Buried water pipes - Heat Transfer

[dalibormiskov]

Hello,

I would like help for setting up the CFD model (Buried in ground water pipes) because I tried many times and i receive bad results with constant temperature of the water throughout the pipe.

On inlet i set

Velocity 1500mm/s, on outlet P=0 Gage

Ground Total Temperature is 1° Celsius

Water Static Temperature 15°

Film coeff. on the outside Surfaces of the Polyethylene Pipes 5000W/m2*K (is this coefficient OK or not)

 Initial Conditions

Ground Total Temperature 1° Celsius

Water Static Temperature of 15°

2 Simulations are conducted

With the first Simulation I only solve the Flow, with the Heat Transfer, Radiation and Autoconvection OFF, when the graph is converged, I continue with the second Simulation for Heat Transfer with Heat Transfer, Radiation, Gravity and Auto Convection ON and Flow is OFF.

I don't know if the result is reliable.

Thank you in advance, Dalibor Mishkov.

[Jon.Wilde]

Hey,

There are a few points to make here 🙂

Firstly, the most important question - what are you trying to do/measure/achieve here?

Then, some points

• Inlet should have a flow rate and temp
• Outlet P=0
• There should be no internal boundary conditions - it sounds like your film coefficient is one of these. Delete it or don't mesh anything surrounding the pipe - CFD will calculate the film coeff for you depending on material properties and local temperatures.

• Initial conditions are not necessary unless you are running transient.

• Why not just solve flow and thermal together? Or run Auto Forced Convection, which automatically runs them in series. This is OK to do here I think as your flow and thermal results are not affecting each other.

Hope that helps,

Jon

[dalibormiskov]

Hey Jon,

I will answer in order as you asked.

1. I want to see the Temperature difference between inlet and outlet, or with other words how much Celsius Deg. the Water will lose through this 1 m Pipe.

2. Inlet and outlet is clear now.

3. I have more Sub questions for the Film Coeff. and the Mesh around the pipes

• Because I have CAD model of Soil (Ground) around the pipes and the pipes are buried into the ground, that means that I don't need Film Coeff.??? Please for Reply.
• As I understood you said that I eather have to delete the Film Coefficient or to leave the Film Coeff. and delete the Mesh applied to the Soil (Ground). If that is as I above stated, how without Mesh on the Soil the Heat Transfer between the Soil and the Pipes will be Calculated, or that is in the Software like this implemented?

4. I'm running Transient (20 Seconds) and because of that I think that I have to separate the Flow Analysis from the Heat Transfer Analysis.

5. I will try to solve them together and I will give you Feedback.

Thank you, Dalibor.

[Jon.Wilde · Accepted solution]

Hey Dalibor,

OK, a point to know - pipe flow is actually quite difficult to model (and much easier with a hand calc). To properly capture it in CFD and match hand calculations, we need to ensure we have fully developed flow upstream, before the fluid reaches the area of interest, or we are nowhere near realistic.

Check out this article for an idea of the inlet length you need: Inlet pipe length.

Can you also use 1/2 symmetry here? I suspect yes 🙂

Yes, you cannot assign a film coefficient if you have the soil modelled. CFD calculates this for you as above 🙂

OK on the transient solution, then running flow first 100% makes sense, nice work!

Thanks,

Jon

[dalibormiskov]

Hallo Jon,

I made Hand calculations but I wanted to confirm them with the CFD. Yesterday I made the Simulation as you said and it worked. Thanks.

I compared the Simulation results to the Hand Calculations and it was only 1% difference. Were many Conductivity coeff.(X, Y and Z direction) for Soil and I simply took something average.(1,5 W/m*K). For specific heat 890 J/kg*K, also something average.

I left the Simulation to almost full convergence  ( see Picture and .csv attached) if you mean of that (Fully developed flow upstream)

I think the results are looking promising.:)

I will check about the Inlet length.

Good Idea, I will use symmetry 1/2 (vertical)

I removed the film coeff. Thanks.

Originally my model is 70m Long pipes(4 Pipes) that will suck water like in the Airplane Toilets:)). But for me is important how much will be the temperature difference between the inlet and the outlet. When the temperature loss is bigger I will consider insulation also.

I tried to mesh the whole model but my Computer doesn't have so much RAM Memory. I will try now with coarser Mesh for the Soil,and Little bit finer for the Pipes and the Water and all that in 1/2 symmetry. Hopefully my PC will be able to calculate that. (Gaming Laptot G750JX 8GB RAM, CPU:Intel Core i7 4700HQ @2.4Mhz)

Thank you very much Jon.

Have a nice day, Dalibor.