Subsea Spool Heat Transfer Simulation Help.
I am trying to evaluate the thermal efficiency of a subsea warming spool at 47.3C submerged in sea water with an ambient temperature of 4C , in a variety of arrangements In 2D in a 50mby 50m domain. Firstly, single straight Pipe, then a 2 Pipe setup with offset in the X Direction with the distance between the pipes as a factor of the pipe diameter (i.e 2*D, 3*D , 4*D etc), and finally a 2 Pipe setup with offset in the YDirection with the distance between the pipes as a factor of the pipe diameter (i.e 2*D, 3*D , 4*D etc).
Firstly, as I am trying to model to evaluate the Total heat transfer rate and surface heat transfer coefficent through the pipe to the surrounding sea water and the surface heat transfer coefficent. Do I input the properties of the pipe in the reference value section or of seawater in the reference value, boundary conditions and operating conditions section . In addition, for the pressure in the reference value and operating conditions section do I input the hydrostatic pressure at the water depth. If so the bottom of the seafloor is 800m below sea water and the pipe is in the midldle of the domain. Do I use the Hydrostatic pressure at a depth 800m or at 750m
The variation of seawater density with temperature has been inputed using the piecewise linear function in ANSYS for 50 data points from 47.3C to 4.7C.
Secondlly, there is no velocity for the seawater so is it necessary to use a turbulence model in my set up. When Using the laminar model I see the covective wake I expect at the bottom of the pipe and the build up and jetting of cold fluid at the bottom of the pipe:
When using the Komega model (with and without low Recorrection) I dont see this result, I see no covective wake at all. I do understand that the Komega model is best suited for aerofilols and turbomachineries but i dont understand why. Finally when trying to get a value for the Surface Heat Transfer Coeefficent out of ANSYS Fluent and CFD POST (+/) Xe16 which is very far away from the hand calculated value of 218.
Looking forward to hearing from you soon.
Best Answer

Rob UKForum Coordinator
The wake is formed by the buoyant plume (warm, less dense material rises). If you get the pressure bc's wrong (ie don't account for hydrostatic head) such that you get flow induced by the boundaries it can mask or reverse the buoyancy driven flows.
The near wall mesh will effect the heat transfer from the solid to the surrounding fluid. Given the motion is driven solely by the temperature gradients getting it right is critical. You also need to account for the flow and thermal boundary layer thickness: they can be different.
Answers
Please Pardon My Spelling mistakes
The reference pressure is used for pressure coefficient calculations, so doesn't matter here. I'd also suggest checking how each heat transfer coefficient is calculated in Fluent as we have 34 of them. My usual approach is to use the heat flux, and area from Fluent and then pick the temperatures that make sense to you as you would in an experiment and use Excel/calculator/piece of paper to find the HTC.
The only other thing to watch is gravity and operating density to prevent the water moving due to height effects. Look at section 7.3.1.5 and I'd suggest making sure that rho_0 (operating density) is exactly the same as rho_s.
Re the turbulence, RNG ke with buoyancy terms on is recommended if it's turbulent. I'd also extend the profile to be larger than the temperature range you're modelling.
Good Morning. When I do that I do get the currect values for the heat transfer coefficent as my imperically calculated values I don't how ever see the convective effects Illustrated in the models above. I see no convection in the velocity Contour and No fluid Build Up at the Bottom of the pipe. Why does Changing the Way Pressure is modelled have an effect on the expected convective effect and the total heat tranfer rate?
It's not the pressure, it's the operating density that's being fixed. Check the documentation section I suggested, the flow is a result of rho_s  rho_0 not being zero and you not calculating the exact pressure on each bc. It's not zero it's a function of the height and density difference, so the bottom boundary will have a pressure of a few pascals more than the top, the sides are then a variable value based on position.
Are you then suggesting that the pressure gradient is what is preventing the observed convection wake when i dont model hydrostatic pressure. i have gone through the document and understand what you mean with regards to rho_o , what is confusing me is why changing the hydrostatic pressure affects the presense of a convection wake I have observed in previous simulation. I am aslo no wwondering if I am using the correct inflation layer set up. When i use a total thickness inflation setup and specify the thickness to 20mm I reach steady state much later in my simulation I also get a much larg much larger range for total heat flux and the wrong final value. Where as when I use a first layer thickness Specification at 5mm for the first layer; I get the correct value for Total heat Transfer rate and reach steady state in the faction of a second. I dont understand why there is such a variation ?
The wake is formed by the buoyant plume (warm, less dense material rises). If you get the pressure bc's wrong (ie don't account for hydrostatic head) such that you get flow induced by the boundaries it can mask or reverse the buoyancy driven flows.
The near wall mesh will effect the heat transfer from the solid to the surrounding fluid. Given the motion is driven solely by the temperature gradients getting it right is critical. You also need to account for the flow and thermal boundary layer thickness: they can be different.