Flow Across Tube Banks - Transient vs Steady State

HeatTransferFan · September 11, 2012, 19:01

Hello everyone,
I have been trying to model flow across a tube bank. I am trying to simulate flow and heat transfer across a heat sink with pin fins. The fluid section is 6.7 mm wide and about 229mm long with 34 cylinders (3.175mm in diameter) in cross flow. There are symmetry BC on the sides. I am trying to replicate some experimental results that were given for this flow in terms of average heat transfer coefficient and pressure drop obtained in a wind tunnel. I have a 115mm inlet section with 2m/s inlet velocity to allow the flow to develop and a 229mm outlet section at the end of which I have a 0 (relative) static pressure outlet. The flow is laminar. The problem I have been having is bouncy convergence. I get convergence up to 1e-3 or 1e-4 but then it become bouncy. I have tried refining the mesh, adjusting time steps (local and physical) and I get a little better or worse but never below e-4. Also I have been monitoring the area averaged inlet and outlet pressure and the htc. These values converge withing 40-50 iterations, however they change drastically when I adjust the mesh (I got values of 90kPa to 25kPa). I believe that the problem is because at the end of the last tube I get a vortex shredding region in the outlet section that is transient and cannot be simulated with a steady state analysis. Do you agree? If that is the case, should I worry about the vortex shredding if I am worried only in the pressure drop across the tubes? I get good convergence when I set up a coarse mesh in the outlet region. Sorry for the long explanation and thanks for your help,

Krsto

ghorrocks · September 11, 2012, 20:21

See this FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Also are you sure this is laminar? I suspect the flow is of a high enough Re number to be turbulent, and that would also affect convergence.

HeatTransferFan · September 11, 2012, 23:22

Glenn,
I read that post before I posted. I tired everything on there (besides transient runs) and it did not help. I have some doubts about the turbulence part. Most of the data is experimental so there is no clear definition of a Re number that gives onset of turbulence. I could guess from the experimental graph for friction factor that it is at about Re=1000 (that is when the curve starts leveling off). My current Re is about 770. I'll try at lower Re and let you know. Is there a way to see if the flow is stable or not using CFX? I feel that lack of convergence is not a good indicator. I can try to run it at turbulent but then again, the fact that it convergence doesn't mean that it is turbulent (Right?). What about the vortex shredding issue? Do you think I have to worry about that if I am only interested in the area average pressure at the inlet and outlet?
Thanks a lot for your help,

Krsto

ghorrocks · September 12, 2012, 09:17

Quote:

My current Re is about 770.

In that case it could be laminar or turbulent depending on many things. You are going to have to work out which way it is. But my suggestion is to assume turbulent and use a turbulence model suitable for low Re flows such as SST. This turbulence model is still pretty good in high laminar flows and does not dissipate too much, in general.

Alternately you could use a turbulence transition model. This is an even better approach again, but will probably require a pretty massive mesh to run.

Quote:

Is there a way to see if the flow is stable or not using CFX?

Run it transient and have a look at what the flow is doing.

Quote:

I feel that lack of convergence is not a good indicator.

Agreed.

HeatTransferFan · September 15, 2012, 00:24

Glenn,
I have tried raising the Re # to make sure that the flow is turbulent and use SST to model the flow but I still get the same convergence issue. The RMS gets to about 1e-3 and then it start bouncing around. I have tried again playing with the mesh but the only thing that happens is that the residual settles at a lower RMS. I also tried running it for very low Re where I know there is no vortex shedding and it converged quite well. My point is that all I want is the average pressure drop in the system so I am not too worried about capturing all the features of the flow. I already have experimental results so I know what my average pressure should be. Do you suggest that I run it still in steady state possibly with a coarser mesh (which might not capture the instability in the flow but still give me a relatively accurate pressure drop) or would the results just be wrong? The main idea is that I want to be able to validate my mesh for a certain diameter and then study the effect of increasing diameter with the same mesh. Thank you so much for your help,

Krsto

ghorrocks · September 15, 2012, 08:20

If you get vortex shedding (especially transient shedding like a von Karman vortex street) then you will never get a steady state simulation to converge. You have to model it transient as the flow is transient.

I think this is what is happening to you - vortex shedding is preventing convergence for you steady state run. You need to run transient.

HeatTransferFan · September 17, 2012, 14:53

Glenn,
I still tried to run steady state and didn't work... Obviously. The problem is that the RMS gets around 1e-4 and the points of interest (inlet and outlet area averaged pressure) fluctuate very little around the experimental values. I found some paper and they claim that vortex shedding is not an important phenomena in our case but it is present around the first 3-4 tubes. I am thinking about (after my transient run) to just put a coarser mesh in that region and try to run steady state and see what happens. Because I plan on doing a parametric study, I am really trying to avoid transient because of the computational time required. Anyway, I'll let you know how it goes.
Thanks again for your help,

Krsto

HeatTransferFan · September 18, 2012, 01:39

Hello,
So I am running the transient simulation and the problem is definitely transient and has features that change very quickly. From the Strhoul numern for a single cylinder I calculated the frequency of the Von Karman vorteces and I selected an adaptive time step. The problem now is that it takes about 10-14 coefficient loops to achieve a MAX of less than 1e-3 and each time step is 0.0001 [s]. So it will take forever to get a solution over a valid interval. Anyway, that is just a fact however I have a question. I attached the plot of the inlet and outlet area averaged pressure along with the HTC. As you can see, the HTC is steady state, the outlet pressure converges within each iteration but the inlet pressure looks to be constantly changing. In my understanding of the transient solver, at each timestep (if the solution is good) the inlet pressure should achieve a constant value if the solution at that timestep has converged. Thus, the convergence plot for the inlet pressure should be a series of steps and not a continous function as it is right now. Is that correct? If that is the case, why does that happen? My RMS at each timestep is usually ~ 1e-6 so I would say that the solution is pretty good. Can anyone help me? Is my understanding wrong?
Thank you very much for your help,

Krsto Sbutega

ghorrocks · September 18, 2012, 01:50

Transient simulations take a long time, that is unavoideable.

If you are taking 10-14 coeff loops per time step then you should use adaptive time stepping to target 3-5 coeff loops per time step. That will run more efficiently.

Your attachments were not posted. Can you post an image of your geometry?

Note that tight convergence is only one requirement for accuracy. There are many others - see http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

HeatTransferFan · September 27, 2012, 16:02

Glenn,
Sorry for the late answer. So I managed to obtain convergence. What I did is I ran the simulation transient but the oscillations were so fast that I had to use a timestep of about 1e-5. So I went and did some reading on flow across pin fins and I found that indeed there is some transient effects and some Coanda effect. So I shifted my symmetry planes by one pitch length and put it through the middle of the circular pins (as opposed through the middle of the channel). This will not allow me to capture the Coanda effect around the cylinders but I am willing to live with that. Also, I switched to k-epsilon turbulence because I have read that the k-espilon model will stamp out the oscillations. Once again that is not ideal but I am only interested in the overall pressure drop and heat transfer coefficient so I am not interested in the minute details of the flow. Bottomline, I obtain convergence now and the computed results are within 7% for the pressure drop and 5% for the heat transfer coefficient of the experimental values.
Thank you for your help

ghorrocks · September 27, 2012, 19:22

I am amazed your results are that accurate when you have suppressed some apparently important physics (Coanda, oscillatory flow). These effects could easily modify the pressure loss by quite a bit.

HeatTransferFan · September 28, 2012, 15:21

Glenn,
I have 20 pin fins and it has been shown that the transient effects are on the first 2-3 pins until the flow fully develops. I think that's why I can get away with not modeling these effects. However, SST did not converge. I am going to try at a higher Re because I think that the transient effects decrease as the Re increases. I'll let you know
Thanks a lot for your help. Often problems force you to explore things in more detail and give you a better understanding not only of the CFD software but of fluid mechanics itself.

September 11, 2012, 19:01	Flow Across Tube Banks - Transient vs Steady State	#1
HeatTransferFan New Member Join Date: Jul 2012 Posts: 11 Rep Power: 14	Hello everyone, I have been trying to model flow across a tube bank. I am trying to simulate flow and heat transfer across a heat sink with pin fins. The fluid section is 6.7 mm wide and about 229mm long with 34 cylinders (3.175mm in diameter) in cross flow. There are symmetry BC on the sides. I am trying to replicate some experimental results that were given for this flow in terms of average heat transfer coefficient and pressure drop obtained in a wind tunnel. I have a 115mm inlet section with 2m/s inlet velocity to allow the flow to develop and a 229mm outlet section at the end of which I have a 0 (relative) static pressure outlet. The flow is laminar. The problem I have been having is bouncy convergence. I get convergence up to 1e-3 or 1e-4 but then it become bouncy. I have tried refining the mesh, adjusting time steps (local and physical) and I get a little better or worse but never below e-4. Also I have been monitoring the area averaged inlet and outlet pressure and the htc. These values converge withing 40-50 iterations, however they change drastically when I adjust the mesh (I got values of 90kPa to 25kPa). I believe that the problem is because at the end of the last tube I get a vortex shredding region in the outlet section that is transient and cannot be simulated with a steady state analysis. Do you agree? If that is the case, should I worry about the vortex shredding if I am worried only in the pressure drop across the tubes? I get good convergence when I set up a coarse mesh in the outlet region. Sorry for the long explanation and thanks for your help, Krsto

September 15, 2012, 00:24		#5
HeatTransferFan New Member Join Date: Jul 2012 Posts: 11 Rep Power: 14	Glenn, I have tried raising the Re # to make sure that the flow is turbulent and use SST to model the flow but I still get the same convergence issue. The RMS gets to about 1e-3 and then it start bouncing around. I have tried again playing with the mesh but the only thing that happens is that the residual settles at a lower RMS. I also tried running it for very low Re where I know there is no vortex shedding and it converged quite well. My point is that all I want is the average pressure drop in the system so I am not too worried about capturing all the features of the flow. I already have experimental results so I know what my average pressure should be. Do you suggest that I run it still in steady state possibly with a coarser mesh (which might not capture the instability in the flow but still give me a relatively accurate pressure drop) or would the results just be wrong? The main idea is that I want to be able to validate my mesh for a certain diameter and then study the effect of increasing diameter with the same mesh. Thank you so much for your help, Krsto Last edited by HeatTransferFan; September 15, 2012 at 01:10.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
mass flow in is not equal to mass flow out	saii	CFX	12	March 19, 2018 06:21
Surface inejction- steady state - mass flow rate	CFD-student	FLUENT	0	January 25, 2012 14:40
???????simulate heat distribution in an incompressibe laminar steady state flow??????	anijdon	OpenFOAM	1	November 27, 2010 15:37
initialize flow field with steady state solution	holg	FLUENT	0	July 13, 2009 18:10
About the difference between steady and unsteady problems	Lisa	Main CFD Forum	11	July 5, 2000 15:37

September 11, 2012, 20:21		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	See this FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria Also are you sure this is laminar? I suspect the flow is of a high enough Re number to be turbulent, and that would also affect convergence.

September 11, 2012, 23:22		#3
HeatTransferFan New Member Join Date: Jul 2012 Posts: 11 Rep Power: 14	Glenn, I read that post before I posted. I tired everything on there (besides transient runs) and it did not help. I have some doubts about the turbulence part. Most of the data is experimental so there is no clear definition of a Re number that gives onset of turbulence. I could guess from the experimental graph for friction factor that it is at about Re=1000 (that is when the curve starts leveling off). My current Re is about 770. I'll try at lower Re and let you know. Is there a way to see if the flow is stable or not using CFX? I feel that lack of convergence is not a good indicator. I can try to run it at turbulent but then again, the fact that it convergence doesn't mean that it is turbulent (Right?). What about the vortex shredding issue? Do you think I have to worry about that if I am only interested in the area average pressure at the inlet and outlet? Thanks a lot for your help, Krsto

September 15, 2012, 08:20		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	If you get vortex shedding (especially transient shedding like a von Karman vortex street) then you will never get a steady state simulation to converge. You have to model it transient as the flow is transient. I think this is what is happening to you - vortex shedding is preventing convergence for you steady state run. You need to run transient.

September 17, 2012, 14:53		#7
HeatTransferFan New Member Join Date: Jul 2012 Posts: 11 Rep Power: 14	Glenn, I still tried to run steady state and didn't work... Obviously. The problem is that the RMS gets around 1e-4 and the points of interest (inlet and outlet area averaged pressure) fluctuate very little around the experimental values. I found some paper and they claim that vortex shedding is not an important phenomena in our case but it is present around the first 3-4 tubes. I am thinking about (after my transient run) to just put a coarser mesh in that region and try to run steady state and see what happens. Because I plan on doing a parametric study, I am really trying to avoid transient because of the computational time required. Anyway, I'll let you know how it goes. Thanks again for your help, Krsto

September 18, 2012, 01:50		#9
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	Transient simulations take a long time, that is unavoideable. If you are taking 10-14 coeff loops per time step then you should use adaptive time stepping to target 3-5 coeff loops per time step. That will run more efficiently. Your attachments were not posted. Can you post an image of your geometry? Note that tight convergence is only one requirement for accuracy. There are many others - see http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

September 27, 2012, 16:02		#10
HeatTransferFan New Member Join Date: Jul 2012 Posts: 11 Rep Power: 14	Glenn, Sorry for the late answer. So I managed to obtain convergence. What I did is I ran the simulation transient but the oscillations were so fast that I had to use a timestep of about 1e-5. So I went and did some reading on flow across pin fins and I found that indeed there is some transient effects and some Coanda effect. So I shifted my symmetry planes by one pitch length and put it through the middle of the circular pins (as opposed through the middle of the channel). This will not allow me to capture the Coanda effect around the cylinders but I am willing to live with that. Also, I switched to k-epsilon turbulence because I have read that the k-espilon model will stamp out the oscillations. Once again that is not ideal but I am only interested in the overall pressure drop and heat transfer coefficient so I am not interested in the minute details of the flow. Bottomline, I obtain convergence now and the computed results are within 7% for the pressure drop and 5% for the heat transfer coefficient of the experimental values. Thank you for your help

September 27, 2012, 19:22		#11
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,870 Rep Power: 144	I am amazed your results are that accurate when you have suppressed some apparently important physics (Coanda, oscillatory flow). These effects could easily modify the pressure loss by quite a bit.

September 28, 2012, 15:21		#12
HeatTransferFan New Member Join Date: Jul 2012 Posts: 11 Rep Power: 14	Glenn, I have 20 pin fins and it has been shown that the transient effects are on the first 2-3 pins until the flow fully develops. I think that's why I can get away with not modeling these effects. However, SST did not converge. I am going to try at a higher Re because I think that the transient effects decrease as the Re increases. I'll let you know Thanks a lot for your help. Often problems force you to explore things in more detail and give you a better understanding not only of the CFD software but of fluid mechanics itself.