[Akshay]

Hi guys

I was simulating a 2 fluid interface problem and at a particular instant there is some splashing that occurs. The mesh is clean(aspect and other parameters) and I have also increased the itmax to 250. The simulation runs fine and the results look good. But I want to understand the impact of the pressure iteration not converging and in addition to that, the Epsi and Max Resi somtimes vary by a huge factor. I'm assuming this will lead to inaccuracy in my simulations but how do I quantify this? Below is the log.. You can see the epsi is 4.49 and max.resid is 17.59 ... what does this correspond to in terms of accuracy?

LOG

pressure iteration did not converge in itmax= 250 iterations
at time= 2.19336E+00 cycle= 21954 iter= 250 delt= 7.73638E-06
epsi= 4.491E+00 maximum residual= 1.759E+01 at i= 120 j= 79 k= 24 block= 1
restarting cycle with smaller time-step size
present relaxation factor omega= 8.778E-01
present time-step size delt= 7.736E-06
pressure iteration did not converge in itmax= 250 iterations
at time= 2.19338E+00 cycle= 21959 iter= 250 delt= 4.93690E-06
epsi= 5.732E+00 maximum residual= 2.238E+01 at i= 47 j= 209 k= 36 block= 1
restarting cycle with smaller time-step size
present relaxation factor omega= 8.778E-01
present time-step size delt= 4.937E-06
pressure iteration did not converge in itmax= 250 iterations
at time= 2.19370E+00 cycle= 22000 iter= 250 delt= 1.82467E-05
epsi= 5.206E+00 maximum residual= 2.550E+01 at i= 95 j= 155 k= 71 block= 1

[JBurnham]

If the iteration failure keeps occurring, it will eventually make the time step so small that it crashes the simulation (dt < dtmin). Usually this indicates a problem with the mesh, the geometry, or initial conditions/boundary conditions. I've listed the most common problems below. These are probably about 80% - 90% of the reason for getting a lot of error messages. If you have a few error messages in a row and then they stop, okay, it's probably fine. If you have a lot in a row and they continue throughout the simulation, check carefully for the causes below. If that doesn't help, consider calling Flow Science or your local distributor and asking about a support contract.

Mesh problems:
1) Cell size aspect ratio too large (1:1:1 is ideal, 3:1 should be max),
2) Too much size stretching from one cell to the next (1:1 ideal, 1:1.25 max),
3) Poor gridline matching between cells of adjacent mesh blocks (gridlines should match perfectly to minimize interpolation uncertainty),
4) Poor cell size ratio between adjacent mesh blocks (should be either 1:1 or 2:1),
5) Poor flow resolution (thinnest flow region must be resolved by at least 4 cells for stability, 10 - 20 cells for accurate velocity profile & flow rate). Hint: start w/ 4 or 5 cells to prove the case runs, then refine the grid for accuracy.

Geometry problems:
1) Sliver cells (cells w/ very small open volume & very large open face areas),
2) Bad .stl files (reversed facets, holes, etc). FLOW-3D doesn't check .stl files 3) so use netfabb Basic before you put the file in the simulation,
4) Poor solid resolution (need at least 3 or 4 cells across the thinnest piece of geometry).

Initial Condition problems:
1) Initial conditions don't match boundary conditions.
2) Initial conditions cause a lot of splashing early in the simulation.
3) Initial conditions are unrealistic or incorrect.

Boundary Condition problems:
1) Boundary conditions don't match initial conditions.
2) Boundary conditions cause a lot of splashing.
3) Boundary conditions are unrealistic or incorrect.

[Akshay]

Hi Jeff

Thanks for the detailed reply. But I still did not find what I'm looking for. I do understand all the points listed by you and it is all taken care of. In my case, I have splashing. Now it is understandable that the pressure iteration works extra hard to converge during the splashing phase. My question is during these iterations(as shown in my log) , the Epsi and Max Resid are very different. I believe this difference results in some level of inaccuracy. I want to understand this concept and how do I quantify this inaccuracy?

Akshay

[JBurnham]

The residual is the difference between the LHS (left hand side) and RHS (right hand side) of the momentum conservation equations. The pressure term in those equations is implicit and must be solved for iteratively.

Epsi is the acceptable tolerance for LHS and RHS disagreement. FLOW-3D selects Epsi dynamically based on the pressure solver that's being used and other properties of the flow. You can multiply FLOW-3D's guess with EPSADJ (default = 1), like 0.001 for a 1000x tighter convergence criteria.

Interpreting the inaccuracy is not possible - you must compare CFD results to an analytical solution or experiment. If you use an experiment, you must account for uncertainty in the experimental results and measurements of input properties like viscosity and density.

You can only say that when the ratio resid/epsi is larger than 1, the pressure solver has not converged to the expected tolerance, and therefore more uncertainty exists in the pressure solution than the dynamically-selected epsi intended. The extra uncertainty may result in a negligible or large loss of accuracy in the failure cell, and the effects on the global field may or may not be noticeable.

To illustrate the idea, it is possible to have simulations that are very inaccurate (or unstable) even when res/epsi is < 1. It is also possible to have simulations where res/epsi > 1 that are extremely accurate and stable. It all depends on the size of epsi, which FLOW-3D selects dynamically. In my experience, FLOW-3D is almost always very reliable in picking a good epsi, so you almost never need to worry about the size of epsi.

In general if you have some isolated convergence failures, the effect on the overall flow accuracy can be expected to be very small or non-existent. If you have pressure convergence failures that repeat very regularly through the whole simulation, then the effects are more likely to be noticeable or even severe. Again, the only way to know for sure is to test against something known.

[Akshay]

That couldn't have been answered in a better way Thanks a lot Jeff!!