I programed 3D NS code with the SIMPLEC method. It based on pressure. I want to calculate compressible flow field in turbomachinery with this code, but I can't get a convergent solution any way. So I doubt if this method is suitable for turbomachinery problem, or is there some problem should be noted? any advice would be appreciated.

M < 0.5 : No problems with standard incompressible approach plus gas law.

0.5 < M < 2 : Introduce some transportive mechanism into the pressure. Generally need time step approaching the Courant limit because of strong coupling of segragated variables (perhaps 10 times bigger but it obviously depends on the flow). The choice of u or rho*u as solution variable will also influence the set of problems one ends up addressing.

M > 2 : Serious problems. The physics tends to defeat the approach in an analagous manner to running a standard compressible code at low speeds.

I have a question. Since your flow is compressible, why do you use a projection method (simplec) which goal is to calculate a divergence free flow?

Isn't it better to use a complete set of equations (mass, mouvement, energy + state equation) to solve the flow?

I think we may be at cross purposes. lhb is not going to get very far without solving a complete set of equations in the compressible regime. I had implicitly assumed that this was the case and was addressing the difference between solving a non-transportive equation for pressure (SIMPLEC) or a transportive equation for density. I was trying to indicate that subject to "retarding" the pressure a pressure based scheme can be pushed up to about M=2 before things fall apart which makes it suitable for a lot of turbomachinery applications.

We may be further at cross purposes if your posting was not meant for me?

Regards.

hi,

the original SIMPLEC was'nt meant for compressible flows. The original authors (patankar and others) have extended pressure based methods to compressible flows. The additional terms that come up as result of compressible flows are density correction and use of schemes like CVS(Shyy et al), TVD (Lin-Lin). Many authors have extended SIMPLE class of methods for compressible flows. It seems to work ok. Let me know if u want to know more.

abhijit

Do you have any references? I would appreciate.

Regards

I have a couple of questions regarding the SIMPLE scheme and it's variants (SIMPLER, SIMPLEC etc.).

i) How large a CFL number can one use with these methods to retain accuracy.

ii) You prescribe the pressure values (Dirchlet BC) at the outflow and you use a Neumann condition at the inflow. How do you make sure that the Greens theorem (volume integral of the source term = surface area integral of the pressure gradient) is satisfied discretely while using these boundary conditions. I would think that if this discrete condition (resulting from the theorem) is not satisfied, there would be a problem with conserving mass.

>>> I have a couple of questions regarding the SIMPLE scheme and it's variants (SIMPLER, SIMPLEC etc.).

>>> i) How large a CFL number can one use with these methods to retain accuracy.

They are methods for solving a set of discretized equations. They have nothing to do with accuracy - that depends on the procedure used to generate the discretized equations.

>>> ii) You prescribe the pressure values (Dirchlet BC) at the outflow and you use a Neumann condition at the inflow.

Not normally. Usually Neumann conditions are used everywhere. However, if you choose to fix the pressure at the exit then you must loosen the boundary conditions applied to the velocity at the exit. For example, zero gradient and allowing the mass flow to float.

>>> How do you make sure that the Greens theorem (volume integral of the source term = surface area integral of the pressure gradient) is satisfied discretely while using these boundary conditions.

Many schemes would not necessarily difference the pressure gradient term to conserve this quantity. Other discrete quantities may be considered more desirable (you cannot conserve everything discretely). However, if you want to then normal cell boundary face cancellation will ensure it occurs if you evaluate the pressure gradient in strong conservation form. Why do you think it might be a problem?

(On rereading I am confused. I had assumed you were referring to a force balance (your RHS) but guess your LHS is referring to a mass balance? Mass balances by ensuring cell face cancellation of mass flux at the cell faces in most schemes).

> I would think that if this discrete condition (resulting from the theorem) is not satisfied, there would be a problem with conserving mass.

There would be a force imbalance but not a mass imbalance - this depends on the velocity components. The most common form of pressure influencing mass balance is collocated schemes mixing pressure smoothing terms and mass flux terms.

There certainly would be a force imbalance but the primary problem is the mass balance. This is because the pressure updating is the step that couples the momentum conservation with the mass conservation (i.e., the velocity component prior to pressure update do not satisfy continuity).

E.g. : If you solve the Poisson equation with some arbitrary BC, the velocity field would be divergence-free in the interior. That does not ensure mass conservation. An additional constraint is required at the boundaries (I am not fully sure but it is "normal gradient of divergence of velocity = 0"). This additional condition is equivalent to the Greens theorem I had mentioned.

hi sebastian,

please see following 1.Patankar et.al "Pres. based calculation procedure for flow at all speeds in arbitary configurations". AIAA Journal Vol 27 no 9 pp 1167-1174. 1989

2. Peric et.al "A Collocated FV method for Prediction of Flow at all speeds Int. Jrnl for Num. Methods in Fluids Vol 16 pp 1029 - 1050 1993

3. A book called "Computtional Techniques for Complex and Interfacial Fluid Flow" by Wei Shyy. There is a entire chapetr on Pressure Based Methods. here u will find use of TVD like shock capturing methods used with Pressure Based Procedures.

bye bye abhijit

Hi kalyan,

There is no real limit on CFL (theoritically since these are essentially implict, to be more specific Semi Implicit methods) but i hav found for Mach 1.2 CFL of 0.7-0.8 works with a strongly implicit solver like ADI. Regarding B.C yes u got to be careful. The B.C's differ for compressible and incompressible flows. In compressible flows i usually fix the exit static pressure. U can calculate the inlet static Temp from knowing the inlet Mach No. for Mach no 0.4 i was able to use under-relaxation with deltaT=1e30, the true CFL independence of Semi Implicit Class of Methods was found. For higher mach no u need false transients to stabilise the iterations. For Incompressible flows at inlet velocity and pressure hav to be specified and at exit either of Pres /Velocity needs to be specified and other variable calculated by solving the equations. Otherwise the div.(gradP) is not satisfied. see the reference for satisfactory interploation of pressure to satisfy the greens theorem.

"On Pres Boundary cond. for incomp NS Equns using Non Stag Grids" Cook etal, Num.Heat Transfer. Vol 13. pp 241 252 1988.

bye bye abhijit

thank u all for such a good discussion

(1). What is the Mach number of your problem? (2). Is your problem transonic at the exit? (3). Were you able to get a solution for any Mach number? What is the Reynolds number? turbulence model used? and the mesh size?

>>Peric et.al "A Collocated FV method for Prediction of Flow at all speeds Int. Jrnl for Num. Methods in Fluids Vol 16 pp 1029 - 1050 1993

I followed the method used in this paper, and calculated a subsonic flow field over a bump at Mach=0.5. But I couldn't get a symmetric pressure contours distribution like this paper presented, I tried many other commercial codes, all they couldn't get a very symmetric contours distribution. I guessed I gave some wrong conditions, but what they might be?

Thanks all discussions at here, and Sorry for my late response, for my ISP got wrong, I couldn't connect this site those days.
1). What is the Mach number of your problem? <2
2). Is your problem transonic at the exit? sometimes is
3). Were you able to get a solution for any Mach number? I have not tried very high Mach Number.
:What is the Reynolds number? turbulence model used? and the mesh size? By this time, I have only tested the invisid method.