Learning Forum

[tomk88]

Hi, nI'm currently simulating the heat transfer from a large tank filled with stationary, hot fluid to a colder stream of fluid which runs through a pipe in the centre of the tank, going up its length vertically. The cold fluid enters at the bottom and is pumped through the pipe towards the top. Once simulating, the temperature distribution looks great everywhere apart from at the pipe outlet. For some reason, the temperature at the top of the pipe drops at the tip despite the fact the rest of the pipe and water inside it heats up until this point. The temperature of the surrounding pipe also drops at this point, as does the inner face of the water tank at this point. The boundaries are all adiabatic, so the heat isn't being lost to the surroundings. I simply can't understand why the top of the pipe is losing heat despite heating up well up to this point. The inlets and outlets are mass in flows and outflows. Can anyone help?nThank you. n

[YasserSelima]

Can you plot the velocity profile in the tank. You might have large circulation happening.n

[tomk88]

nI can plot the velocity profile in the tank, and it looks good. I would expect to see movement in the tank since convection will take place due to the fact I have a density and temperature relationship enabled. The hot water rises to the top and the colder water drifts to the bottom, as expected. The velocity profile vectors in the tank shoot down the outside side of the pipe which is what I would expect. Is this a problem? n

[YasserSelima]

Not a problem. This is what I wanted to see. nWhat about the velocity profile at the top of the tank? Zoom on the top wall and check the velocity and temperature.n

[YasserSelima]

I have a guess but I am not sure.nThe solver is forced to change the velocity profile at the tip of the pipe to uniform velocity outflow boundary condition. This forces cold liquid from the core of the pipe to move into the walls causing this temperature drop at the pipe walls.n

[YasserSelima]

If this is the case, you will find cold layer stuck in the tank near the pipe and doesn't circulate. Also you will see the water in the pipe flowing from the center towards the wall at the tip of the pipe.n

[tomk88]

nI think your assumptions are potentially correct, so I will attach some images for you to review.nThe first image is the temperature of the water in the pipe when I have disabled gravity in the simulation, hence there is no convection transfer occurring in the tank. Yet the problem persists so I know it is not the convection action in the tank that is causing the problem.nThe second image shows the gravity enabled, and although it is not clear since the temperature differences are small compared to the global scale, there is convection occurring in the tank - I can see this by turning on velocity vectors too. You can see the temperature drop at the pipe tip clearly. Also, like you suggested, the water in the pipe flows towards the wall at the tip of the pipe, why is this?nFinally, the last picture shows a few reverse velocity vectors at the tip of the pipe, I cannot understand why this is occurring. At no point in the solver did the Fluent program state there was reversed flow on the outlet face, I am confused. nCan you advise further how to solve the problem now you have seen the images? nn

[YasserSelima]

The outflow boundary condition is a zero velocity gradient. In your case, the flow inside the pipe heats as it goes up, the layers close to the wall will have higher velocity because of the higher temperature and hence they move toward the center. Close to the tip, Ansys forces the opposite to have zero gradient at the exit.nTry changing the outlet to outlet pressure, and make the back flow from neighbors (You might get back flow at low mass flowrates). This might solve the problem. Another solution could be increasing the pipe length a little bit above the tank. nIn all cases I believe your solution is valid. Try Volume weighted average of the temperature and you should find this increasing to the tip. n

[tomk88]

nI changed the outlet to a pressure outlet and also extended the top of the pipe by a small distance. I also simulated the case where the outlet was a pressure outlet, but without the pipe extension - both simulations with the same mass flow rate from inlet. The pipe extension simulation gives me an outlet temperature closer to my desired value compared with the previous model, so I think I will move forward with this design. Furthermore, to achieve this, I had to change the backflow temperature to my desired output value which I had not previously considered. I still get a backflow at the pipe outlet, but the temperature issue is solved by setting the backflow temperature issue. Will there always be a backflow present at low flow rates?nI have attached further images in the hope you can confirm the validity of them. Both images are from the situation where the pipe is extended beyond the length of the tank.nThe first image shows the temperatures in the tank and pipe. I think this is reasonable, considering I have set the backflow temperature to a value I expect to see given the pipe dimensions and mass flow rate. Can you comment on this, is this a reasonable temperature profile inside the pipe?nThe second image shows the velocity vectors, and a backflow is clearly visible at the top, but if you think this is not an issue and is to be expected at low flow rates, then I understand and I will read into related literature about this. nnn

[YasserSelima]

Hello,nI will start my comment on the second figure, the back flow. For upward vertical flow in a pipe, because of the velocity profile, the high velocity fluid will move radially towards the low velocity fluid. In your case, the vertical velocity is higher at the large radius. Just beyond the boundary layer. (This is the red region in the temperature distribution. So, the flow from this red region goes towards the centre. At the exit, because of the constant pressure ... the flow find it easier to leave the pipe than going towards the centre. Meanwhile, at the centre, the upward flow rate can not continue without being fed from the red region. nMy recommendation is just to make the back flow from neighbouring cells. This will account for part of this radial flow without having energy imbalance.nFor the temperature distribution, I think it makes sense. nOne thing that is important when generating your report, the temperature distribution and velocity vectors are nice and they would enrich the report .. but when you are reporting numbers, get the mass average of the temperature ...

[tomk88]

nI've taken your advice and set the outlet condition to define the backflow relative to neighbouring cells and this seems to have improved the design further. The final average temperature at the outlet is within a 0.5% tolerance of the expected result, so it looks like the model works. I think I have determined this design is now suitable, and I can justify the results. Thank you for your help once again, I really do appreciate it!n

[YasserSelima]

You are welcome!n