Pump Water Flow inside a pool
 

Hello, I want to simulate how the water flow inside a swimming pool when a water pump is placed inside the pool. The pump has been created by establishing the pool as a fluid domain and the pump is subtracted using Boolean. For the boundary conditions, I have used one side as velocity inlet and other as pressure outlet and used meshing as element order quadratic with 300mm size. I have used the pressure solver and the k-epsilon model. The result is attached below but it somehow does not look sensible. Please give me your suggestions on where I went wrong or how I should have done it better?

Pump
 

It appears that you have modeled the pump as a simple box, which is not bad, but then the solution would be according to the assumption. 300 mm is quite a large size for turbulent flow. You have to use smaller size, at least an order of magnitude smaller, i.e., 30 mm or may be 50 mm. 300 mm is used for atmospheric flows but water has much smaller kinematic viscosity and a lot can change over 300 mm. As far as the flow-field is concerned, if pump is modeled as a box, then the results are alright provided the case has reached convergence.

Hello,
Thank you for the reply. For the pump, I have modelled it using a cylinder with diameter 0.3m and length 0.6m where the two faces acts as velocity-inlet and pressure-outlet. As the boundary condition I used a velocity inlet of 2m/s and pressure outlet 0 Pa. The swimming pool domain has been meshed with element size of 300mm, adaptive sizing and inflation on. I have some question: when you say 300 mm for turbulent flow, you mean that i should mesh the entire swimming pool fluid domain with that element size of 30 or 50 mm? Also, even when I ran the analysis for about large iterations, the curves are not converging and the vector flow is also not symmetric. Please suggest me what I should change to get an accurate result. Thanks in advance

Objective
 

It all boils down to the objective of the simulation. Cylinder or box, which I mentioned, essentially mean the same thing; a simplified representation implying study of pump is not the motive. So, do you want to observe fluid flow in the pool? And if only the boundaries of the pump are being modeled, why there is flow inside the pump region? Or is it that my understanding is incorrect?

Yeah, it got it right. I want to observe the fluid flow in the pool, how it circulates in the pool. there is no fluid flow inside the pump, the one you see in the zoomed figure is on the pump wall. I displayed the velocity-inlet, pressure-outlet, and pump wall while checking the velocity vector field. So that's why you see the blue arrow on the circumference. I tried to create 30 or 50 mm element size for the pool domain but the meshing takes a long time. (it does not finish) because the fluid domain (pool) is too big (25x18x2m), also I have a limitation on the student ansys version. Is there any way I can get the accurate results and still be inside limit?
I am really stuck in this now

Mesh
 

Generate a finer mesh close to the inlet and outlet of the pump and coarser away from it. The fineness closer to the pump depends on the size of inlet and outlet. There should be at least 48 nodes around the circle that represents inlet (or outlet). Furthermore, you might be able to use vertically symmetry if the pump is in the center of the pool.

Thank you for your reply. I did use a fine mesh for the pool with an element size of 100 mm throughout, adaptive sizing on and resolution increased to 6 (near the max), so the mesh nodes were close to 3756989 nodes. I ran the iteration to 500 and 1000 iterations and the image looks like this. One quick question, should I be using pressure based solver or density based solver and steady analysis or transient analysis? once again my motive is to see how the fluid flow in the pool

Flow
 

You forgot to attach an image. You should use pressure based, steady-state solver. Density based is meant to be used only if Mach > 2 or at least with compressible flows, i.e., Mach > 0.3. Every flow is transient, however, what you want to observe is steady flow field. So, no need to run a transient case.

Sorry here are the images. As you can see the iteration curves are not converging even after 1000 iterations. Can you advise what should I do??

Boundary Conditions
 

You have to change your boundary conditions to represent reality better. The outlet of the pump, which is inlet for the pool, is being represented by velocity inlet, which applies a uniform velocity throughout the boundary. In reality, this is a profile, hence, you should apply a proper pressure or velocity profile instead of constant velocity. Output of the pool (inlet of the pump) is alright.

To get a realistic profile for pump outlet, you need to either get an experimental data or run another simulation to develop a profile. For that, you can take a long cylindrical duct of the boundary size and run case with turbulence model enabled. Then extract profile from the out of that case and apply it in your current case of the pool. This would be better than applying a constant velocity magnitude. Best would be to run a pump simulation but that would require more effort than could be justified.

How can i use the fleunt analysis output of one as an input into another fliuent analysis? can you please advise?

Output as Input
 

It depends on the type of output. For your case, you have to write a profile from first case and use that as input for the second case. Once you have completed first case, go to File > Write Profile and then choose New Profile, select the outlet boundary and then select the fields for which you want to write profile, i.e., velocity components and turbulence fields. In second case, go to File > Read Profile and this file. Then you can apply these fields at the outlet of the pump in the current case.