Two questions:

(1) I'm running a series of simulations on an air inlet at M=0.2 to M=0.9. The free stream total pressure is one of the variables I need in the end. No problem to do this, what interests me is the accuracy (within 0.01%) I get, when I compare it to the total pressure from compressible flow theory. My question is whether the code is just damn good (:->) at solving the navier stokes equations, or if it just solves the same equations as I did to get the total pressures, in which case I shouldn't be so impressed, just happy it can multiply correctly!

(2) At M=0.9 I have a quite substantial region of supersonic flow through which the inlet streamtube flows. My problem is that I do not exactly get mass flow conservation through the inlet for this case: The mass flow in a plane just inside the inlet is different from the mass flow boundary I specified at the exit of the inlet duct. Would this be because of the supersonic flow upstream causing difficulties with the solver? I know transonic flow is problematic because the nature of the equations change, I just need a "reason" for this . I have specified max continuity loop = 2, which kept the simulation stable; residuals have become stable so it won't converge any more, and the global imbalance in mass flow is 0.007% which I feel is more than acceptable for the problem. Any ideas?

Hi Lowrens,

ANS (1): You are probably solving the same equations as the code (unless you have some other compressible flow equations no-one has heard of) AND it is damn good . If you are curious, all the equations are outlined in the Solver section of the theory doc.

(2) Are you calculating this mass flow in CFX-Post or elsewhere? The global conservation looks good but what residual have you converged to?

Regards, Robin

1. Nah, same old equations as everybody else... and I got the reference to the total pressure calculation in the docs an hour or two after I posted the question!

2. At that specific plane I calculate the mass flow using a matlab program I wrote, but it's been validated thoroughly and it gives the same values as Post does. Mass converged to just above 1e-5 before going stable. All residuals oscillate rapidly, which I attribute to the huge amount of separation. All momentum residuals oscillated in around approx 5e-4... What bugs me is that my simulations at lower mach numbers with same amount of separation and same ``shaky'' convergence don't have the error in continuity??

Hi Louwrens,

The problem is your Matlab program cannot get the same mass flows as Post does because Post uses the actual IP mass flows from the solver. Mass flows are calculated at the integration points and it is more complicated than simply interpolating values to the faces (particularly with compressible flows). Unless your Matlab code discretizes the space exactly the same way as the solver, you will not get exact mass flow.

CFX-Post has been designed to use the exact same data structures as the solver, therefore calculations in Post are exact. The same cannot be said for third party applications.

I suggest doing these calculations within Post and you will find that there is no error in continuity.

Regards, Robin

Hi Robin

My program uses the variable values at the geometric positions exported from post. This then goes into a mesher again to get a triangular mesh on the surface and the values on the plane is approximated by summing the average of the values at the corners of each triangle. It works very well, normally getting to within 0.5% of the values given by Post. I got the right answers for flight speeds up to M=0.8, its just my M=0.9 simulation that gives problems. I checked with Post, and I also don't get the same mass flow higher up in the duct than what I applied at the exit.

Moral of a long story: I don't get continuity at M=0.9 and I'm not quite sure why...

L

Louwrens,

That's very odd. If the solution is converged, mass will be conserved everywhere. I suggest sending your res file to your support rep for a closer look.

Robin

It doesn't matter what your matlab program does, whatever it does it is not consistent with what is done in the flow solver. The mass flows used by CFX-Post are written by the flow solver and the values of those mass flows specifically depend on the details of the discretisation.

However, that being said, let me ask the following:

1) What is your inlet P-mass flow?

2) What is your outlet P-mass flow? (This should exactly equal your specified value if you are using a m-dot specified outlet)

3) What is the MAX P-Mass residual in the solution you call converged?

4) What is the RMS P-Mass residual in the solution you call converged?

5) It sounds like the solution has stalled, for whatever reason. So, where exactly does the MAX P-Mass residaul occur? Is it in a separation region? Is it near some bad grid? etc...

6) Did you try setting "relax mass" to something less than the default?

Neale

Hi All,

A similar problem involving total pressure and transonic flows. Have anyone of your faced problems with conservation of total pressure at stagnation points with reference to free stream total pr? I'm using CFX-5 with an unstructured mesh.

I've also been facing problems with the exact shock location, I've used pressure based mesh adaptation.

Thanks, Danie

Hi Danie,

Exactly what kind of problem are you having at the stagnation poiint?

It is possible for the total pressure to rise at a stagnation point due to visous effects. As you approach a stagnation point, the shear stress on either side of a fluid element are in the same direction, resulting in additional force on that element and a rise in total pressure. The size of the region where this occurs will diminish with increased mesh resolution, however the effect is physically realistic.

Regards, Robin

Hi,

it is not unusual to have an approximate interpolation scheme (which is what you must have as your stuff in Matlab) which works ok for some flows and then falls apart for others.

Basically, your interpolations seem to work for smooth variations in the solution field for density and velocity but not as the variations increase (as they often do with increasing Mach number!) Look at it this way, if the solution is phi=constant then any reasonable interpolation will work and give the exact answer. If phi varied linearly then a linear interpolation will yield the exact value. As the solution variation in space becomes more complex there is an error which is proportional to some power of the discrete length scale and some higher order derrivative of the solution (depending upon the order of the interpolation and the order of the surface inegration method chosen). Hence at higher Ma it falls apart!

There is an excellent discussion on this issue in chapter 4 of Ferziger and Peric's book "Computational Methods for Fluid Dynamics"

Regards,

BAK_FLOW