|
[Sponsors] |
August 28, 2014, 14:33 |
Error detected by routine MAKLNK
|
#1 |
Senior Member
ali
Join Date: Oct 2009
Posts: 318
Rep Power: 17 |
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? |
|
August 28, 2014, 15:39 |
|
#2 |
Senior Member
Join Date: Jun 2009
Posts: 1,799
Rep Power: 31 |
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 ? |
|
August 28, 2014, 17:26 |
|
#3 |
Senior Member
ali
Join Date: Oct 2009
Posts: 318
Rep Power: 17 |
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.
|
|
August 28, 2014, 17:26 |
|
#4 |
Senior Member
ali
Join Date: Oct 2009
Posts: 318
Rep Power: 17 |
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 |
|
August 28, 2014, 18:00 |
|
#5 |
Senior Member
Join Date: Jun 2009
Posts: 1,799
Rep Power: 31 |
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. |
|
August 29, 2014, 11:36 |
|
#6 |
Senior Member
ali
Join Date: Oct 2009
Posts: 318
Rep Power: 17 |
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.
|
|
August 29, 2014, 11:57 |
|
#7 |
Senior Member
ali
Join Date: Oct 2009
Posts: 318
Rep Power: 17 |
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 |
|
August 29, 2014, 14:13 |
|
#8 |
Senior Member
Join Date: Jun 2009
Posts: 1,799
Rep Power: 31 |
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. |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
user subroutine error | CFDUSER | CFX | 2 | December 9, 2006 06:31 |
CFX 10 User Routine NOT in Fortran | Andre | CFX | 14 | August 8, 2006 23:03 |
user defined function | cfduser | CFX | 0 | April 29, 2006 10:58 |
CFX 10 User Sub Routine | Claudia | CFX | 6 | February 15, 2006 08:32 |
FORTRAN Routine - variable passing | Malcolm | CFX | 1 | August 11, 2005 18:51 |