# how can I set up the boundary

 Register Blogs Members List Search Today's Posts Mark Forums Read

 June 5, 2008, 03:30 how can I set up the boundary #1 pdz711 Guest   Posts: n/a As the follow picture depicts,there is a problem that can be simplified to internal flow of siphon discharge passage,I want to konw the velocity and pressure distribution in the siphon passage.how can I set up the boundary conditions?Can water surface be set up to "pressure inlet",passage outlet be set up to "pressure outlet". [http://i290.photobucket.com/albums/l.../Drawing2.jpg]

 June 6, 2008, 06:11 Re: how can I set up the boundary #2 Victor Guest   Posts: n/a Hello, I think you can have two different approachs for the solution of this problem, i'll talk about the simplest first: (1) Supposing you have a given H, you should "cut" your water tank under H, let's say, 0.7*H, and set a "pressure inlet" BC there. You calculate the pressure by yourself using: P_inlet = P_atm + rho*g*(1-0.7)*H And you set the outlet BC as "pressure outlet" with the value of atmospheric pressure. It's a simplified solution, as you'll assume that the level of the water never changes, and you'll finally have a steady solution for the flow through the siphon. (2)If you're interested in the whole unsteady solution, with the variation of the level of water, you'll have set a VOF (volume of fluid, i think that it's the best model in Fluent to use, but I'm not quite sure) simulation. I'd "cut" the water tank above H, let's say 1.4*H, and then set a BC of "pressure inlet" with atmospheric pressure as the value, and air as the entering fluid. And then you'd initialize the domaind between 1.4*H and H with air, the rest with water. For the outlet BC you'll also set as "pressure outlet" with the atmospheric pressure value. --- You just have to decided if you're interested in the whole unsteady simulation of just the solution when the level of the water is H. My best regards, Victor

 June 6, 2008, 10:08 Re: how can I set up the boundary #3 pdz711 Guest   Posts: n/a Thanks very much for your help,I have done some works on your advice.because the pressure increase with depth,I set up the pressure inlet by UDF.Would you give me some advice again? As the follow picture depicts,The left is water,the depth is H and H is constant,the distance between water and outlet is h,the height of the outlet is D.In the "pressure inlet" interface,I define "gauge total pressure" by UDF,"supersonic/initial gauge pressure" is set to 0. [http://i290.photobucket.com/albums/l.../Drawing1.jpg] UDF: #include"udf.h" DEFINE_PROFILE(pressure_inlet,thread,position) { real x[ND_ND]; real y; face_t f; begin_f_loop(f,thread) { F_CENTROID(x,f,thread); y=x[1]; F_PROFILE(f,thread,position)=998.2*9.81*(h+(D/2-y)); } end_f_loop(f,thread) }

 June 6, 2008, 12:07 Re: how can I set up the boundary #4 Victor Guest   Posts: n/a So you're setting your inlet at the the entrance of the siphon (i.e. where the diameter turns do D)? I thought you'd like to simulate the flow a little bit before entering the siphon... But if you're interested only in the flow in the siphon, I think your setting is ok, but you're going get only a approximate steady result, and I think you can get a better solution but adding some simple stuff. Let me tell you what I think you could to improve a little bit your simulation. I've made some modifications in your drawing: http://www.flickr.com/photos/90857689@N00/2555638251/ So, now we have the inlet away from the entrance of the siphon, with that we'll have a better velocity profile that enters the tube. You'll have to set a(0) (beggining of the simulation, now we're unsteady). It depends of how long you wanna simulate... If you set a(0) too small, the level of water (i'll explain it) will soon approach it, and then you'll have to finish your simulation, but if you set it too big you have the inlet too near from the siphon entrance, so you'll not have the best discretization in that region. It's up to you to decide! For DD, you have to think that if you have a DD too big, you have a larger simulation domain where you're not interested in the solution, and will just consume CPU time. If you have a real geometry to compare, that would be useful for you to have a more strict geometry. Now it's the important part: we can simulate a H in function of time via UDF. The inlet will be physically static, but as a(t) will change with time, as a result of a variation in the level of water, you'll just have to change de hydrostatic pressure for the inlet boundary. First you find the a(t), with the resolution of this differncial equation: da(t)/dt = a(0) - V_waterlevel As you have a incompressible flow, V_waterlevel is equal to V_inlet, so you can take if from the Fluent solution. The solution of the equation can be something like this: a(t) = a(0) - a(t-1) - V(t-1)*dT Where dT is your time-step size. For V(0) you're normally have zero, but you can change it depending in what you want. And then you can calculate the pressure inlet with the ordinary hydrostatic equation, but now using the a(t) that depends on time. Something like this: p_inlet(t) = rho*g*(a(t)+D/2) I hope it could be useful. My best regards, Victor

 June 7, 2008, 04:14 Re: how can I set up the boundary #5 pdz711 Guest   Posts: n/a I have studied your advice today.If the water volume outside the siphon entrance is limited,the methed you give me is good.In my problem,outside of the siphon entrance is sea and its volume is huge and invariable in the whole process,it means depth H is constant.so I prefer to consider that the flow is steady.In steady case,the inlet boundary can also be defined in water surface,Do you think which is better? In my next work, unsteady simulation is indeed needed.in this case the outlet of siphon is connect to a container.when water depth in the container rise,the effective water depth(sea water depth â€" container water depth) decrease and velocity distribution in the siphon alter.But the total flux in unstead process reach to 300000m3,we should use VOF on top of huge container which have volume of 300000m3. I am afraid that my computer(P4 3.0G+2G RAM) can not afford the simulation.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Thomas FLUENT 1 June 17, 2008 05:14 A. Al-zoubi CFX 0 November 3, 2007 08:11 Shukla Main CFD Forum 3 November 11, 2005 16:02 dalton Main CFD Forum 12 April 3, 2005 23:52 AFP Main CFD Forum 0 January 30, 2004 08:16

All times are GMT -4. The time now is 03:25.