[panagiat]

Hello!

I recently made a steady-state FVM Incompressible 2D Navier Stokes solver using the SIMPLE algorithm for a collocated cartesian orthogonal grid in C++.

As far as the discretization goes, for diffusion and pressure I am using central differencing and for convection I am using 1st order upwinding (for which I have read that does not have any conditions regarding stability as far as the Reynolds number goes). I am also using under-relaxation with values of 0.7 and 0.3 for velocity and pressure.

It seems to be working perfectly for some benchmark problems such as the lid-driven cavity, provided the reynolds number is not too high (not over 1000) in a 100x100 grid. Though it diverges for higher reynolds numbers and this happens to be the case for other problems as well such as pipe flow and flow against a circle (each problem seems to pose a different "limit" for Reynolds number in terms of convergence though no problem seems to be able to pass the 1000 Reynolds number mark). I am also noticing a sudden (maybe exponential?) increase in convergence time when that limit is approached until it doesn't converge anymore.

So, so my question is:
Are there any other convergence criteria I am missing?

As far as the solver selection, I know that the SIMPLE algorithm I am using makes a simplification regarding the velocity correction equations, which inherently makes it prone to divergence.
So would another solver improve the situation? (SIMPLER, SIMPLEC, PISO etc.)

As far as the discretization schemes, is it true that by introducing higher order schemes (even just for the reynolds numbers they would support regarding stability) increase convergence rate? From what I've read they can only increase the accuracy of the result but I could be mistaken.

I've also read that people use turbulence models at higher reynolds numbers where turbulence plays a bigger role. Would implementing a turbulence model such as k-ε improve convergence or does it only have to do with capturing the turbulent effects themselves rather than helping with convergence?

Lastly, could the culprit be the mesh itself? Would modifying my code to work for unstructured meshes and thus being able to add more detail to BC's also improve it?

Anything else that could hinder convergence?
I am really confused on the convergence part since there seem to be so many things that can affect it. It also amazes me how people manage to converge more complicated problems such as flow around airfoils where the Reynolds number can hit the millions, with such high velocity and low viscosity.

Thanks!

[LuckyTran]

who said 1st order upwind is always stable? LOL

Even 1st order upwinding is unstable at high Courant numbers. For sure, for a fixed grid, if you strictly increase the velocity, then there is for sure a critical Reynolds number that will diverge.

Higher order schemes increase the order of the accuracy, not necessarily the absolute accuracy. Although ideally, and in theory, the two should be positively correlated. Convergence rate is also hard to define. Does convergence rate include mesh refinement? If so, then higher order schemes will converge faster (w.r.t. to the mesh) than a low order scheme. Does convergence rate mean compute power consumed to get to the answer? Well then higher order schemes also excel here.

Turbulence models are for modeling turbulence. If you have no turbulence model, your solver should still work, you just don't model what happens in reality. You continue to solve whatever is your model equations and your solutions are "accurate" in the mathematical sense and they should converge to the correct numerical solution, which may be different than what you expect to occur in real life. Note that there is a difference between "what you expect to occur in real life" and "physically meaningful." What you don't expect may still be physically meaningful, because flows can remain laminar at extremely high Reynolds numbers if perturbations are well controlled. So, it is still accurate numerically, and physically real, even if it is not what you expect.

There definitely is an influence of the grid size.

[panagiat]

Originally Posted by LuckyTran

who said 1st order upwind is always stable? LOL

Even 1st order upwinding is unstable at high Courant numbers. For sure, for a fixed grid, if you strictly increase the velocity, then there is for sure a critical Reynolds number that will diverge.

Higher order schemes increase the order of the accuracy, not necessarily the absolute accuracy. Although ideally, and in theory, the two should be positively correlated. Convergence rate is also hard to define. Does convergence rate include mesh refinement? If so, then higher order schemes will converge faster (w.r.t. to the mesh) than a low order scheme. Does convergence rate mean compute power consumed to get to the answer? Well then higher order schemes also excel here.

Turbulence models are for modeling turbulence. If you have no turbulence model, your solver should still work, you just don't model what happens in reality. You continue to solve whatever is your model equations and your solutions are "accurate" in the mathematical sense and they should converge to the correct numerical solution, which may be different than what you expect to occur in real life. Note that there is a difference between "what you expect to occur in real life" and "physically meaningful." What you don't expect may still be physically meaningful, because flows can remain laminar at extremely high Reynolds numbers if perturbations are well controlled. So, it is still accurate numerically, and physically real, even if it is not what you expect.

There definitely is an influence of the grid size.

Thanks for the detailed answer. Is the courant number relevant in my case where am solving a steady-state? If so, how can this be since I don't have defined any dt? Is there any pseudo time step taken into consideration?

Regarding turbulence, if I understood correctly, for example, whether the problem I am solving is a plain lid-driven cavity or a fully fledged airfoil simulation at high reynolds, or anything else, turbulence models should not have any effect on whether or not the solver will converge, it's there just for modelling what would probably happen in reality.

[sbaffini]

Originally Posted by panagiat

Regarding turbulence, if I understood correctly, for example, whether the problem I am solving is a plain lid-driven cavity or a fully fledged airfoil simulation at high reynolds, or anything else, turbulence models should not have any effect on whether or not the solver will converge, it's there just for modelling what would probably happen in reality.

I don't know if that was the original point BUT, I would highlight that indeed lack of convergence may well be due to the fact that you are trying to catch a steady solution with a steady solver while, in fact, at those Re numbers, your solution cannot be steady.

In this regard, adding a turbulence model based on eddy viscosity, always increases the flow stability and, as a consequence, helps convergence. Altough, deciding if this is actually the correct thing to do in that specific case is a totally different matter and the answer is not always obvious, especially for 2D flows at barely transitional Re numbers.

[panagiat]

Originally Posted by sbaffini

I don't know if that was the original point BUT, I would highlight that indeed lack of convergence may well be due to the fact that you are trying to catch a steady solution with a steady solver while, in fact, at those Re numbers, your solution cannot be steady.

In this regard, adding a turbulence model based on eddy viscosity, always increases the flow stability and, as a consequence, helps convergence. Altough, deciding if this is actually the correct thing to do in that specific case is a totally different matter and the answer is not always obvious, especially for 2D flows at barely transitional Re numbers.

That is a good point, thanks!

[FMDenaro]

Originally Posted by panagiat

Hello!

I recently made a steady-state FVM Incompressible 2D Navier Stokes solver using the SIMPLE algorithm for a collocated cartesian orthogonal grid in C++.

As far as the discretization goes, for diffusion and pressure I am using central differencing and for convection I am using 1st order upwinding (for which I have read that does not have any conditions regarding stability as far as the Reynolds number goes). I am also using under-relaxation with values of 0.7 and 0.3 for velocity and pressure.

It seems to be working perfectly for some benchmark problems such as the lid-driven cavity, provided the reynolds number is not too high (not over 1000) in a 100x100 grid. Though it diverges for higher reynolds numbers and this happens to be the case for other problems as well such as pipe flow and flow against a circle (each problem seems to pose a different "limit" for Reynolds number in terms of convergence though no problem seems to be able to pass the 1000 Reynolds number mark). I am also noticing a sudden (maybe exponential?) increase in convergence time when that limit is approached until it doesn't converge anymore.

So, so my question is:
Are there any other convergence criteria I am missing?

As far as the solver selection, I know that the SIMPLE algorithm I am using makes a simplification regarding the velocity correction equations, which inherently makes it prone to divergence.
So would another solver improve the situation? (SIMPLER, SIMPLEC, PISO etc.)

As far as the discretization schemes, is it true that by introducing higher order schemes (even just for the reynolds numbers they would support regarding stability) increase convergence rate? From what I've read they can only increase the accuracy of the result but I could be mistaken.

I've also read that people use turbulence models at higher reynolds numbers where turbulence plays a bigger role. Would implementing a turbulence model such as k-ε improve convergence or does it only have to do with capturing the turbulent effects themselves rather than helping with convergence?

Lastly, could the culprit be the mesh itself? Would modifying my code to work for unstructured meshes and thus being able to add more detail to BC's also improve it?

Anything else that could hinder convergence?
I am really confused on the convergence part since there seem to be so many things that can affect it. It also amazes me how people manage to converge more complicated problems such as flow around airfoils where the Reynolds number can hit the millions, with such high velocity and low viscosity.

Thanks!

It seems you have a lack in understanding that the steady flow assumption is valid only for a limited number of case. There is transition to unsteady solution when the Re number increases.
Using a turbulence model in RANS formulation (but the flow must be fully turbulent) means you search for convergence to a statistically steady solution. That is different from the laminar steady state for the local variables.

[pgcet1]

Originally Posted by panagiat

Hello!

I recently made a steady-state FVM Incompressible 2D Navier Stokes solver using the SIMPLE algorithm for a collocated cartesian orthogonal grid in C++.

As far as the discretization goes, for diffusion and pressure I am using central differencing and for convection I am using 1st order upwinding (for which I have read that does not have any conditions regarding stability as far as the Reynolds number goes). I am also using under-relaxation with values of 0.7 and 0.3 for velocity and pressure.

It seems to be working perfectly for some benchmark problems such as the lid-driven cavity, provided the reynolds number is not too high (not over 1000) in a 100x100 grid. Though it diverges for higher reynolds numbers and this happens to be the case for other problems as well such as pipe flow and flow against a circle (each problem seems to pose a different "limit" for Reynolds number in terms of convergence though no problem seems to be able to pass the 1000 Reynolds number mark). I am also noticing a sudden (maybe exponential?) increase in convergence time when that limit is approached until it doesn't converge anymore.

So, so my question is:
Are there any other convergence criteria I am missing?

As far as the solver selection, I know that the SIMPLE algorithm I am using makes a simplification regarding the velocity correction equations, which inherently makes it prone to divergence.
So would another solver improve the situation? (SIMPLER, SIMPLEC, PISO etc.)

As far as the discretization schemes, is it true that by introducing higher order schemes (even just for the reynolds numbers they would support regarding stability) increase convergence rate? From what I've read they can only increase the accuracy of the result but I could be mistaken.

I've also read that people use turbulence models at higher reynolds numbers where turbulence plays a bigger role. Would implementing a turbulence model such as k-ε improve convergence or does it only have to do with capturing the turbulent effects themselves rather than helping with convergence?

Lastly, could the culprit be the mesh itself? Would modifying my code to work for unstructured meshes and thus being able to add more detail to BC's also improve it?

Anything else that could hinder convergence?
I am really confused on the convergence part since there seem to be so many things that can affect it. It also amazes me how people manage to converge more complicated problems such as flow around airfoils where the Reynolds number can hit the millions, with such high velocity and low viscosity.

Thanks!

Try using a fully coupled solver instead of SIMPLE. You can go all the way to Re 10000 for the Lid Driven Cavity Case with no turbulence. Mesh do matter. Near wall clustering improves convergence.