[alinik]

Hi,

I am modeling flow inside a domain that is composed of several domains. I use Frozen-rotor interface type for some reason and I receive this error message:

Details of error:-
----------------
Error detected by routine MAKLNK
COLDNM = MAXCLOOP CNEWNM = MAXSTEP
CRESLT = OLD
+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine MEMERR |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+
the simulation is steady state and the interface's sides are fully overlapping
Any idea on that?

[Opaque]

What release version are you running ? R15.0 ?

Are you running a model with mesh deformation/motion ?

Would you mind posting the SOLVER CONTROL section of your setup ?

[alinik]

Yes I am using R 15 and no I do not have any mesh motion or mesh deformation. Although one of the domains has motion but the interface type is Frozen Rotor and simulation type is steady state.

[alinik]

Here is the solver control setup:

p, li { white-space: pre-wrap; } FLOW: Flow Analysis 1
&replace SOLVER CONTROL:
Turbulence Numerics = High Resolution
ADVECTION SCHEME:
Option = High Resolution
END
CONVERGENCE CONTROL:
Maximum Number of Iterations = 100
Minimum Number of Iterations = 1
Physical Timescale = 0.002 [s]
Timescale Control = Physical Timescale
END
CONVERGENCE CRITERIA:
Residual Target = 0.000001
Residual Type = RMS
END
DYNAMIC MODEL CONTROL:
Global Dynamic Model Control = Yes
END
EQUATION CLASS: continuity
ADVECTION SCHEME:
Option = Upwind
END
END
EQUATION CLASS: ke
ADVECTION SCHEME:
Option = High Resolution
END
END
EQUATION CLASS: momentum
ADVECTION SCHEME:
Option = Upwind
END
END
EQUATION CLASS: tef
ADVECTION SCHEME:
Option = High Resolution
END
END
INTERSECTION CONTROL:
Option = Direct
Permit No Intersection = On
END
END
END

[Opaque]

Try removing all the EQUATION CLASS stuff, and see what happens.

On a separate topic, would mind sharing the goal of reducing accuracy of the advection scheme for some equations or not others ? I guess most of us would go for the most accurate scheme, and only reduce it for an equation where such level of accuracy create robustness/convergence problems.

Barring robustness issues, changing accuracy between strongly inter-related equations may create all sort of issues that are not easy to detect later on.

[alinik]

I did that but the same error occurs. The reason for different equation class is that some parameters tend to converge later than they should be and thus I need to sacrifice accuracy in order to have convergence. This problem since it has more than one domain is hard to get a solution.

[alinik]

It seems that the problem was mesh motion. It has to be set to "none" instead of "regions of motion specified".
I had it set to the latter because one of the domains is moving in real world. but in F/R case both domains have to be stationary

[Opaque]

My advice is to read the documentation to understand the differences between domain motion, and mesh deformation. Why of their existence, how they interact and when they should be activated.

Earlier, you said you did not have mesh motion set.

If your equations are not converging, you must look at other alternatives (heavily discussed in this forum). However, reducing the accuracy of the two main equations: momentum and energy, is definitely not one of them unless you are not interested very much about the final solution.