The Onset of Surge in a centrifugal compressor
i want to start some simulations of a full 360° centrifugal compressor using Ansys CFX. I simulate the compressor involving inlet, impeller, vaneless diffuser, volute and outlet. With different mass flow rates i want to examine the onset of surge. First i gonna do some steady state simulations with the frozen rotor interface. Afterwards i want to try the unsteady Simulation. I found this paper about the topic: http://www.ansys.com/events/proceedi...PAPERS/252.pdf
Because surge is an unsteady phenomena it cannot be modelled with a steady state simulation. Thats why the convergence rate for the calculations tends to stall near surge. Despite the fact of convergence difficulties the results for lower mass flow rates were plotted in this paper because they often matched experimental data very well. So the peak for pressure ratio in the resulting plots was used to localise the onset of surge and comparing the result with the experimental data. Is there any other way of capturing the onset of surge? Maybe calculating negative mass flow rates inside of the compressor? Did anybody setup a similar simulation or does anybody know another paper about this topic?
I'm simulating a centrifugal compressor and a vaned diffuser, with the same conditions like yours. I've found that paper at Ansys.com too. But I've got a lot of problems during my work. My compressor stage reached the surge at more lower pressure ratio, than it had to (We made measures of course). Any ramping function (wich was described in the papers), and modifying of the boundary conditions etc. couldn't help. There was a big separation started from the suction side of the impeller blades, wich closed the area. My operating pressure ratio at 116000RPM is 3.17, but we can reach only about 2.5. After that we made a periodic modell with only one blade passage, with millions of elements, in a transient simulation, where the pressure at the outlet was ramped up. So the mesh was very fine and good quality. Thus we reached the targeted PR, but this transient simulation takes a lot of time (1 week absolute simulation time).
So there is an other problem with my modell, but we don't now what exactly.
To the surge: Yes, we made surge in steady simulation. For example, at 2.4PR, the mass flow is very small. You step to 2.5PR, and the fluid is flowing back into the domain. To get this, you have to use opening boundary conditions of course. With outlet you will get convergence problems, with the message "Wall has been placed at portions of an outlet...". So I recommend to use opening. Also the Mass flow outlet wasn't helpful to avoid surge at these low pressure ratios.
Could anybody send a picture about a good mesh in cf compressor? With hexahedral mesh could I reach lower element numbers and more accurate results?
Finally, sorry for my english :)
i`m running my first steady state simulation at operating point (160.000 RPM and a massflow of 0.2kg/s, Pressure ratio of 2.7). My inlet boundary condition is Total Pressure and Temperature, outlet boundary is the massflow. But you`re right when it comes to unsteady surge effects i should use an opening boundary condition at the inlet instead! I use the frozen rotor interface between stator and rotor and wanted to start the stage model afterwards initialising the simulation with the results from the frozen rotor model. I guess this could safe some computing time....Which model are you using? So you initiated surge by changing the pressure ratio and not the mass flow? My first simulation is not ready yet...the only thing i see is that the results are oscillating but seem to converge...any idea why that is happening? From my backup file i see that the simulated pressure ratio is also much too small...there is a great loss of pressure inside of the volute and between volute and outlet it rises again abruptly. To the mesh: i have to use scripts that generate a tetra mesh for impeller and volute, for inlet and outlet i made hexameshes. I dont know if my mesh is ok. I want to make a net study first refining the mesh of impeller and volute. I think inlet and outlet dont have to get lots of elements. Hexameshes are always a better solution because you need less elements and less computing time. And you can control the number of elements in a better way! But it should have no effect on the quality of your results i think, because your solution must be approximately independent of the used mesh.
Have you been through the basic stuff to obtain convergence? As discussed here:
I'm using both frozen rotor and stage interface. With the stage interface the solver averages the values at the interface, so you can get more general values, for example in the vaned diffuser. It can help you to avoid some convergence problems caused by flow separation, but I think, it can safe not too much computing time. Stage is useful, when your geometry is periodic, and you can not use frozen rotor. But with frozen rotor, you can study the interferences between the rotor and stator (in my work, the blades of impeller and diffuser are very close together). You can get a more accurate simulation, when you make a steady simulation with frozen rotor, and then a transient simulation (with initialization from the steady of course).
I've got the surge by increasing the pressure ratio, by 0.1 or lower values. With mass flow my simulation diverges near surge, but I've got a different geometry model. If I have a bit time, I will upload some pictures next week...
What is the main goal of your simulation? To get the characteristic, or just getting the surge line? I ask it because when your goal is getting the characteristic curves, i recommend you some "tricks" to get them faster. You should start your simulation at lower RPM-s, for example at 60%, and with very low PR. When you have time, it can be PR 1.0. With PR1.0 the simulation finishes fast, with a high mass flow rate. From these results, you can increasing the PR, keeping the RPM constant. At the beginning, you can use bigger steps in PR (1.0->1.5), but at higher PR-s, when you don't want to have a divergence, more lower (PR 2.4->2.5 or lower).
It is also intersting, that when I set a mass flow value I get a PR. When I set this PR, I got a different mass flow, and it was a big difference. After that I saw it's better not to use mass flow outlet boundary conditions. But I note again, my geometry is different than yours!
When you finished your simulation, please share with me the results, I'm very intresting in it.
Have a nice weekend,
|All times are GMT -4. The time now is 07:08.|