Hi I´m studying at the University of Kalmar. Sweden. I´m working on optimizing an ejector pump. I think the only way to do this is with computer simulation. I´m using ANSYS ED 5.4 It simply doesn´t work and NO ONE at the University knows the CFD part of this software.

First, to verify that my bounadary constraints and everything else is correct, I´ve created a model with the same dimensions as the real ejector they are using right now. If I´ve done everthing right my model should give the same flow as the real ejector does, right?

Well, it doesn´t. The flow in the computer becomes 2-3 times greater then the real flow. I´ve tried everything!(allmost) What is wrong?

I´m using an axisymmetric model with the FLOTRAN Fluid 142-element. the fluid is water. incompressible turbulent flow. If anyone could give me just a small tip som that i could solve this problem I would be VERY thankful. If someone wants, maybe I could email you the model(554 KB, compressed). It´s a little bit difficult to give a total description of the problem in text.

Thanks in advance / Erik Walfrdsson, Sweden

Hi Erik; Below are some point which may help: 1-Are you solving 3-D? If Not then you may switch to Fluid 141 with choosing axisymmetric at the begining. 2-Check the turbulemce parameters well such as the turbulence intensity for example 10%, the turbulence inlet scale factor,and the turbulence ration (for ex. 100000). 3-Check the relaxation factors (for example relax,visc,0.1,and relax,evis,0.1), and stability parameters such as (stab, mome,1.0 ,stab, pres,1,stab,turb,1,and stab,visc,0.1. 4-Make sure that the solution you got is the converged solution. AT the converged solution, there is no significant decrease in the normalized ressidual and all the variables are monotonically decreasing. 5-Check in the filename.pfl for the mass balance which should be almost equal. FLOTRAN will give you mass in and mass out.

GOOD LUCK Ramadan

(1). I am not trying to answer your question related to the code. ( the last impression I had on the code was the solution did not converge after three months on the computer. a semi-joke.) (2). In general,there are two ways to simulate the internal flow problems. (3). The first one is to specify the inlet velocity profiles completely. The other is to specify the inlet total pressure and exit static pressure. This one is good for compressible flows. (4). So, for incompressible flows, it is easier to specify the inlet velocity profiles. And, if you specify the velocity profile at the inlet, your mass conservation problem should be solved. In other words, you run the ejectorpump problem as if it is a two stream mixing problem. You specify the velocity profile at the primary flow and the secondary flow. (5). This will change your problem into a two pumps flow problem. Then the next thing to do is to adjust the secondary flow velocity, run another calculation, until your ejectorpump condition is achieved, that is the pressure conditions meet your operating conditions. (6). This is assuming that the code is in working conditiion. To find out that, you need to do some benchmark case testings on the code first.

i also had many problems using Ansys for fluid analysis. i think your grid must be structured. ie you have to use mapped mesh. i could not do this for my problem so i could not get properly converged results. you haven't said how your results are converging. if they aren't then the range of problems is wide. if they are then you probably have bad boundary conditions. bad turbulence parameters should not give you the magnitude of problems you describe. try running laminar and see. all this is just my speculation. my best suggestion is to contact Ansys and see if they will help. i know student versions don't come with support but if you plead (beg, grovel etc) they might help. or better yet find someone who has a full liscence and put the problem to ansys thru them. now that i think of it perhaps because you are limited in the number of elements in the student version you may be suffering from inadequate mesh size. however you can overcome this so i don't know what to say

(1). I have received your e-mail and the velocity plot of the ejector pump flow field. (2). the configuration is horizontal, so I think, the body force of the water (weight) is not going to affect the results. If you position the ejector pump in the vertical direction and wish to consider the body force effect, you need to find out how to include the effect first. (from the user's guide or contact the vendor. Since I am not a user of this code, I can't help you in this area.) That should take care of the body force, rho*g*H term. (3). You said that the limit on the mesh is 2000 points (or cells), so, you could try several mesh arrangement and check the effect on the results. From the plot , it looks like that you have 10 points in the radial direction. You can increase the grid points in the radial direction first. This is important, because the ejector pump is based on the principle of momentum mixing. Without the mixing, the jet will remain as a jet. (4). To capture the mixing process, you can increase the mesh density in the location r=r,center jet. That is put more points in the mixing zone around the center jet lip radius location. The mixing zone will spread out and reach the wall to complete the mixing process. So, you must capture this process properly, otherwise, the device is not going to work. (5). For the mesh distribution in the axial direction (in your application, it is vertical upward direction ), you can stretch it from the lip location with finer grid size near the lip and coarser grid size toward the exit. (6). It is a good idea to study the jet spreading behavior (and spreading angle of the mixing zone), so that you can arrange the mesh to capture the fine feature of the mixing zone. This is important, because you want to have a long enough pipe length for the mixing zone to reach the wall and complete the mexing process. (7). You have to run this case as a turbulent flow case. (8). So the key to the answer is to mesh the mixing zone properly with long enough pipe length to capture the mixing process which is essential to the operation of the ejector pump. (9). You can also run a check case using laminar flow with a Reynolds number set equal to 50 or 100 based on the jet diameter and velocity.

(1). In CFD, one of the most important issue is the mesh independent solution. Because that is the begining of design and analysis. (2). Without the mesh independent solution, the discussions about the design and the analysis using the computed results are useless. (3). Using a code limited to 2000 nodes, a student would not be able to draw any useful conclusion from the computed results. Thus, nothing could be learned. (4). I think a student should at least use a standard version of the code, so that the skill learned or knowledge acquired will be useful later on. (5). In my opinion, using a 2000 nodes code can only hurt the users and the impression on CFD by general public. (6). If a brain surgen can only use a very crude model of the brain in school training, he is going to have big troubles working as a medical doctor later on.