Warning Message : L1/L2 DIV(V)
Dear Developers, I am trying to run an LES in a turbine blade passage and I ran into this warning message during my production run: L1/L2 DIV(V) : 1.9224E-01 2.3951E+00 L1/L2 QTL : 1.9180E-01 2.3014E+00 L1/L2 DIV(V)-QTL: 4.3317E-04 6.6792E-01 WARNING: DIV(V)-QTL too large! I tried to grep it to the source code and found that the quantity QTL refers to the thermal divergence ( I do use usrdiv in my outlet ). But my case is purely from a fluids perspective and does not involve heat transfer. So I am wondering how QTL would pop up in my simulation. And I also noted that the error message comes up only when I use PN-PN basis function. I would like to know if this error message is a concern at all . Regards Shriram
The WARNING tells you that the divergence of your flow field is too large. It's hard to say why this happens because there are many possible reasons (wrong bc, resolution to low, timestep to large, etc.). I agree in your case the thermal divergence is ZERO. In your case the norms of div(v) and div(v)-qtl should be the same because qtl=0. Do you add some divergence to the outflow boundary? In this case the user specified divergence will be stored using qtl. Stefan On May 3, 2010, at 9:56 PM, [email protected] wrote:
Dear Developers,
I am trying to run an LES in a turbine blade passage and I ran into this warning message during my production run:
L1/L2 DIV(V) : 1.9224E-01 2.3951E+00 L1/L2 QTL : 1.9180E-01 2.3014E+00 L1/L2 DIV(V)-QTL: 4.3317E-04 6.6792E-01 WARNING: DIV(V)-QTL too large!
I tried to grep it to the source code and found that the quantity QTL refers to the thermal divergence ( I do use usrdiv in my outlet ). But my case is purely from a fluids perspective and does not involve heat transfer. So I am wondering how QTL would pop up in my simulation. And I also noted that the error message comes up only when I use PN-PN basis function. I would like to know if this error message is a concern at all .
Regards Shriram _______________________________________________ Nek5000-users mailing list [email protected] https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users
Hi Stefan, I have 23k elements and an lx1=11, so I am guessing my resolution is reasonably good (32 Mil Nodes) . As regarding the boundary conditions, yes I do add some divergence at the outflow. I am running it at CFL of close to 2 with 2nd order time stepping. Would you recommend lowering the Courant to say 0.5 ? Even though the warning pops up, I don't see any crazy stuff happening in my flow . Regards Shriram Jagannathan
Well I cannot tell you if you resolution is large enough. As you know this depends on the scales you need to resolve. Is this a DNS resolution? If you do some large scale runs I recommend to run with lx1=8 and a larger number of elements. A high polynomial order N is typically not needed for engineering type problems. In addition there are several reason why you don't want to increase N more than needed: - CFL scales with 1/N^2 so with a higher N you have to use a smaller dt - the number of pressure iterations may depend on N (depending on your mesh and preconditioner) Are you using IFCHAR=T? Filtering? Dealiasing? You may want to post the logfile. Stefan On May 3, 2010, at 10:15 PM, [email protected] wrote:
Hi Stefan,
I have 23k elements and an lx1=11, so I am guessing my resolution is reasonably good (32 Mil Nodes) . As regarding the boundary conditions, yes I do add some divergence at the outflow. I am running it at CFL of close to 2 with 2nd order time stepping. Would you recommend lowering the Courant to say 0.5 ? Even though the warning pops up, I don't see any crazy stuff happening in my flow .
Regards Shriram Jagannathan
_______________________________________________ Nek5000-users mailing list [email protected] https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users
Hi Stefan, I am running an LES with the following parameters: 1. p101=3 and p103 =0.05(filter weight). 2. De aliasing enabled and set to 16. (lxd = 16 ) 4. lx1 = 11 3. Yes, IFCHAR is on and a CFL close to 2 is used. 4. I add some divergence to the flow outlet using the same procedure detailed in the examples. This is my first flow through the domain and I intend to run it for a couple more depending on the results. Thank you for the info on order of interpolation polynomial. I would have to refine my domain in order to match the resolution by reducing the lx1. I will look into it. Please find attached pieces of rea and log file stacked together in the attachment. Thanks. Regards Shriram
You may want to use lx1=10 and compile Nek with K10_MXM in case your running on machine with AMD 10h processors. In addition you can lower the pressure tolerance to 5e-5 to save computational time. Is there a specific reason not to use the PN/PN-2 formulation? Your pressure iterations are quite high but I guess this is because of your mesh. At the moment the PN/PN does not support our multi-grid preconditioner and you're more sensitive to high aspect ratios (effected by the element size + N). Also please I recommned to use dt = -3e-3 and param(27)=2. Typically a Courant number of two gives you the best performance for the characteristics scheme. I may help to visualize the difference in divergence. Where are the high values (at element boundaries, domain boundaries, etc.)? In your case QTL contains the user specified divergence at the outflow. Stefan On May 3, 2010, at 10:52 PM, [email protected] wrote:
Hi Stefan,
I am running an LES with the following parameters:
1. p101=3 and p103 =0.05(filter weight). 2. De aliasing enabled and set to 16. (lxd = 16 ) 4. lx1 = 11 3. Yes, IFCHAR is on and a CFL close to 2 is used. 4. I add some divergence to the flow outlet using the same procedure detailed in the examples.
This is my first flow through the domain and I intend to run it for a couple more depending on the results.
Thank you for the info on order of interpolation polynomial. I would have to refine my domain in order to match the resolution by reducing the lx1. I will look into it.
Please find attached pieces of rea and log file stacked together in the attachment. Thanks.
Regards Shriram
<logfile>_______________________________________________ Nek5000-users mailing list [email protected] https://lists.mcs.anl.gov/mailman/listinfo/nek5000-users
Hi Stefan, I apologize for the delay in replying to your questions. 1. In earlier conversation I was told that PN-PN formulation has resulted in better accuracy. As such, I am not sure how one would choose which basis (PN-PN / PN-PN-2) is appropriate for their problem. I am working in transitional flows. Would you recommend any particular choice of basis for this type of applications ? 2. Yes, I believe I am running it on AMD 10h processors. I will compile with K10_MXM for my production run. Thanks. 3. As regarding the divergence : Though the warning pops up every step, nothing blows up in my simulation. The high values ( that are acceptable) are at the outflow where we add some divergence to the flow. 4. I did observe one thing, If I lower the courant to very low value, the error drops down but not by a huge margin. Thanks Shriram
1. In earlier conversation I was told that PN-PN formulation has resulted in better accuracy. As such, I am not sure how one would choose which basis (PN-PN / PN-PN-2) is appropriate for their problem. I am working in transitional flows. Would you recommend any particular choice of basis for this type of applications ? In general I would recommend to use the PN/PN formulation. However there are some features (e.g. moving mesh, free surface flows, MHD, etc.) which only work for PN/PN-2 for now. In addition we don't have the SEMG multigrid preconditioner in place for PN/PN. So depending on your mesh the cost of the pressure solve is higher (more iterations are needed for a given tolerance) although the cost is usually lower per iteration for PN/PN (no interpolation is needed).
2. Yes, I believe I am running it on AMD 10h processors. I will compile with K10_MXM for my production run. Thanks. For the moment the tuned version is only available for lx1=10 and lx1=8!
3. As regarding the divergence : Though the warning pops up every step, nothing blows up in my simulation. The high values ( that are acceptable) are at the outflow where we add some divergence to the flow. Sure you will have some pretty large values at the outflow. That's ok but I am confused by the large L2-norm of the difference in divergence.
4. I did observe one thing, If I lower the courant to very low value, the error drops down but not by a huge margin. Yes there is a time step effect but usually your limited by spatial resolution.
Stefan
participants (1)
-
nek5000-users＠lists.mcs.anl.gov