Hi everybody. I simulated steady flow in a Francis turbine with the following bc:

Inlet massflow + cylindrical velocity components from experimental data (BC interpolation file).

Outlet with average pressure imposed.

I find a very low torque compared to experimental (about 4 %). Can you suggest me why? I used k-epsilon and SST with hexa mesh and good y+ but no changes I found! Always the same error!

Thank you

Have you checked your scales, fluid properties, proper dimensions, mass flow rate, etc. Also make sure you have properly accounted for the number of sectors you are modeling.

I wouldn't expect an exact agreement with experiment, but 96% error suggests a problem with the setup.

-CycLone

Hi,

scales, fluid properties, mass flow rate, ect are correct. I think the problem is about inlet location. If it's too near the blade probably the resultes are modified. Now I try to move it away. Outlet is very far from the blade but I imposed an averaged pressure value. Can draft influence pressure profile on the outlet so as justify this difference?

Regards

Hi, if you are changing the location of your inlet, you should pay attention to the flow angle at inlet. It should be kept the same. As a rough approximation, if you are not calculating the whole turbine (i.e. spiral case, stay vanes and/or guide vanes missing) you should keep the product (radius * tangetial velocity component) constant, it means, model the tangential component as a constant vortex, and the angle will be kept. Remember to adjust the normal velocity component to keep the same flow. The draft tube should have minimal influence in the integral results, such as the torque. Check if your velocity components are compatible with the referential in which they are defined. Check also the runner rotation speed. Finally check if you set the correct runner rotation direction and if the blades orientation agrees with it, it seems simple, but this a more common mistake than one can belives.

Hi, I set the mass flow rate at inlet and cylindrical directions for velocity: axial direction is zero while radial and circumferencial are set as -sin(alpha) and cos(alpha) respectively, where alpha is the mean value of flow angle downstream guidevane. I simulate only the runner. I'm sure rotation direction and value are correct. I can't explain why I find this difference! I simulated the GAMM Francis turbine (see http://lmhwww.epfl.ch/Research/EVA/Gamm_files/Gamm.pdf). I used the correct geometry and inlet and outlet used for measuraments. I find a very different Cp distribution at inlet and a torque 4% less then experimental! Where do I wrong?

Regards

Hi, I took a quick look at the GAMM turbine. I could not find the machine nq (and I didn't really want to calculate it based on psi and phi, sorry!). But if the model turbine cross section in the report corresponds to the real machine, I guess it has a high nq for a Francis turbine. In this case, the velocity profile along the guide vane height (i.e. machine axis direction) will definitely not be constant! If that is the case, a simulation including the guide vane and a stage-interface could deliver better results. Including also the stay vanes will improve it, but not as much as by including the guide vanes. If you are using the mesh depicted at the end of the report, it doesn't seen so fine, specially in the runner, near the hub. In this region the flow might be not so "well-behaved" for an old machine with high nq, although it should not contribute significantly for the torque, because of its radial position. Assuming once again that the cross section corresponds to the real machine, it seems to have an old design, therefore there might be unexpected features in the flow, such as cavitation and separation, then a good turbulence model and a very good mesh would be required. However, near to the optimum point it is unlikely to occur (only in the case of a very poor design). In my personal experience CFX could predict the torque with less than 1% deviation, although it would not be so accurate for the head, influencing efficiency (some calibrate the turbulence model constants to improve it, but I can't help you with the values). The dynamic effects could also slightly influence the results, but it should not be observed for the torque. To sum up it all and to make it simple, I would try it with the guide vanes.

Hi, nq is about 80! I didn't use that mesh. My mesh has about 500,000 hexa cells with good refinement near walls with an averaged y+ value about 30. I have already simulated other Francis runner with guidevane and stayvane (not GAMM yet) but I didn't see any differences. I tried with stage rotor (because I have always 24 guidevanes and 13 runner blades) and with frozen rotor but I find a torque less then experimental. For low mass flow rate the error is up to 10%! I'd like to simulate only the runner and to have results according to experimental measuraments. I accept a 1% error on torque but not 4%! I have just a question for you! I have a Francis runner and I know only mass flow, head and rotational speed. Up to now I set mass flow at inlet with a test value of alpha angle and an averaged pressure value at outlet. So I changed alpha value until I found a torque on the runner equal at what I aspected. About your experience is this a correct way? About last GAMM Francis results I think I wrong all up to now! What do you suggest me? Thanks for your time.

Regards

Hi, if you simulated other turbines with low nq and you didn't see significant differences with the addition of the guide vanes, it is quite reasonable. But if you have simulated machines with high nq and the guide vane causes no changes, I would be surprised. With high nq, for Francis machines, the flow is not constant at the runner inlet. The flow is pretty higher near to the crown for new designs. Taking a quick look at the GAMM measurements at inlet, there is also a kind of such a tendency, although it is not so evident. But the measurements show that the flow at inlet is not constant. So, I would suggest to include the guide vanes in the simulation. If you don't feel like spending time in preparing its geometry, its mesh and changing your simulation, a work-around could be to move the inlet really far away from the runner, but accuracy can still be affected and you are looking for something below 1% deviation. About modelling the interface between runner and guide vanes, the stage-interface might deliver better results than frozen rotor, as it roughly reflects the mixing effect at runner inlet. But there are people who prefer frozen rotor. Changing the velocity inlet angle to get the correct torque value would not be recommended. Your need to test different values of this angle is because the flow angle at the guide vanes outlet doesn't exactly correspond to the geometric opening angle. Moreover, in a numerical simulation, if your changing the guide vane opening, your are changing the head, than you are calculating a different operating point in your hill chart. For small flows, or partial load, the flow becomes progressively fully unsteady. With 80% flow of the rated, CFX could deliver results with more than 2% accuracy. But for flows below 70% or even 50% of the rated, you should already be happy to have converged results for a steady state simulation. About convergence, the CFX defaults might not be sufficient for some turbine geometries, try a smaller value and monitor some important flow features, during the solution stage.

Hi, I simulated stay-vane and guide-vane too with stage interface. I set inlet mass flow and I used 29 deg angle as the GAMM report suggests. I find 4.5 % error on torque. I haven't still understood where I wrong. Is it correct to calculate power as omega*number of blades*torque_z()@Blade (where z is rotation axe)? I used also default turbine macro in CFX and I find the same value for torque. So I don't know what think anymore!

Regards

Hi, your procedure to calculate the torque seems to be correct. It was not real clear if you used stage-interface between guide vanes and stay vanes, there you could use GGI if their number is the same. Well, to verify your simulation try the following: 1) Check that your geometry is IDENTICAL to the GAMM turbine. 2) Check if the guide vane openning and the flow correspond EXACTLY to your operanting point in the hill chart. 3) Check the water properties (density and dynamic viscosity), they MUST be the same as in the model test. Do not approximate them, use the exact values, it can influence your results. 4) If geometric information of the GAMM turbine is available, check if the inlet angle at the stay vanes is really 29 degrees, although it is given in the report. 5) Check your mesh quality (distortion and so on...). 6) Check the solution convergence: small residual values, stable convergence. 7) Add monitor points for the partial head, flow at outlet and torque, they must also smoothly converge. 8) Check if your flow at outlet corresponds to your prescribed value. 9) Be sure that your outlet is not too close to the runner.

Hi, I used stage rotor whit automatic pitch change and GGI as mesh connection method because runner has 13 blades while guidevanes are 24. Now I'm trying with frozen rotor for different runner position relative to stayvane. And then I get a mean value of the torque but first results aren't encouraging (I find about same value of stage rotor).

1)I'm sure my geometry is correct. I checked it more and more times.

2)Guide vane opening is correct and it's 25 degrees.

3)GAMM report doesn't specify density and dynamic viscosity used but it gives a reference temperature. I used IEC properties calculated for that value of temperature. I think they would have to be very similar. Probably not equal!

4) I can't verify if stay vane inlet angle is 29 degree but if I look about its position I can tell you 29 degree could be a very probable angle.

5) My mesh is 1 stay vane + 1 guide vane + 1 blade = 1073452 nodes (979400 hexas). Quality is: Maximum Face Angle (Min: 89.9288 [degree],Max: 159.102 [degree]); Minimum Face Angle ( Min: 23.406 [degree], Max: 90.6736 [degree]); Edge Length Ratio ( Min: 1.02113, Max: 98.8927); Max element Volume Ratio is 12 but a very small % of cells.

6) I stopped my simulation when P, u, v, w RMS residuals are less then 10^-6. Imbalance is less then 0.01 %.

7) I added monitors for torque. I find the same value in last 20 iterations so monitor curve is flat.

8) My outlet flow respects bc I imposed

9) My outlet is on reference plane indicated in GAMM report figure. It's probably too far but I'm sure it isn't too close.

Thank you for you interest. I hope there will be people who use CFX better then me and who get better results. If there is someone who investigated GAMM Francis with CFX 11 with more success then me please contact me. I must understand where I wrong.

Hi, it seems that your model is OK. There might be less probable deviation sources, try the following (after that, I will run out of suggestion...): 1) Take a look at the MAX residaul values, not only the RMS. 2) Make sure that the blade surface was generated with the same conformal planes as the GAMM turbine. Different planes, specially when they are not numerous, can result in geometric deviations. 3) Although your n1' and Q1' are equal to the operating point you are calculating, make sure your diameter and rotation are the same as in the model, to avoid step-up effects. 4) Many people are still using the k-e model for hydraulic turbines. They might have a reason. Maybe you could try it.

Hi,

1) max residual values are somewhere about 10^-4.

2) Blade runner is defined by 17 section (200 points for pressure side and 200 points for suction side per section). I used them to import blade geometry in turbogrid by which I created my mesh. I think they are enough to rappresent blade shape correctly.

3)Diameter and rotation are ok.

4)I used k-epsilon and k-omega (I didn't find relevant differences)

I contact my Ansys supplier. He told me a 4-5% error on torque isn't absolutely a CFX standard. What CFX version do you use?

Regards

Hi, Normally, I run the simulation until the max residual values are below 1E-5, 5E-5 or even lower. With versions 10.0 and 11.0, I normally can go to less than 1% deviation. Check the flow features of the GAMM turbine in the post-processor. Since it has an old design, there might be recirculation and separation zones and the turbulence model can be facing difficulties.

Hi, An additional remark, in a turbine with such a high nq, the optimum can be close to the fixed cavitation limit on blade inlet suction side, or even beyond it. You can check this region, specially in the proximity to the crown. If that is the case, there might be separation occuring and causing difficulties to the turbulence model. A good test could be trying to calculate a different operating point, with higher n1' (between 2 and 8 units higher) with higher flow (between 5% and 10%) and a little higher guide vane opening, corresponding to this new head and flow. I guess the experimental data for such a point is available from the GAMM hill chart. Depending on your results for this new point, you'll be able to verify if you need to improve your simulation model or if the deviations are caused by the flow features, which may be separation and transient effects.