# HELP..3D-pump optimizing using FLUENT/ GAMBIT

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 October 29, 1999, 06:06 HELP..3D-pump optimizing using FLUENT/ GAMBIT #1 Marcel Schmutz Guest   Posts: n/a Hi... I'm a student from the swiss ingeneering school of Biel. Perhaps also known from the solar races in austrailia. I try to optimize a hot water pump. The model is 3D. I got real big problems to get the geometri in, and to generate the mesh. I have to say that our HP- UNIX stations aren't the fastest one so I have to generat a non complex grid. So i'm looking for some people, which can give me some good tips. ==> how to get and clean up the geometri ==> Which typ of mesh would you take (tet, tri/pav,hybrid..) ==> Which wall- funktions and other settings and parameters. I would be glad to become some good tips of real professional because i got no support from my teachers. If it's a problem which isn't interresting for this forum so pleas send my your tips by mail

 October 29, 1999, 13:26 Re: HELP..3D-pump optimizing using FLUENT/ GAMBIT #2 John C. Chien Guest   Posts: n/a (1). What is a hot water pump? (2). What does it look like?

 October 31, 1999, 03:45 Re: HELP..3D-pump optimizing using FLUENT/ GAMBIT #3 tom Guest   Posts: n/a 1. I suppose it's a centrifugal-pump and you have the meridional contour and the pressure and suction side als iges-files 2. Calculate periodic and only the channel between the two sides 3. First try tetrahedral-mesh 4.Behind D12 extrude in radial-direction still about 1/8*D12 and make there the pressure-outlet. 5. Use velocity-inlet 6.You can use boundary-layers in gambit but my experience is, that it does not work in such complex cases with strong-curved pressure-side, suction-side, hub and shroud tom

 November 5, 1999, 12:23 Re: HELP..3D-pump optimizing using FLUENT/ GAMBIT #4 Francisco Saldarriaga Guest   Posts: n/a Marcel: the pump must have excess of geometry that you need to clean. My experience is that if you do all that in your drawing package and only import the necessary (wire frame and/or faces) geometry via .igs files, your making of the model with Gambit will be much easier when defining the blocks in the domain. It is at this stage that you do what John describes to generate the mesh. Because you have a limitation in computer hardware you could do only a passage but I my case I always want to do the complete impeller. It is a long process and you need to keep clear undestanding of your geometry and how the solver works in the control volumes. Must of all I assume you want to see counter flows and for that you need to grade and size the mesh properly. Can you explain in more detail your pump? fco.

 November 9, 1999, 10:01 Re: HELP..3D-pump optimizing using FLUENT/ GAMBIT #5 Marcel Schmutz Guest   Posts: n/a Ok...I'm sorry about my english...but I try to explain more. The pump is designed for industrial heating and climatisation systems. the pump works with a radial working pump impeller. It gots two numbers of revolutions..2780 rpm/ 2350 rpm. The performanc is between 640...1550/ 500...1150 (coresponding to rpm). m^3/ h is between 0...55 H is between 0...12 m here some geometrie infos: Outer limits: (b x h x l) = (265 x 340 x 384) [mm] Impeller: (d1 ; d2 ; z ; s) = (72 ; 105 ; 9 ; 2) [mm] I have to say that im not a absolut greenhorn, I know how to generat the geometrie. The geometrie contains a lot of non planar faces. I have to work with free form surfaces. After generating the faces I creat a solid body. I can export IGES surfaces, but i got some problem with cleaning up the geometrie. I tryed to change some parameters in GAMBIT like toleranc and vortexconection (allows deleting the short line between two vortex)...but i spend a lot of time in cleaning up the geom. When I got a solid body I like to use it, and I'm looking now to convert my PRO/E files in STEP and after this back to SAT. Like this I hope to have a file which is conform whit the kernel of gambit. And normaly you got less problems whit solid bodys, because you dont have the problem with non closed surfaces. And is there anybody out there who can tell me, that the automatic clean up modus in GAMBIT is working well?..normaly the system crashs. The second thing i wanted to know is how fine the mesh have to be...it depends on the results your interested in. If you only wand to have a first look on whats going on inside, sow a simple model is enough to visualize the path lines. But you have to build a real fine grid if you want to know the efficiency of your pump or other dates. And is there anybody who can tell me, wich is the range of validity of CFD. If you have a look on the pump, sometimes your geometrie properties are changing enorm.After the pump impeller you got a backflow throug the space sealing (impeller)...I hope you understand. And what the hell contains the Y+. It's something about the law on walls. It contains the speed and the shear stress. So when you got a backflow along the wall, the speed goes to zero and the Y+ colaps also to zero. I hope you know now more about my problems or should I say about my search for CFD- Infos. Thanks for the mails I became... Hope there are some more... Thanks to all....Marcel

 November 9, 1999, 12:03 Re: HELP..3D-pump optimizing using FLUENT/ GAMBIT #6 John C. Chien Guest   Posts: n/a (1). The centrifugal pump is a very common device, but the flow field is always 3-D and with some degree of flow separation. In other words, the geometry is complex (unless you are using a 2-D blade design) and the flow is even more complicated. But it is an important and widely used device. (2). After having said that, I think, there are several approaches one can take to simulate the geometry and the flow field. (3). The solid modeling in CAD is good for a group of simple geometry. It is not good for complex geometry. My approach is always the bottom up approach, that is defining the points, the curves, and the surface. For the structured mesh or volume, one needs to plan ahead, similar to the lego toy method. In other words, try to cut the flow field into small six sided blocks, from the inlet to the exit. The same method can be applied to the back side cavity region. I have used this approach with unstructured mesh with great success for very complex radial turbine and pump applications. ( I have not actually used the Gambit/Fluent5, but I have used the Prebfc in the past. I think, any CAD/mesh generation codes should have the basic bottom up tools, point, curve, surface...) (4). So, in the geometry generation area, I would recommand the use of the surface mesh approach rather than the solid geometry modeling. In this way, you will have the complete and connected surface model. You can then use the automatic meshing tools to generate the surface and the volume meshes. (5). The problem with the radial machine is that due to the relatively thin balde leading edge, and its sensitivity to the relative flow angle (mass flow, the rpm and the radial position), the flow is always 3-D and with flow separation. So, the radial pump flow is actually the most complicated internal flow problem. (6). In the turbulence modeling area, ideally, you would like to use a low Reynolds number model, or a two-layer model. This will eliminate any uncertainty about the use of the wall function. But this will cost you a lot of mesh points, especially you are dealing with 3-D flow. There is no simple way out. At the same time, you can always try the wall function version to check the results. (7). As for the range of validity of CFD results,for simple flow problems, it is fairly accurate. For the complex problem like the radial machine, it is more reliable to predict the efficiency using the traditional empirical formula approach. (8). The use of 3-D CFD appraoch in radial machine analysis is still relatively new. So, it will take a while to overcome the limitations on the computer memory and the turbulence model.

 November 9, 1999, 15:59 Re: HELP..3D-pump optimizing using FLUENT/ GAMBIT #7 Jurek Guest   Posts: n/a Cfd-calculations of centrifugal-pumps are a very very hot thing. It is no problem to show you, that it is not possible: 1.) You should use a two-layer-model ->lots of cells 2.) Shouldn't you use Reynolds-Stress ? The fluid-flow is strongly curved .. 3.) If you calculate one channel as I said at an other topic you sometimes get backflow at the outlet. -> bad convergence, and is this situation (p=const) correct at all ? That means, you should calculate the whole machine -> lots of cells 4.) What about the typical models for rotating machines ? I heard, that behind the blades (if the fluid is still in moving referenc frame) still energy is added to the fluid. If you make two fluid-zones at D12 you will often not satisfy the condition for that interface: the fluid-flow has to be "balanced-out" there. You will have even backflow over that interface. Mixing-Plane provides also convergence-problems -> You should calculate to time-dependent with moving-mesh ... You see, it's not easy. I for myself even calculated an efficiency of 110%, so I thought of an turbine behind the pump... Conclusion: The quantitative results of such calculations are often very poor and the calculations are better done by hand. Nevertheless you can get good qualitative informations about the fluid-flow inside the pump.

 November 9, 1999, 17:05 Re: HELP..3D-pump optimizing using FLUENT/ GAMBIT #8 John C. Chien Guest   Posts: n/a (1). Great, you have said it all.......(2). By the way, it took a life time of two great females to fight for women's right to vote. It was realized many years after they died. (3). I think, technical issues shouldn't take that long. But one still need to start from somewhere.

 November 9, 1999, 20:35 Re: HELP..3D-pump optimizing using FLUENT/ GAMBIT #9 Sigve Gjerstad Guest   Posts: n/a I have to say this is a most interesting discussion. My final year theses involved modeling a centrifugal pump at which we were interested in how well a one-phase CFD calculation could predict cavitation at the leading edge. What I found while doing this project was that resolving every phenomena in a centrifugal pump in one single calculation is like wishing for Christmas in january. It is very difficult and very CPU time demanding and probably a waste of time. I agree with that using CFD for improving the efficiency of a radial machine is not the way forward yet....Because the empirical method gives us a good answer. However CFD has proven to be very good in addressing and identifying areas of problem such as cavitation, resirculation, secondary flows and stall. This is areas in which the empirical correlation's don't give you an straight answer. so you need to be asking yourself: "What do I want to optimize?" Because optimizing the whole pump is going to take you a lifetime. PS. I found that modeling one single channel with a K-E model and a relative dense grid gave a good solution. (To my problem at least) Sigve

 November 10, 1999, 03:16 Re: HELP..3D-pump optimizing using FLUENT/ GAMBIT #10 Jurek Guest   Posts: n/a Hy John and Sigve thank you for your comments. I think a big problem for cfd-engeneers in centrifugal-pumps is, that you do not have much information of the "state-of-the-art" in this area. If you read cfd-online you think: Oh my god, my y+ is very bad, I have backflow at the outlet, I have to make the model in 1 day and then calculate Q/Qopt=1 the night, because in pumping-industy is not as much money as in gas/steam-turbine-industry, I only can use standard k-eps, the mesh is not very good and the convergence is often also not very good and beside this I cannot calculate Q/Qopt<0.7 what the much more interesting flow-situation is, because at Q/Qopt=1 and an efficiency of 95% you can calculate the impeller frictionless with much simpler codes with very good results. It was big big (psychologic) help for me to read some weeks ago an article from a pump-guru about cfd in centrifugal-pumps: He wrote, that it is still a long long way ...and he presented some results of cfd-calculations. Does anyone know of an article or something like this about: "cfd in centrifugal-pumps, what's possible today ?". Can I read your "final year theses" or is it secret ? Centrifugal-pumps and cfd also is not very "academic", you do not find much articles about this. Quality of results: Sometimes they are very good, sometimes they are very bad. But often the good results are at machines, where an experienced designer sais, that it is an "easy" machine whereas at "difficult" impellers (in the cases where cfd is really needed) the results are often bad. Jurek

 November 24, 1999, 09:47 Re: HELP..3D-pump optimizing using FLUENT/ GAMBIT #11 Marcel Schmutz Guest   Posts: n/a First of all thank's a lot for your answers. I'm trying to involve all your ideas in my next models. Next week I'll start with them an we would see what's going on... ....marcel

 November 26, 1999, 18:16 Re: HELP..3D-pump optimizing using FLUENT/ GAMBIT #12 jurek Guest   Posts: n/a recently I heard from a cfd-guru: the calculation of a (centrifugal-) pump is more complicated than a whole airplane.

 November 26, 1999, 22:55 Re: HELP..3D-pump optimizing using FLUENT/ GAMBIT #13 John Chien Guest   Posts: n/a (1). I would say he is right. (2). 3-D turbulent, internal flow with separation is very complicated. (3). In the airplane aerodynamics, the free stream is always uniform and the only problem is the boundary layer on the wings and fuselage. (4). There will be flow separation at transonic speed and high angle of attack. But those are exceptions. Inviscid codes and boundary layer codes used to be good enough for the aircraft aerodynamic design. I would say these codes are still being used, even though Navier-Stokes solutions for a full configuration has been in use for over ten years. (5). So, don't under-estimate the degree of difficulty related to the simple pumps.

 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 kharnabnew FLUENT 0 October 5, 2010 09:33 Ralf Schmidt FLUENT 2 February 25, 2009 22:35 Steve Johnson FLUENT 0 February 8, 2009 15:21 Vincent Ryan FLUENT 2 January 11, 2009 08:34 Bo Jensen FLUENT 1 January 17, 2003 10:55

All times are GMT -4. The time now is 10:59.

 Contact Us - CFD Online - Top