Direct stability analysis problem
Hello, I have problem with direct stability analysis of flow around NACA airfoil. In my case, I'm using mesh with rectangular elemennts generated in Icem, and than exported as Nastran file to Gmsh. Main proble with my case is connected with "CG iterations made = 5001 using tolerance of 1e-09 (error = 0.0231643, rhs_mag = 1045.02)". I'was trying to identify problem but with no positive results. Which is quite interesting problem occurs only with parallel work using mpi. In serial mode solver starts normaly. Maybe some of you could help me find problem. Best regards, Witold
Hi, The error you are getting means that the linear solver failed to converge within a prescribed (hard coded maximum) number of iterations. 1. You might to give a try to the ARPACK driver (serial only) as it sometimes converges better. 2. I had more luck with the Coupled solver than with the time stepping. 3. Do you know anything about the instability you seek? Like approximate growth and frequency? You could use this info to improve convergence of the coupled solver. 4. I see you are not providing any initial conditions in your session files. Which probably means that those are random. I had a similar problem and Spencer has pointed out that this random initial conditions together with not satisfying the LBB conditions (same expansion for velocity and pressure) will lead to wrong, non physical solutions. To address that try a smoother initial condition (some sin and cos?), or an expansion like: <EXPANSIONS> <E COMPOSITE="C[36]" TYPE="MODIFIED" NUMMODES="9" FIELDS="u,v" /> <E COMPOSITE="C[36]" TYPE="MODIFIEDQUADPLUS2" NUMMODES="7" FIELDS="p" /> </EXPANSIONS> 5. You seem to be using a rather low order expansion, I understand the problem gets to be big. Best, Stan Gepner On 08/10/2017 01:11 PM, wkrusz wrote:
Hello, I have problem with direct stability analysis of flow around NACA airfoil. In my case, I'm using mesh with rectangular elemennts generated in Icem, and than exported as Nastran file to Gmsh. Main proble with my case is connected with "CG iterations made = 5001 using tolerance of 1e-09 (error = 0.0231643, rhs_mag = 1045.02)". I'was trying to identify problem but with no positive results. Which is quite interesting problem occurs only with parallel work using mpi. In serial mode solver starts normaly. Maybe some of you could help me find problem. Best regards, Witold
_______________________________________________ Nektar-users mailing list Nektar-users@imperial.ac.uk https://mailman.ic.ac.uk/mailman/listinfo/nektar-users
Hi As Stan has said you are hitting a convergence issue with the iterative solver. It may be that you will need to use a better preconditioner than the default diagonal one for this type of simulation. Your mesh is very refined for a p-type method and so you may also wish to try a less coarse mesh and perhaps a lower Re to initially see how to set things up. Finally I had a quick look at your base flow and it did not seem right. The u-velocity varies from -6 to 12 so quite possibly something is going wrong in this part of the setup too. Cheers, Spencer. [cid:C0081D23-0868-44B2-98D1-58FF6351D90F] On 10 Aug 2017, at 18:18, Stanisław Gepner <sgepner@meil.pw.edu.pl<mailto:sgepner@meil.pw.edu.pl>> wrote: Hi, The error you are getting means that the linear solver failed to converge within a prescribed (hard coded maximum) number of iterations. 1. You might to give a try to the ARPACK driver (serial only) as it sometimes converges better. 2. I had more luck with the Coupled solver than with the time stepping. 3. Do you know anything about the instability you seek? Like approximate growth and frequency? You could use this info to improve convergence of the coupled solver. 4. I see you are not providing any initial conditions in your session files. Which probably means that those are random. I had a similar problem and Spencer has pointed out that this random initial conditions together with not satisfying the LBB conditions (same expansion for velocity and pressure) will lead to wrong, non physical solutions. To address that try a smoother initial condition (some sin and cos?), or an expansion like: <EXPANSIONS> <E COMPOSITE="C[36]" TYPE="MODIFIED" NUMMODES="9" FIELDS="u,v" /> <E COMPOSITE="C[36]" TYPE="MODIFIEDQUADPLUS2" NUMMODES="7" FIELDS="p" /> </EXPANSIONS> 5. You seem to be using a rather low order expansion, I understand the problem gets to be big. Best, Stan Gepner On 08/10/2017 01:11 PM, wkrusz wrote: Hello, I have problem with direct stability analysis of flow around NACA airfoil. In my case, I'm using mesh with rectangular elemennts generated in Icem, and than exported as Nastran file to Gmsh. Main proble with my case is connected with "CG iterations made = 5001 using tolerance of 1e-09 (error = 0.0231643, rhs_mag = 1045.02)". I'was trying to identify problem but with no positive results. Which is quite interesting problem occurs only with parallel work using mpi. In serial mode solver starts normaly. Maybe some of you could help me find problem. Best regards, Witold _______________________________________________ Nektar-users mailing list Nektar-users@imperial.ac.uk<mailto:Nektar-users@imperial.ac.uk> https://mailman.ic.ac.uk/mailman/listinfo/nektar-users _______________________________________________ Nektar-users mailing list Nektar-users@imperial.ac.uk<mailto:Nektar-users@imperial.ac.uk> https://mailman.ic.ac.uk/mailman/listinfo/nektar-users Spencer Sherwin McLaren Racing/Royal Academy of Engineering Research Chair, Professor of Computational Fluid Mechanics, Department of Aeronautics, Imperial College London South Kensington Campus London SW7 2AZ s.sherwin@imperial.ac.uk<mailto:s.sherwin@imperial.ac.uk> +44 (0) 20 759 45052
participants (3)
-
Sherwin, Spencer J
-
Stanisław Gepner
-
wkrusz