I'm trying to simulate water flow through a mini hydro power plant. My dam is 6 m high, and has a pipe with diameter of 0.5 m, situated 5 m from the top water level. For simulation purposes I have built model which consists of single object, square based prism 6 m tall, which has cylinder 0.1 m long, positioned 5 m from the top. There are neither turbines nor propellers, or valves. I have defined all boundary conditions of my water object as slip/symmetry, besides top input, and pipe output, which are both defined as steady state static pressure of 0 Pa. Meshing was done automatically. Simulation was started with Physics tab, Flow check box checked, incompressible, Heat Transfer checked, with gravity method Earth, pointed 0,0,1 (it seems that direction is inverted. Force is pushing water in –Z direction). This last part with Heat Transfer is also not clear to me. Is this correct procedure? Based on manual, heat transfer is used for buoyancy effects, but my model does not have heat sources?!? Simulation runs, and final result gives maximum water velocity in cylinder of cca 480 mm/s. This result is really strange. As I remember elementary school physics, potential energy on start should equal kinetic energy at the exit. So, m*g*h = m*v2/2, which gives v = sqrt(2*g*h) = sqrt(2*9,81*5) = 9,9 m/s, which is a lot bigger number compared to my 0,4 m/s.
What am I doing wrong?
I’m using Autodesk Simulation CFD 2013.
Sorry for my bad English.
If you look at your pressure contours, do you see pressure gradually increasing towards the bottom? This should ensure the gravity is setup properly. Can you attach a snap of your pressure contours?
This is the whole project:
Since initial post, I have decided to change boundary conditions from slip to velocity = 0.
This is pressure distribution, and distribution looks ok, but values are wrong.
1000kg/m3 * 9,81m/s2 * 6m = 58,8 kPa != 116 Pa
And there is this thing that gravity is reversed. Now it points in -Z, but simulation was done using +Z direction ?!?!?
As I suspected, the problem seems to be the pressure distribution and not the velicity being different than theoretical one.
Can you check basic things:
1) Boundary conditions and water properties (its density etc)
2) Dimensions of the geomdetry. It shouldn't be wrongly scaled.
3) Are you sure you got a mesh independent converged solution?
Since your "down" means negative Z, the gravity vector should be (0,0,-1).
I just realised, the top surface is not "free surface" in your case. You have enforced a zero pressure and zero velocity. Now, the trouble is, you are asking software to let the fluid go off the tank from bottom pipe, but not letting any fluid in because of top condition being zero velocity. This vilolets continuity. Even if you remove the top zero velocity condition and just keep zero pressure, you still won't be able to let the fluid out from bottom since there isn't adequate pressure gradient at the top boundary to let more fluid in, as the bottom fluid goes out. The whole situation is unphysical and unreal!
Free surface modelling includes modelling of two phases with interphase interactions being solved. Ideally you should have created a zone of air at the top of the tank, specifying it as air, while the fluid zone below it would be water, creating an interphase between water and air (Water level). As water goes out from the bottom, the interface (water level) lowers, filling in air from the top. Thus continuity is honoured.
As far as know, it is possible to do such a multiphase modelling in SimCFD. There may as well be a clever way to model this. You may want to post this as a case to Autodesk Subscription center.
I have not forced zero velocity condition on top inlet, only zero pressure. Gravity should push water through outlet, and create negative pressure at inlet; this should pull more water from the top.
I don’t understand what you are trying to achieve with air above water. Air should also have some sort of boundary condition, and then we are back at the beginning of the problem.
After some time I have decided to cut 1 m of water from the top of model, and assign calculated static pressure on this newly created inlet, 1000 kg/m3 * 9,81 m/s2 * 1m = 9810 Pa. This has resulted in considerable flow of water through outlet, but final flow rate was 30-40% less than calculated. Additionally I have done same simulation, but this time with Heat Transfer switched off (along with its definition of gravity), and I have got exactly the same result. This has led me to conclusion that SimCFD 2013 does not support gravity driven simulations.
Regarding Autodesk Subscription center, unfortunately I don’t have contract with Autodesk, therefore I cannot ask questions there. Do you maybe have ability to ask them what they think about my problem, .....
......or maybe somebody else is willing to help?
And OJ, much appreciated your interest in solving this problem.
I was referring to the free surface flow, such that, as your dam leaks the water from the bottom pipe, the liquid level in the tank will fall. Autodesk SimCFD 2014 has this feature now, as I read here:
The example of free surface flow there (you need to expand it) is similar to yours to some extent, driven by gravity.
I admit I mistakenly thought the zero velocity condition was specified at inlet, but as I observe your cfz. it is on the walls. That's strange! Not sure what you'd achieve with that. Keeping it regular walls (or slip/symmetry if you are simulating a section of dam) made sense.
As I think aloud, originally you had zero pressure gradient between inlet and outlet with inlet at 0 pressure (free surface of water). When the tank is emptying, water has to enter from top. But you can't expect water to be fed to your inlet if it is a free surface, which should start coming down. You have to model a free surface, which you can't do in 2013. So you need to tell SimCFD, that there is a reservior of water above that boundary. That's what happened when you chopped off uper inlet by 1 m, and then put a pressure worth 1 m of water on lnlet. Now, the boundary is more realistic, there is a pressure gradient across inlet to outlet, and there is a water at the top of boundary (as suggested by your inlet pressure).
To be honest, if you are interested in calculating just outlet velocity, this seems an adequate approch, instead of simulating whole tank. I tried your cfz file, cut your inlet still further such that the tank is now only 1.5 m high. Then I applied the inlet pressure as (9.81*1000*4.5=) 44145 Pa. I got the average outlet velocity of m/s, close to your theoretical value of 9.9 m/s. I have attached a snap.This seems a way forward, though I would recommend to keep more height than I chose, to avoid unreal situations.
Partly, the inaccuracy in your solution can be explained. Your mesh is really very coarse. You have used ADV1 advection scheme and using basic k-eps model. All these will extremely diffusive in nature and hence your solution will be inaccurate. Try using ADV5, RNG model to obtain a mesh independent solution. You'd have better results.
Anyways, your case is really interesting, so I did a bit of thought-marathon! Perhaps there can be better suggestiosn by Autodesk personnel. I have subscription priviledges, but on my company's account, which can't be used for cases other than those related to company. Sorry. But Autodesk personnel are active on this forum. If you persist, you may get more advice