TimeIntegrationMethod in 3D homogeneous case
******************* This email originates from outside Imperial. Do not click on links and attachments unless you recognise the sender. If you trust the sender, add them to your safe senders list https://spam.ic.ac.uk/SpamConsole/Senders.aspx to disable email stamping for this address. ******************* Hi All, I wish all of you are fine these days, I am running a 3D homogeneous case for a square cylinder, when I run the case at high Reynolds 2000 it keeps crashing, I tried *"SpectralVanishingViscosity"* it is working but it is filtering my field, what about using a different time integration method *"BDFImplicitOrder2" *instead of using *"IMEXOrder2"*, I think the two of them are 2nd order but using Implicit instead of Implicit explicit will not crash, but also I will keep CFL under 1 to be sure it is fine, even with this method i can go for higher CFL, my Reynolds is 2000 turbulent flow. Regards, Reda UPC Barcelona +34 632 675 853
HI Reda, I would definitely try Dealiasing, at least in the Spectral Element plane. Also you need to make sure the outflow boundary condition is not causing problems and possibly require HOUTFLOW conditions at the outflow? The IMEXOrder2 is BDF2 on the linear viscous solve but we do not have a scheme to make the advection term implicit currently. It should certainly run at Re=2000. We have a number of runs for a circular cylinder at Re=3900. @Andrea: Could you forward a session file for that? Thanks, Spencer. Spencer Sherwin FREng, FRAeS Head of Aerodynamics Section, Director of Research Computing Service, Professor of Computational Fluid Mechanics, Department of Aeronautics, s.sherwin@imperial.ac.uk<mailto:s.sherwin@imperial.ac.uk> South Kensington Campus, Phone: +44 (0)20 7594 5052 Imperial College London, Fax: +44 (0)20 7594 1974 London, SW7 2AZ, UK http://www.imperial.ac.uk/people/s.sherwin/ On 14 Jun 2020, at 07:15, sgepner@meil.pw.edu.pl<mailto:sgepner@meil.pw.edu.pl> wrote: Hi Reda, Have you tried using Dealliasing? Pozdrawiam, Stanisław Gepner 14 cze 2020 01:32 Moto Light <redamansyhh@gmail.com<mailto:redamansyhh@gmail.com>> napisał(a): This email from redamansyhh@gmail.com<mailto:redamansyhh@gmail.com> originates from outside Imperial. Do not click on links and attachments unless you recognise the sender. If you trust the sender, add them to your safe senders list<https://spam.ic.ac.uk/SpamConsole/Senders.aspx> to disable email stamping for this address. Hi All, I wish all of you are fine these days, I am running a 3D homogeneous case for a square cylinder, when I run the case at high Reynolds 2000 it keeps crashing, I tried "SpectralVanishingViscosity" it is working but it is filtering my field, what about using a different time integration method "BDFImplicitOrder2" instead of using "IMEXOrder2", I think the two of them are 2nd order but using Implicit instead of Implicit explicit will not crash, but also I will keep CFL under 1 to be sure it is fine, even with this method i can go for higher CFL, my Reynolds is 2000 turbulent flow. Regards, Reda UPC Barcelona +34 632 675 853 _______________________________________________ Nektar-users mailing list Nektar-users@imperial.ac.uk<mailto:Nektar-users@imperial.ac.uk> https://mailman.ic.ac.uk/mailman/listinfo/nektar-users
Dear Reda, Attached is a session file with the numerical setup I would suggest to use (obviously change the expansion order to as you see fit). I would keep SVV turned on, and if the simulation still blows up increase diffusion coefficient and decrease cutoff ratio for the homogeneous direction. As Spencer was saying, you also have to be careful about the outflow - possibly coarsening the mesh in this region might help. As a diagnostic tool, I would suggest using the IO_CFLWriteFld parameter to understand where the instability is arising, which may give you hints on how to tackle the problem. Kind regards, Andrea Cassinelli PhD candidate Department of Aeronautics Imperial College London London SW7 2AZ Mob.: +44 (0)7956957642 On 14 Jun 2020, at 21:46, Sherwin, Spencer J <s.sherwin@imperial.ac.uk<mailto:s.sherwin@imperial.ac.uk>> wrote: HI Reda, I would definitely try Dealiasing, at least in the Spectral Element plane. Also you need to make sure the outflow boundary condition is not causing problems and possibly require HOUTFLOW conditions at the outflow? The IMEXOrder2 is BDF2 on the linear viscous solve but we do not have a scheme to make the advection term implicit currently. It should certainly run at Re=2000. We have a number of runs for a circular cylinder at Re=3900. @Andrea: Could you forward a session file for that? Thanks, Spencer. Spencer Sherwin FREng, FRAeS Head of Aerodynamics Section, Director of Research Computing Service, Professor of Computational Fluid Mechanics, Department of Aeronautics, s.sherwin@imperial.ac.uk<mailto:s.sherwin@imperial.ac.uk> South Kensington Campus, Phone: +44 (0)20 7594 5052 Imperial College London, Fax: +44 (0)20 7594 1974 London, SW7 2AZ, UK http://www.imperial.ac.uk/people/s.sherwin/ On 14 Jun 2020, at 07:15, sgepner@meil.pw.edu.pl<mailto:sgepner@meil.pw.edu.pl> wrote: Hi Reda, Have you tried using Dealliasing? Pozdrawiam, Stanisław Gepner 14 cze 2020 01:32 Moto Light <redamansyhh@gmail.com<mailto:redamansyhh@gmail.com>> napisał(a): This email from redamansyhh@gmail.com<mailto:redamansyhh@gmail.com> originates from outside Imperial. Do not click on links and attachments unless you recognise the sender. If you trust the sender, add them to your safe senders list<https://spam.ic.ac.uk/SpamConsole/Senders.aspx> to disable email stamping for this address. Hi All, I wish all of you are fine these days, I am running a 3D homogeneous case for a square cylinder, when I run the case at high Reynolds 2000 it keeps crashing, I tried "SpectralVanishingViscosity" it is working but it is filtering my field, what about using a different time integration method "BDFImplicitOrder2" instead of using "IMEXOrder2", I think the two of them are 2nd order but using Implicit instead of Implicit explicit will not crash, but also I will keep CFL under 1 to be sure it is fine, even with this method i can go for higher CFL, my Reynolds is 2000 turbulent flow. Regards, Reda UPC Barcelona +34 632 675 853 _______________________________________________ Nektar-users mailing list Nektar-users@imperial.ac.uk<mailto:Nektar-users@imperial.ac.uk> https://mailman.ic.ac.uk/mailman/listinfo/nektar-users
Hi Spencer. Thanks for replying I wish you a great day, could you check this is my settings and I will be very grateful if Andera can send me his file at 3900 to check the settings. but also what about using a different time integration method *"BDFImplicitOrder2" *instead of using *"IMEXOrder2" in *"TimeIntegrationMethod" , I think the two of them are 2nd order but using Implicit instead of Implicit explicit will not crash, also I will keep CFL under 1 to be sure it is fine, I tried *"SpectralVanishingViscosity"* it is working but it is filtering my field when I checked the velocity spectrum it was filtered. Also another case , please check my attachment file it has the same settings even with lower Reynolds at 400 using velocity ratio is crashing, for outlet BC i am already using *HOutflowa.* ----------------------------------------------------------------- <?xml version="1.0" encoding="UTF-8" ?> <NEKTAR> <EXPANSIONS> <E COMPOSITE="C[1]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 1 Domain inlet plate upper --> <E COMPOSITE="C[2]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 2 Domain inlet plate lower --> <E COMPOSITE="C[3]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- ****3 Domain square faces up down front meshs**** --> <E COMPOSITE="C[4]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 4 Domain upper domain lower in up stream --> <E COMPOSITE="C[5]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 5 Domain upper lower downstream --> <E COMPOSITE="C[6]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- ***6 Domain down stream back side square*** --> <E COMPOSITE="C[7]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 7 Domain down stream after square big one --> <E COMPOSITE="C[8]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 7 Domain down stream after square big one --> </EXPANSIONS> <CONDITIONS> <SOLVERINFO> * <I PROPERTY="SOLVERTYPE" VALUE="VelocityCorrectionScheme"/> <I PROPERTY="EQTYPE" VALUE="UnsteadyNavierStokes" /> <I PROPERTY="Projection" VALUE="Continuous" /> <I PROPERTY="EvolutionOperator" VALUE="Nonlinear" /> <I PROPERTY="TimeIntegrationMethod" VALUE="IMEXOrder2" /> <I PROPERTY="Driver" VALUE="Standard" /> <I PROPERTY="HOMOGENEOUS" VALUE="1D" /> <I PROPERTY="AdvectionForm" VALUE="SkewSymmetric" /> <I PROPERTY="Extrapolation" VALUE="Standard" /> <I PROPERTY="USEFFT" VALUE="FFTW" />* <!-- <I PROPERTY="DEALIASING" VALUE="ON" /> --> * <I PROPERTY="SPECTRALHPDEALIASING" VALUE="ON" />* <!-- <I PROPERTY="SpectralVanishingViscosity" VALUE="True" /> --> </SOLVERINFO> <PARAMETERS> <P> TimeStep = 0.0003 </P> <P> NumSteps = 550000 </P> <!-- 60sec --> <P> IO_CheckSteps = 5000 </P> <!-- 120 check files--> 520 <P> IO_InfoSteps = 10 </P> <P> Re = 2000 </P> <P> Kinvis = 1./Re </P> <P> IO_CFLSteps = 50 </P> <P> LZ = 10 </P> <!-- 3. * Fastest spanwise --> <P> HomModesZ = 16 </P> <!-- how many cells for Z direction --> </PARAMETERS> <VARIABLES> <V ID="0"> u </V> <V ID="1"> v </V> <V ID="2"> w </V> <V ID="3"> p </V> </VARIABLES> <BOUNDARYREGIONS> <B ID="0"> C[9] </B> <!-- Inlet1_upper --> <B ID="1"> C[10] </B> <!-- Inlet2_Lower --> <B ID="2"> C[11] </B> <!-- Splitter plate --> <B ID="3"> C[12] </B> <!-- Upper Boundary --> <B ID="4"> C[13] </B> <!-- Lower_Boundary --> <B ID="5"> C[14] </B> <!-- Outlet --> <B ID="6"> C[15] </B> <!-- Wall_square --> </BOUNDARYREGIONS> <BOUNDARYCONDITIONS> <REGION REF="0"> <!-- Inlet_upper --> <D VAR="u" VALUE="1" /> <D VAR="v" VALUE="0" /> <D VAR="w" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0"/> </REGION> <REGION REF="1"> <!-- Inlet_lower --> <D VAR="u" VALUE="1" /> <D VAR="v" VALUE="0" /> <D VAR="w" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0"/> </REGION> <REGION REF="2"> <!--Splitter plate --> <D VAR="u" VALUE="0" /> <D VAR="v" VALUE="0" /> <D VAR="w" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> </REGION> <REGION REF="3"> <!-- Upper Boundary --> <N VAR="u" USERDEFINEDTYPE="H" VALUE="0" /> <D VAR="v" VALUE="0" /> <N VAR="w" USERDEFINEDTYPE="H" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> </REGION> <REGION REF="4"> <!-- Lower_Boundary --> <N VAR="u" USERDEFINEDTYPE="H" VALUE="0" /> <D VAR="v" VALUE="0" /> <N VAR="w" USERDEFINEDTYPE="H" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> </REGION> <REGION REF="5"> <!-- Outlet --> * <N VAR="u" USERDEFINEDTYPE="HOutflow" VALUE="0" /> <N VAR="v" USERDEFINEDTYPE="HOutflow" VALUE="0" /> <N VAR="w" USERDEFINEDTYPE="HOutflow" VALUE="0" /> <D VAR="p" USERDEFINEDTYPE="HOutflow" VALUE="0" /> * </REGION> <REGION REF="6"> <!-- WallA_square --> <D VAR="u" VALUE="0" /> <D VAR="v" VALUE="0" /> <D VAR="w" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> </REGION> </BOUNDARYCONDITIONS> <!-- We initialise from pre-computed flow for speed --> <FUNCTION NAME="InitialConditions"> <E VAR="w" VALUE="awgn(1e-3)*cos(2*PI*z/LZ)" /> --> <!-- <F VAR="u,v,w,p" FILE="Start.chk" /> --> <!-- <E VAR="u,v,w,p" VALUE="0" /> --> <F VAR="u,v,p" FILE="Start2D.chk" /> <!-- start from 2D results --> </FUNCTION> <FUNCTION NAME="ExactSolution"> <E VAR="u" VALUE="0" /> <E VAR="v" VALUE="0" /> <E VAR="w" VALUE="0" /> <E VAR="p" VALUE="0" /> </FUNCTION> </CONDITIONS> ---------------------------------------------------------------------------------- Thanks, Regards On Sun, Jun 14, 2020 at 10:46 PM Sherwin, Spencer J < s.sherwin@imperial.ac.uk> wrote:
HI Reda,
I would definitely try Dealiasing, at least in the Spectral Element plane. Also you need to make sure the outflow boundary condition is not causing problems and possibly require HOUTFLOW conditions at the outflow?
The IMEXOrder2 is BDF2 on the linear viscous solve but we do not have a scheme to make the advection term implicit currently.
It should certainly run at Re=2000. We have a number of runs for a circular cylinder at Re=3900. @Andrea: Could you forward a session file for that?
Thanks, Spencer.
Spencer Sherwin FREng, FRAeS Head of Aerodynamics Section, Director of Research Computing Service, Professor of Computational Fluid Mechanics, Department of Aeronautics, s.sherwin@imperial.ac.uk South Kensington Campus, Phone: +44 (0)20 7594 5052 Imperial College London, Fax: +44 (0)20 7594 1974 London, SW7 2AZ, UK http://www.imperial.ac.uk/people/s.sherwin/
On 14 Jun 2020, at 07:15, sgepner@meil.pw.edu.pl wrote:
Hi Reda,
Have you tried using Dealliasing?
Pozdrawiam, Stanisław Gepner
14 cze 2020 01:32 Moto Light <redamansyhh@gmail.com> napisał(a):
This email from redamansyhh@gmail.com originates from outside Imperial. Do not click on links and attachments unless you recognise the sender. If you trust the sender, add them to your safe senders list <https://spam.ic.ac.uk/SpamConsole/Senders.aspx> to disable email stamping for this address.
Hi All,
I wish all of you are fine these days, I am running a 3D homogeneous case for a square cylinder, when I run the case at high Reynolds 2000 it keeps crashing, I tried *"SpectralVanishingViscosity"* it is working but it is filtering my field, what about using a different time integration method *"BDFImplicitOrder2" *instead of using *"IMEXOrder2"*, I think the two of them are 2nd order but using Implicit instead of Implicit explicit will not crash, but also I will keep CFL under 1 to be sure it is fine, even with this method i can go for higher CFL, my Reynolds is 2000 turbulent flow.
Regards, Reda UPC Barcelona +34 632 675 853
_______________________________________________ Nektar-users mailing list Nektar-users@imperial.ac.uk https://mailman.ic.ac.uk/mailman/listinfo/nektar-users
Sorry, this is the error i have always CG iterations made = 5001 using tolerance of 1e-09 (error = -nan, rhs_mag = -nan) Thanks On Sun, Jun 14, 2020 at 11:21 PM Moto Light <redamansyhh@gmail.com> wrote:
Hi Spencer.
Thanks for replying I wish you a great day, could you check this is my settings and I will be very grateful if Andera can send me his file at 3900 to check the settings. but also what about using a different time integration method *"BDFImplicitOrder2" *instead of using *"IMEXOrder2" in *"TimeIntegrationMethod" , I think the two of them are 2nd order but using Implicit instead of Implicit explicit will not crash, also I will keep CFL under 1 to be sure it is fine, I tried *"SpectralVanishingViscosity"* it is working but it is filtering my field when I checked the velocity spectrum it was filtered. Also another case , please check my attachment file it has the same settings even with lower Reynolds at 400 using velocity ratio is crashing, for outlet BC i am already using *HOutflowa.*
----------------------------------------------------------------- <?xml version="1.0" encoding="UTF-8" ?> <NEKTAR>
<EXPANSIONS> <E COMPOSITE="C[1]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 1 Domain inlet plate upper --> <E COMPOSITE="C[2]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 2 Domain inlet plate lower --> <E COMPOSITE="C[3]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- ****3 Domain square faces up down front meshs**** --> <E COMPOSITE="C[4]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 4 Domain upper domain lower in up stream --> <E COMPOSITE="C[5]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 5 Domain upper lower downstream --> <E COMPOSITE="C[6]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- ***6 Domain down stream back side square*** --> <E COMPOSITE="C[7]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 7 Domain down stream after square big one --> <E COMPOSITE="C[8]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 7 Domain down stream after square big one -->
</EXPANSIONS> <CONDITIONS> <SOLVERINFO>
* <I PROPERTY="SOLVERTYPE" VALUE="VelocityCorrectionScheme"/> <I PROPERTY="EQTYPE" VALUE="UnsteadyNavierStokes" /> <I PROPERTY="Projection" VALUE="Continuous" /> <I PROPERTY="EvolutionOperator" VALUE="Nonlinear" /> <I PROPERTY="TimeIntegrationMethod" VALUE="IMEXOrder2" /> <I PROPERTY="Driver" VALUE="Standard" /> <I PROPERTY="HOMOGENEOUS" VALUE="1D" /> <I PROPERTY="AdvectionForm" VALUE="SkewSymmetric" /> <I PROPERTY="Extrapolation" VALUE="Standard" /> <I PROPERTY="USEFFT" VALUE="FFTW" />* <!-- <I PROPERTY="DEALIASING" VALUE="ON" /> --> * <I PROPERTY="SPECTRALHPDEALIASING" VALUE="ON" />*
<!-- <I PROPERTY="SpectralVanishingViscosity" VALUE="True" /> -->
</SOLVERINFO>
<PARAMETERS> <P> TimeStep = 0.0003 </P> <P> NumSteps = 550000 </P> <!-- 60sec --> <P> IO_CheckSteps = 5000 </P> <!-- 120 check files--> 520 <P> IO_InfoSteps = 10 </P> <P> Re = 2000 </P> <P> Kinvis = 1./Re </P> <P> IO_CFLSteps = 50 </P> <P> LZ = 10 </P> <!-- 3. * Fastest spanwise --> <P> HomModesZ = 16 </P> <!-- how many cells for Z direction --> </PARAMETERS>
<VARIABLES> <V ID="0"> u </V> <V ID="1"> v </V> <V ID="2"> w </V> <V ID="3"> p </V> </VARIABLES>
<BOUNDARYREGIONS> <B ID="0"> C[9] </B> <!-- Inlet1_upper --> <B ID="1"> C[10] </B> <!-- Inlet2_Lower --> <B ID="2"> C[11] </B> <!-- Splitter plate --> <B ID="3"> C[12] </B> <!-- Upper Boundary --> <B ID="4"> C[13] </B> <!-- Lower_Boundary --> <B ID="5"> C[14] </B> <!-- Outlet --> <B ID="6"> C[15] </B> <!-- Wall_square --> </BOUNDARYREGIONS>
<BOUNDARYCONDITIONS>
<REGION REF="0"> <!-- Inlet_upper --> <D VAR="u" VALUE="1" /> <D VAR="v" VALUE="0" /> <D VAR="w" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0"/> </REGION>
<REGION REF="1"> <!-- Inlet_lower --> <D VAR="u" VALUE="1" /> <D VAR="v" VALUE="0" /> <D VAR="w" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0"/> </REGION>
<REGION REF="2"> <!--Splitter plate --> <D VAR="u" VALUE="0" /> <D VAR="v" VALUE="0" /> <D VAR="w" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> </REGION>
<REGION REF="3"> <!-- Upper Boundary --> <N VAR="u" USERDEFINEDTYPE="H" VALUE="0" /> <D VAR="v" VALUE="0" /> <N VAR="w" USERDEFINEDTYPE="H" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> </REGION>
<REGION REF="4"> <!-- Lower_Boundary --> <N VAR="u" USERDEFINEDTYPE="H" VALUE="0" /> <D VAR="v" VALUE="0" /> <N VAR="w" USERDEFINEDTYPE="H" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> </REGION>
<REGION REF="5"> <!-- Outlet -->
* <N VAR="u" USERDEFINEDTYPE="HOutflow" VALUE="0" /> <N VAR="v" USERDEFINEDTYPE="HOutflow" VALUE="0" /> <N VAR="w" USERDEFINEDTYPE="HOutflow" VALUE="0" /> <D VAR="p" USERDEFINEDTYPE="HOutflow" VALUE="0" /> * </REGION>
<REGION REF="6"> <!-- WallA_square --> <D VAR="u" VALUE="0" /> <D VAR="v" VALUE="0" /> <D VAR="w" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> </REGION>
</BOUNDARYCONDITIONS>
<!-- We initialise from pre-computed flow for speed --> <FUNCTION NAME="InitialConditions"> <E VAR="w" VALUE="awgn(1e-3)*cos(2*PI*z/LZ)" /> --> <!-- <F VAR="u,v,w,p" FILE="Start.chk" /> --> <!-- <E VAR="u,v,w,p" VALUE="0" /> --> <F VAR="u,v,p" FILE="Start2D.chk" /> <!-- start from 2D results --> </FUNCTION> <FUNCTION NAME="ExactSolution"> <E VAR="u" VALUE="0" /> <E VAR="v" VALUE="0" /> <E VAR="w" VALUE="0" /> <E VAR="p" VALUE="0" /> </FUNCTION>
</CONDITIONS>
----------------------------------------------------------------------------------
Thanks, Regards
On Sun, Jun 14, 2020 at 10:46 PM Sherwin, Spencer J < s.sherwin@imperial.ac.uk> wrote:
HI Reda,
I would definitely try Dealiasing, at least in the Spectral Element plane. Also you need to make sure the outflow boundary condition is not causing problems and possibly require HOUTFLOW conditions at the outflow?
The IMEXOrder2 is BDF2 on the linear viscous solve but we do not have a scheme to make the advection term implicit currently.
It should certainly run at Re=2000. We have a number of runs for a circular cylinder at Re=3900. @Andrea: Could you forward a session file for that?
Thanks, Spencer.
Spencer Sherwin FREng, FRAeS Head of Aerodynamics Section, Director of Research Computing Service, Professor of Computational Fluid Mechanics, Department of Aeronautics, s.sherwin@imperial.ac.uk South Kensington Campus, Phone: +44 (0)20 7594 5052 Imperial College London, Fax: +44 (0)20 7594 1974 London, SW7 2AZ, UK http://www.imperial.ac.uk/people/s.sherwin/
On 14 Jun 2020, at 07:15, sgepner@meil.pw.edu.pl wrote:
Hi Reda,
Have you tried using Dealliasing?
Pozdrawiam, Stanisław Gepner
14 cze 2020 01:32 Moto Light <redamansyhh@gmail.com> napisał(a):
This email from redamansyhh@gmail.com originates from outside Imperial. Do not click on links and attachments unless you recognise the sender. If you trust the sender, add them to your safe senders list <https://spam.ic.ac.uk/SpamConsole/Senders.aspx> to disable email stamping for this address.
Hi All,
I wish all of you are fine these days, I am running a 3D homogeneous case for a square cylinder, when I run the case at high Reynolds 2000 it keeps crashing, I tried *"SpectralVanishingViscosity"* it is working but it is filtering my field, what about using a different time integration method *"BDFImplicitOrder2" *instead of using *"IMEXOrder2"*, I think the two of them are 2nd order but using Implicit instead of Implicit explicit will not crash, but also I will keep CFL under 1 to be sure it is fine, even with this method i can go for higher CFL, my Reynolds is 2000 turbulent flow.
Regards, Reda UPC Barcelona +34 632 675 853
_______________________________________________ Nektar-users mailing list Nektar-users@imperial.ac.uk https://mailman.ic.ac.uk/mailman/listinfo/nektar-users
HI Moto, I think Andrea has sent you an input file for the cylinder case so I would recommend trying that setup. I do not often use the SkewSymmetric advection form but tend to use the convective form with de-aliasing instead so I would try that. We also tend to run the 2.5D solver with a direct multi-level solve (which can also be run in parallel). I cannot see a preconditioner in your setup so it will likely be using a diagonal preconditioner which is not great for the pressure part of the solve. Cheers, Spencer. Spencer Sherwin FREng, FRAeS Head of Aerodynamics Section, Director of Research Computing Service, Professor of Computational Fluid Mechanics, Department of Aeronautics, s.sherwin@imperial.ac.uk<mailto:s.sherwin@imperial.ac.uk> South Kensington Campus, Phone: +44 (0)20 7594 5052 Imperial College London, Fax: +44 (0)20 7594 1974 London, SW7 2AZ, UK http://www.imperial.ac.uk/people/s.sherwin/ On 14 Jun 2020, at 22:42, Moto Light <redamansyhh@gmail.com<mailto:redamansyhh@gmail.com>> wrote: Sorry, this is the error i have always CG iterations made = 5001 using tolerance of 1e-09 (error = -nan, rhs_mag = -nan) Thanks On Sun, Jun 14, 2020 at 11:21 PM Moto Light <redamansyhh@gmail.com<mailto:redamansyhh@gmail.com>> wrote: Hi Spencer. Thanks for replying I wish you a great day, could you check this is my settings and I will be very grateful if Andera can send me his file at 3900 to check the settings. but also what about using a different time integration method "BDFImplicitOrder2" instead of using "IMEXOrder2" in "TimeIntegrationMethod" , I think the two of them are 2nd order but using Implicit instead of Implicit explicit will not crash, also I will keep CFL under 1 to be sure it is fine, I tried "SpectralVanishingViscosity" it is working but it is filtering my field when I checked the velocity spectrum it was filtered. Also another case , please check my attachment file it has the same settings even with lower Reynolds at 400 using velocity ratio is crashing, for outlet BC i am already using HOutflowa. ----------------------------------------------------------------- <?xml version="1.0" encoding="UTF-8" ?> <NEKTAR> <EXPANSIONS> <E COMPOSITE="C[1]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 1 Domain inlet plate upper --> <E COMPOSITE="C[2]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 2 Domain inlet plate lower --> <E COMPOSITE="C[3]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- ****3 Domain square faces up down front meshs**** --> <E COMPOSITE="C[4]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 4 Domain upper domain lower in up stream --> <E COMPOSITE="C[5]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 5 Domain upper lower downstream --> <E COMPOSITE="C[6]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- ***6 Domain down stream back side square*** --> <E COMPOSITE="C[7]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 7 Domain down stream after square big one --> <E COMPOSITE="C[8]" NUMMODES="3" FIELDS="u,v,w,p" TYPE="MODIFIED" /> <!-- 7 Domain down stream after square big one --> </EXPANSIONS> <CONDITIONS> <SOLVERINFO> <I PROPERTY="SOLVERTYPE" VALUE="VelocityCorrectionScheme"/> <I PROPERTY="EQTYPE" VALUE="UnsteadyNavierStokes" /> <I PROPERTY="Projection" VALUE="Continuous" /> <I PROPERTY="EvolutionOperator" VALUE="Nonlinear" /> <I PROPERTY="TimeIntegrationMethod" VALUE="IMEXOrder2" /> <I PROPERTY="Driver" VALUE="Standard" /> <I PROPERTY="HOMOGENEOUS" VALUE="1D" /> <I PROPERTY="AdvectionForm" VALUE="SkewSymmetric" /> <I PROPERTY="Extrapolation" VALUE="Standard" /> <I PROPERTY="USEFFT" VALUE="FFTW" /> <!-- <I PROPERTY="DEALIASING" VALUE="ON" /> --> <I PROPERTY="SPECTRALHPDEALIASING" VALUE="ON" /> <!-- <I PROPERTY="SpectralVanishingViscosity" VALUE="True" /> --> </SOLVERINFO> <PARAMETERS> <P> TimeStep = 0.0003 </P> <P> NumSteps = 550000 </P> <!-- 60sec --> <P> IO_CheckSteps = 5000 </P> <!-- 120 check files--> 520 <P> IO_InfoSteps = 10 </P> <P> Re = 2000 </P> <P> Kinvis = 1./Re </P> <P> IO_CFLSteps = 50 </P> <P> LZ = 10 </P> <!-- 3. * Fastest spanwise --> <P> HomModesZ = 16 </P> <!-- how many cells for Z direction --> </PARAMETERS> <VARIABLES> <V ID="0"> u </V> <V ID="1"> v </V> <V ID="2"> w </V> <V ID="3"> p </V> </VARIABLES> <BOUNDARYREGIONS> <B ID="0"> C[9] </B> <!-- Inlet1_upper --> <B ID="1"> C[10] </B> <!-- Inlet2_Lower --> <B ID="2"> C[11] </B> <!-- Splitter plate --> <B ID="3"> C[12] </B> <!-- Upper Boundary --> <B ID="4"> C[13] </B> <!-- Lower_Boundary --> <B ID="5"> C[14] </B> <!-- Outlet --> <B ID="6"> C[15] </B> <!-- Wall_square --> </BOUNDARYREGIONS> <BOUNDARYCONDITIONS> <REGION REF="0"> <!-- Inlet_upper --> <D VAR="u" VALUE="1" /> <D VAR="v" VALUE="0" /> <D VAR="w" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0"/> </REGION> <REGION REF="1"> <!-- Inlet_lower --> <D VAR="u" VALUE="1" /> <D VAR="v" VALUE="0" /> <D VAR="w" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0"/> </REGION> <REGION REF="2"> <!--Splitter plate --> <D VAR="u" VALUE="0" /> <D VAR="v" VALUE="0" /> <D VAR="w" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> </REGION> <REGION REF="3"> <!-- Upper Boundary --> <N VAR="u" USERDEFINEDTYPE="H" VALUE="0" /> <D VAR="v" VALUE="0" /> <N VAR="w" USERDEFINEDTYPE="H" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> </REGION> <REGION REF="4"> <!-- Lower_Boundary --> <N VAR="u" USERDEFINEDTYPE="H" VALUE="0" /> <D VAR="v" VALUE="0" /> <N VAR="w" USERDEFINEDTYPE="H" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> </REGION> <REGION REF="5"> <!-- Outlet --> <N VAR="u" USERDEFINEDTYPE="HOutflow" VALUE="0" /> <N VAR="v" USERDEFINEDTYPE="HOutflow" VALUE="0" /> <N VAR="w" USERDEFINEDTYPE="HOutflow" VALUE="0" /> <D VAR="p" USERDEFINEDTYPE="HOutflow" VALUE="0" /> </REGION> <REGION REF="6"> <!-- WallA_square --> <D VAR="u" VALUE="0" /> <D VAR="v" VALUE="0" /> <D VAR="w" VALUE="0" /> <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> </REGION> </BOUNDARYCONDITIONS> <!-- We initialise from pre-computed flow for speed --> <FUNCTION NAME="InitialConditions"> <E VAR="w" VALUE="awgn(1e-3)*cos(2*PI*z/LZ)" /> --> <!-- <F VAR="u,v,w,p" FILE="Start.chk" /> --> <!-- <E VAR="u,v,w,p" VALUE="0" /> --> <F VAR="u,v,p" FILE="Start2D.chk" /> <!-- start from 2D results --> </FUNCTION> <FUNCTION NAME="ExactSolution"> <E VAR="u" VALUE="0" /> <E VAR="v" VALUE="0" /> <E VAR="w" VALUE="0" /> <E VAR="p" VALUE="0" /> </FUNCTION> </CONDITIONS> ---------------------------------------------------------------------------------- Thanks, Regards On Sun, Jun 14, 2020 at 10:46 PM Sherwin, Spencer J <s.sherwin@imperial.ac.uk<mailto:s.sherwin@imperial.ac.uk>> wrote: HI Reda, I would definitely try Dealiasing, at least in the Spectral Element plane. Also you need to make sure the outflow boundary condition is not causing problems and possibly require HOUTFLOW conditions at the outflow? The IMEXOrder2 is BDF2 on the linear viscous solve but we do not have a scheme to make the advection term implicit currently. It should certainly run at Re=2000. We have a number of runs for a circular cylinder at Re=3900. @Andrea: Could you forward a session file for that? Thanks, Spencer. Spencer Sherwin FREng, FRAeS Head of Aerodynamics Section, Director of Research Computing Service, Professor of Computational Fluid Mechanics, Department of Aeronautics, s.sherwin@imperial.ac.uk<mailto:s.sherwin@imperial.ac.uk> South Kensington Campus, Phone: +44 (0)20 7594 5052 Imperial College London, Fax: +44 (0)20 7594 1974 London, SW7 2AZ, UK http://www.imperial.ac.uk/people/s.sherwin/ On 14 Jun 2020, at 07:15, sgepner@meil.pw.edu.pl<mailto:sgepner@meil.pw.edu.pl> wrote: Hi Reda, Have you tried using Dealliasing? Pozdrawiam, Stanisław Gepner 14 cze 2020 01:32 Moto Light <redamansyhh@gmail.com<mailto:redamansyhh@gmail.com>> napisał(a): This email from redamansyhh@gmail.com<mailto:redamansyhh@gmail.com> originates from outside Imperial. Do not click on links and attachments unless you recognise the sender. If you trust the sender, add them to your safe senders list<https://spam.ic.ac.uk/SpamConsole/Senders.aspx> to disable email stamping for this address. Hi All, I wish all of you are fine these days, I am running a 3D homogeneous case for a square cylinder, when I run the case at high Reynolds 2000 it keeps crashing, I tried "SpectralVanishingViscosity" it is working but it is filtering my field, what about using a different time integration method "BDFImplicitOrder2" instead of using "IMEXOrder2", I think the two of them are 2nd order but using Implicit instead of Implicit explicit will not crash, but also I will keep CFL under 1 to be sure it is fine, even with this method i can go for higher CFL, my Reynolds is 2000 turbulent flow. Regards, Reda UPC Barcelona +34 632 675 853 _______________________________________________ Nektar-users mailing list Nektar-users@imperial.ac.uk<mailto:Nektar-users@imperial.ac.uk> https://mailman.ic.ac.uk/mailman/listinfo/nektar-users
participants (4)
-
Cassinelli, Andrea
-
Moto Light
-
sgepner＠meil.pw.edu.pl
-
Sherwin, Spencer J