Boundary Conditions at Outlet
Dear All, I've several questions about outflow boundary conditions for boundary regions and conditions specified below for a pipe flow problem: */<BOUNDARYREGIONS>/**/ /**/ <B ID="0"> C[2] </B> <!-- Inlet -->/**/ /**/ <B ID="1"> C[3] </B> <!-- Outlet -->/**/ /**/ <B ID="2"> C[1] </B> <!-- Wall -->/**/ /**/ </BOUNDARYREGIONS>/**/ /**/ /**/ <BOUNDARYCONDITIONS>/**/ /**/ <REGION REF="0">/**/ /**/ <D VAR="u" VALUE="0" />/**/ /**/ <D VAR="v" VALUE="0" />/**/ /**/ <D VAR="w" VALUE="1" />/**/ /**/ <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" />/**/ /**/ </REGION>/**/ /**/ <REGION REF="1">/**/ /**/ <N VAR="u" VALUE="0" />/**/ /**/ <N VAR="v" VALUE="0" />/**/ /**/ <N VAR="w" VALUE="0" />/**/ /**/ <D VAR="p" VALUE="0" />/**/ /**/ </REGION>/**/ /**/ <REGION REF="2">/**/ /**/ <D VAR="u" VALUE="0" />/**/ /**/ <D VAR="v" VALUE="0" />/**/ /**/ <D VAR="w" VALUE="0" />/**/ /**/ <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" />/**/ /**/ </REGION>/**/ /**/ </BOUNDARYCONDITIONS>/* 1) What is the meaning of */<N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> /*and why do we specify such a BC at the wall of the pipe? What happens if I don't specify any pressure BC at the wall of the pipe?*/ /*2) Is there any other option to specify pressure BC at the outlet other than*//**/*/<D VAR="p" VALUE="0" />/*/* ?*/*//*/*For example is it possible to apply the pressure BC at the outlet given below which is specified in a paper (Direct numerical simulation of stenotic flows. Part 1. Steady flow, SONU S. VARGHESE, STEVEN H. FRANKEL AND PAUL F. FISCHER) ? /*In turbulent flows, it is possible to have vortices strong enough to yield a (locally) negative flux at the outflow boundary. Since no flow characteristics are specified on these boundaries, a negative flux condition typically leads to instabilities with catastrophic results. One way to ensure that the characteristics at the exit are always pointing outwards is to force the exit flow through a nozzle, effectively adding a mean axial component to the velocity field. In contrast, schemes based on viscous *//*buffer zones require knowledge of the anticipated space and time scales to ensure that vortical structures are adequately damped as they pass through the buffer zone.*//* *//*This nozzle effect can be imposed numerically without having to change the mesh geometry by imparting a positive divergence to the flow field near the exit (in the spirit of a supersonic nozzle). In the current study, this is done by identifying the layer of elements adjacent to the outflow and imposing a divergence function D(x) that is zero at the upstream end of the layer and ramps to a fixed positive value at the exit. Specifically, we set D(x)=C[1−(x⊥/L⊥)2], where x⊥ is the distance normal to the boundary and L⊥ is the maximum thickness of the last layer of elements. A net gain in mean velocity is obtained over the extent of the layer by integrating the expression for D from x⊥/L⊥=1 to 0. The constant C is chosen such that the gain is equal to the mean velocity prior to the correction.*//* */*/ /*Regards, Kamil
Dear Kamil, 1) What is the meaning of <N VAR="p" USERDEFINEDTYPE="H" VALUE="0" /> and why do we specify such a BC at the wall of the pipe? What happens if I don't specify any pressure BC at the wall of the pipe? the Userdefinedtype flag “h” denotes the use of the high order boundary conditions leading to a Neumann pressure condition which is associated with the Velocity Correction scheme we use for the Navier-Stokes. This scheme is outline in the user guide (4.0.0) on page 55. equation (7.4). The original paper is in JCP and is due to Karniadakis, Israeli and Orszag. 2) Is there any other option to specify pressure BC at the outlet other than <D VAR="p" VALUE="0" /> ? For example is it possible to apply the pressure BC at the outlet given below which is specified in a paper (Direct numerical simulation of stenotic flows. Part 1. Steady flow, SONU S. VARGHESE, STEVEN H. FRANKEL AND PAUL F. FISCHER) ? We have recently been using a high order outflow condition based not the work of Steve Dong in JCP. An example is given in the IncNavierStokesSolver/Tests/Tet_Kovasnay_HOBC.xml where we use the following conditions <REGION REF="1"> <N VAR="u" USERDEFINEDTYPE="HOutflow" VALUE="-Kinvis*KovLam*exp(KovLam*x)*cos(2*PI*y) - 0.5*(1-exp(2*KovLam*x))-0.5*(((1-exp(KovLam*x)*cos(2*PI*y))*(1-exp(KovLam*x)*cos(2*PI*y))+(KovLam/(2*PI)*exp(KovLam*x)*sin(2*PI*y))*(KovLam/(2*PI)*exp(KovLam*x)*sin(2*PI*y))))*(0.5*(1.0-tanh((1-exp(KovLam*x)*cos(2*PI*y))*20)))" /> <N VAR="v" VALUE="KovLam*KovLam/(2*PI)*exp(KovLam*x)*sin(2*PI*y)" /> <N VAR="w" VALUE="0" /> <D VAR="p" USERDEFINEDTYPE="HOutflow" VALUE="-Kinvis*KovLam*exp(KovLam*x)*cos(2*PI*y) - 0.5*(1-exp(2*KovLam*x)) -0.5*(((1-exp(KovLam*x)*cos(2*PI*y))*(1-exp(KovLam*x)*cos(2*PI*y))+(KovLam/(2*PI)*exp(KovLam*x)*sin(2*PI*y))*(KovLam/(2*PI)*exp(KovLam*x)*sin(2*PI*y))))*(0.5*(1.0-tanh((1-exp(KovLam*x)*cos(2*PI*y))*20)))" /> </REGION> Note in general the VALUE is set to “0”. Here we know the analytic solution so can specify a non-zero value. We are using these outflow conditions when we get energetic flow at the outflow and providing the mean flow is crossing the outflow plan they seem to work reasonably well. Details of Dong’s paper are in J. Comp. Phys. We do need to put some information in the user manual on this. Cheers, Spencer. In turbulent flows, it is possible to have vortices strong enough to yield a (locally) negative flux at the outflow boundary. Since no flow characteristics are specified on these boundaries, a negative flux condition typically leads to instabilities with catastrophic results. One way to ensure that the characteristics at the exit are always pointing outwards is to force the exit flow through a nozzle, effectively adding a mean axial component to the velocity field. In contrast, schemes based on viscous buffer zones require knowledge of the anticipated space and time scales to ensure that vortical structures are adequately damped as they pass through the buffer zone. This nozzle effect can be imposed numerically without having to change the mesh geometry by imparting a positive divergence to the flow field near the exit (in the spirit of a supersonic nozzle). In the current study, this is done by identifying the layer of elements adjacent to the outflow and imposing a divergence function D(x) that is zero at the upstream end of the layer and ramps to a fixed positive value at the exit. Specifically, we set D(x)=C[1−(x⊥/L⊥)2], where x⊥ is the distance normal to the boundary and L⊥ is the maximum thickness of the last layer of elements. A net gain in mean velocity is obtained over the extent of the layer by integrating the expression for D from x⊥/L⊥=1 to 0. The constant C is chosen such that the gain is equal to the mean velocity prior to the correction. Regards, Kamil _______________________________________________ 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 (2)
-
Kamil ÖZDEN
-
Sherwin, Spencer J