# Computation through radial impeller

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

 LinkBack Thread Tools Display Modes
 January 11, 2000, 11:51 Computation through radial impeller #1 Ursenbacher Guest   Posts: n/a Hello, I'm doing a computation through a radial impeller but I have some convergence problems. The numerical scheme I use is a 2nd order central sheme with 2nd and 4th order dissipation for spatial discretisation and a 4th order Runge Kutta for time discretisation. The problem is the following: The massflow, the efficiency, the torque,etc.. oscillate. If I reduce the CFL, the wave length of theses oscillations increases. What can I do to avoid theses oscillations and to have a converged solution? What are the effect of the 2nd and 4th order dissipation? Can I suppress the oscillation by varrying theses two parameters? Thanks for your attention, F.Ursenbacher

 January 11, 2000, 12:35 Re: Computation through radial impeller #2 Joern Beilke Guest   Posts: n/a Are you sure that the flow is steady-state in reality ? What about your mesh (2d/3d/y+/??) and the boundary conditions. Does the impeller rotates somehow?

 January 11, 2000, 13:13 Re: Computation through radial impeller #3 John C. Chien Guest   Posts: n/a (1). The physics of the problem is rather complex, because it always involve 3-D flow and flow separations. So, I am not going to get into that area. (2). The method you are using is Jameson's type formulation, that is transient, compressible formulation. The transient, compressible formulation is sensitive to the low Mach number effect. So, try to stay away from the low Mach number regime. (3). It is essential to mention your problem's Mach number and Reynolds number, along with any turbulence model and treatment used. So, remember that next time.

 January 11, 2000, 13:35 Re: Computation through radial impeller #4 Dan Hinch Guest   Posts: n/a The instability could be due to a large number of causes (even if your numerical scheme is appropriate) including the grid (both spacing, and the size/shape of the inlet and exit extensions), the Mach number level (as John has mentioned), the initial guess (how far does the solution converge before going unstable?), and even the design being analyzed (is the flow truely steady state?).

 January 11, 2000, 23:57 Re: Computation through radial impeller #5 Mohammad Kermani Guest   Posts: n/a Hi there: > Dan Hinch, Tue, 11 Jan 2000, 10:35 a.m. WROTE: > and even the design being analyzed (is the flow truely steady state?). when you mention about the unsteadiness of the flow, do you mean flow is physically unsteady in reallity? If so, how such a thing could be invetigated before doing an experiment? Just by cfd simulations? Is that somehow related to the transion from laminar to turbulent? Does these kinds of unsteadinesses happen only in viscous flow simulations? Does the inlet buzz also fall into these categories? Thanks.

 January 12, 2000, 02:27 Re: Computation through radial impeller #6 John C. Chien Guest   Posts: n/a (1). I think, the convergence problem in most cases is related to the mesh, the boundary conditions, the numerical method, turbulence model, and the initial flow field guess. (2). Assuming (pretending) that the method, the model and the B.C.'s are properly selected, the mesh and the initial flow field guess are the two biggest common problem related to the solution convergence. (3). So, the mesh re-adjustment is always a good option to deal with the convergence problem. (4). For the initial flow field guess, one can gradually change the time steps from a small number (sometimes I had to use 1.0E-07 to get it started. In most cases, 1.0E-06 was used), unless a very good initial guess is used. The time steps must be increased, otherwise a strange flow field will develop from the poor initial guess and then it becomes hard to correct the course later on. (5). On the physics side, the inlet condition is important. The operating condition also is very important, which will determine the relative flow condition to the rotating blades.(the mass flow and the RPM are important operating conditions). (6). For the pump, the blade leading edge will be relatively blunt to withstand the wear. Thus, the flow is less sensitive to the relative flow conditions. (leading edge flow separation) (7). For compressor, the blade will be relatively thin, and the relative flow condition will have severe impact on the flow separation at the leading edge. ( Even at the design condition, or the optimum condition, the relative flow condition does not follow the blade leading edge metal angle. (8). Then the 3-D rotating passage flow is extremely complex. You have to see it to believe it. The 3-D flow on the pressure side is completely different from that on the suction side. The same is true for the radial turbine flow field. (9). I would say that, the simplest way at this stage is to control the time steps and to improve the mesh .(if the flow convergence problem can be linked to a particular region of the mesh) This is the first step. Without a converged solution, it is hard to address the rest of the issues. In the transient approach, it is possible to step into a real transient flow field. So, it is important to run the design condition (or close to it) first in order to eliminate un-necessary complications. (10). I have done some systematic testing on the effect of the second-order and the fourth-order artificial terms in one of our turbine code. My experience is that it is worthwhile to do a systematic test. It can smooth out the oscillations (wiggles). But it will also affect the real total pressure loss.

 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 renyun0511 OpenFOAM Running, Solving & CFD 2 November 1, 2011 23:09 BalanceChen ANSYS 2 July 7, 2011 10:26 Mukund Pondkule Main CFD Forum 1 April 5, 2011 09:24 Allan OpenFOAM 0 April 16, 2009 01:00 Ursenbacher Main CFD Forum 3 December 15, 1999 20:56

All times are GMT -4. The time now is 02:26.

 Contact Us - CFD Online - Top