Hi,

I'm trying to run a steady simulation on a transonic blade passage with air injection microtubes mounted on blade tip (CFX v11). I'm using SST model, high resolution and autotimescale (targetting E-5 s order of magnitude).

When I try imposing an uniform inlet boundary of 300 m/s at this microtubes I first get a mach warning (Notice: The maximum Mach number is 2.714E+00., for example) on the early iterations of my 64bit solver (around 10th~11th) after of which, I mean the very next iteration, then cpu goes overflow resulting in this kind of error:

ERROR #001100279 has occurred in subroutine ErrAction. | | Message: | | Floating point exception: Overflow

I tried enabling double precision on solver, but this let the solver survive only longer (34~35 iterations). History max residuals, in both cases, shows cpu strugling towards convergence and it doesn't manage to lower the value of E-1 max residual. Imposing physical timescale to higher values (up to E-2) and switching to upwind resolution have any effect in solution.

The strange thing is that i get an -easy- run when imposing a 150 m/s value instead of 300 m/s. I'm not an expert in CFD, but I guess this can exclude a mesh problem. Could the turbulence model be obsolete?

What do you think about this problem? I will be raising the inlet velocity at higher values, so I need to solve this issue.

Thanks for the attention, ReeKo

by increasing the timescale(physical timescale) you will be incresing you problem.

i would suggest you to decrease the timescale and run it or as your case with 150m/s velocity is going well, so run the case with 150m/s and increase the velocity value in steps to 300m/s this may help you.

Hi,

Does the increase in velocity cause some regions to go transonic? This significantly increases the difficulty of convergence and may be the difference between the slower run converging nicely and the faster run not.

A trick to try is to try ramping up the velocity from the easy slower case to the tricky faster over 100-200 iterations.

Glenn Horrocks

Thank you all for answers,

I tried as you suggest to raise velocity step by step by 10 m/s but I experience a threshold value above which residuals starts fluctuating. Then I realized the autotimescale wasn't hitting at the problem, the latter being "very" unsteady. So I tried to set the same steady simulation to unsteady, imposing a timestep and letting it run for some time only to have some information on flow field frequency. It seems the actual timeorder of unsteadiness is E-7, compared to somethingE-5 used by auto. So I continued my steady with that scale and noticed fluctuations resolved into smooth curves. But, still remaining smooth and waiting for hundreds iterations, residuals don't converge to my goal (max E-4).

I'm cursing the fact I don't have a solid knowledge on numerics, and because of this I refer to you with better hope.

Glenn, that tip region is dreadfully complex in term of physics, compressible effects are only the first feature. So i ask myself: - Is SST turbulence model good for this problem? - Is mesh refinement only solution to my problem?

Hi,

In general SST is a good choice but some times the other models are better. Unless you have a specific reason to use something else stick with SST.

Mesh refinement is likely to make convergence even harder.

Here are some tips: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Glenn Horrocks

Thank you for answers and patience,

I've already seen that link and was to me useful in fixing some problem. But now about this problem I don't really get a solution.

I started a transient with adaptive timestepping, with no better result: at around 8th time step I get a warning about the max mach number, that grows up till 11th resulting in an overflow (divide by zero,??). I also notice that loop by loop residuals rate have a chaotic trend and over the timesteps they start meanly to diverge until overflow.

What the hell is going on?

Some thoughts:

Maybe the correct timestep to solve non linearities is lower then auto and the residual of 5E-4 MAX is foolishly high for a first run, maybe would be reached in a next refined transient run. So the solver jumps to next timestep having not reached criteria jet thus having a solution timestep by timestep "even and even worse" and prorgessively hard to converge.

Are this thoughts right in some way? Would someone suggest me a proper first-run residual criteria for a transient?

yes you are absolutely right, could you tell what are your courant number(max and rms) value for your transient run, because it gives an indication of your timestep, whether it is too large for your simulation and needs to be corrected.

Sure, since timestep are few here is the historic:

TIME STEP = 1 SIMULATION TIME = 1.0000E-08 CPU SECONDS = 6.108E+01

Timestep | RMS Courant Number | Max Courant Number

1.0000E-08 | 0.11 | 2.98

//////// TIME STEP = 2 SIMULATION TIME = 1.8000E-08 CPU SECONDS = 2.133E+03

Adaptive Timestepping Information Direction | Ratio | Last Value | Next Value | RMS Co | Max Co Decreasing

| 0.800 | 1.0000E-08 | 8.0000E-09 | 0.11 | 2.96

//////// TIME STEP = 3 SIMULATION TIME = 2.4400E-08 CPU SECONDS = 4.004E+03

Direction | Ratio | Last Value | Next Value | RMS Co | Max Co

Decreasing | 0.800 | 8.0000E-09 | 6.4000E-09 | 0.09 | 2.37

/////// TIME STEP = 4 SIMULATION TIME = 2.9520E-08 CPU SECONDS = 5.851E+03

Direction | Ratio | Last Value | Next Value | RMS Co | Max Co

Decreasing | 0.800 | 6.4000E-09 | 5.1200E-09 | 0.07 | 1.90

//////// TIME STEP = 5 SIMULATION TIME = 3.3616E-08 CPU SECONDS = 7.695E+03

Direction | Ratio | Last Value | Next Value | RMS Co | Max Co

Decreasing | 0.800 | 5.1200E-09 | 4.0960E-09 | 0.06 | 1.52

///////// TIME STEP = 6 SIMULATION TIME = 3.6893E-08 CPU SECONDS = 9.545E+03

Direction | Ratio | Last Value | Next Value | RMS Co | Max Co

Decreasing | 0.800 | 4.0960E-09 | 3.2768E-09 | 0.05 | 1.21

/////// TIME STEP = 7 SIMULATION TIME = 3.9514E-08 CPU SECONDS = 1.139E+04

Direction | Ratio | Last Value | Next Value | RMS Co | Max Co

Decreasing | 0.800 | 3.2768E-09 | 2.6214E-09 | 0.04 | 0.97

//////// TIME STEP = 8 SIMULATION TIME = 4.1611E-08 CPU SECONDS = 1.324E+04

Direction | Ratio | Last Value | Next Value | RMS Co | Max Co

Decreasing | 0.800 | 2.6214E-09 | 2.0972E-09 | 0.03 | 0.78

Notice: The maximum Mach number is 2.968E+00.

/////// TIME STEP = 9 SIMULATION TIME = 4.3289E-08 CPU SECONDS = 1.509E+04

Direction | Ratio | Last Value | Next Value | RMS Co | Max Co

Decreasing | 0.800 | 2.0972E-09 | 1.6777E-09 | 0.02 | 3.94

Notice: The maximum Mach number is 5.995E+00.

/////// TIME STEP = 10 SIMULATION TIME = 4.4631E-08 CPU SECONDS = 1.694E+04

Direction | Ratio | Last Value | Next Value | RMS Co | Max Co

Decreasing | 0.800 | 1.6777E-09 | 1.3422E-09 | 0.02 | 0.89

Notice: The maximum Mach number is 2.047E+01.

/////// TIME STEP = 11 SIMULATION TIME = 4.5705E-08 CPU SECONDS = 1.882E+04

Direction | Ratio | Last Value | Next Value | RMS Co | Max Co

Decreasing | 0.800 | 1.3422E-09 | 1.0737E-09 | 0.01 | 0.52

Notice: The maximum Mach number is 4.910E+01.

//////// TIME STEP = 12 SIMULATION TIME = 4.6705E-08 CPU SECONDS = 2.070E+04

Direction | Ratio | Last Value | Next Value | RMS Co | Max Co

Decreasing | 0.931 | 1.0737E-09 | 1.0000E-09 | 103.13 | 999.99

ERROR #001100279 has occurred in subroutine ErrAction.

Message:

Floating point exception: Divide by zero

If you can answer and find the proble with that, I would be ver grateful. Your help is gold for me.

your max courant number is quite normal before the last time step, so i think the time step you have used is OK

so my advice is to look at the mesh quality, try to take a backup file at a time step just before you divergence and look at the location where you have these high values...and possibly think of the problem there..may be mesh, or setup of your problem..

Important new feature discovered: I have results from a timestep in which warning said max mach number was 3. I've post-processed by creating an isovolume with mach above 1.7: here you can see the difference of the same plot in the baseline (former) and with actuation configuration (latter)

http://img293.imageshack.us/my.php?i...aselinekb8.jpg (baseline)

http://img389.imageshack.us/my.php?image=vortexju8.jpg (actuation)

Even if the "max mach number" warning i get just before overflowing is 50~60, i can clearly deduce from this results the tip clearance vortex (a common feature of secondary flows in compressors) is the object of my problem. In the baseline no volume of flow field goes up 1.8 mach, while in the actuated diverged the core reaches mach 3 and high speed region has a lenght of 1/3 chord

Now, if you tell me that RMS Courant is ok, I conclude I need a mesh refinement in that zone.

Hi,

The courant number only gives you a guide for timestep size. You should do a timestep sensitivity study to determine the true timestep required for the accuracy you need.

Glenn Horrocks