters you should use the freestream values

Sent from my Redmi Note 3 using CFD Online Forum mobile app

I have been trying to simulate flow over blunt bodies at Mach number 2 so my domain is rectangular with 10 infront of body 15 times backward and 10 times in up and below the body...Can you plz suggest the necessary bc for same for calculation of drag

[Kirill-MIPT]

Originally Posted by paragmangave

I have been trying to simulate flow over blunt bodies at Mach number 2 so my domain is rectangular with 10 infront of body 15 times backward and 10 times in up and below the body...Can you plz suggest the necessary bc for same for calculation of drag

Sorry, I didn't get your calculation area parameters properly. Can you please show the mesh?

Sent from my Redmi Note 3 using CFD Online Forum mobile app

[paragmangave]

Originally Posted by Kirill-MIPT

Sorry, I didn't get your calculation area parameters properly. Can you please show the mesh?

Sent from my Redmi Note 3 using CFD Online Forum mobile app

please see the following image of mesh

[Kirill-MIPT]

1) For this type of the flow one should use computational region with inlet adapted to the shock wave (i.e. very close to it)

By the way, is attack angle = 0? If so, you need a 2D case, not 3D



2) I usually don't need to calculate flow over bottom area so I draw something like this. And do you?



3) Is your problem viscid or not? If viscid, your need inflation near the wall