Now I have a problem about computation.I set the number of iterations as 10000. When the number reachs 200,1000,I interrupt the computation and display vectors of relative velocity.They are different .I want to know which is more accurate and how to set the number?(my solution is very difficult to convenge)

Hi lingo,

It depends on the residuals. the lower the residuals the more accurate the results. Therefore, you should check your residual levels. In addition, 10000 is a very large iteration number. If your problem is well posed(boundary conditions are ok), grid is sufficiently fine in high gradient regions and relaxation parameters are not too low(in segregated solver- courant number in coupled solver) you should reach the convergence easier. I suggest you to check your boundary conditions and grid carefully.

Regards, Mustafa

Hi, I suggest you do not trust the residuals only. From my experience, you may have a flow solution with residuals as low as 10e-5 for momentum and turbulence equations and the solution still changes a lot. Such an example may be a self ventilated machine, where you want to find out what the flow rate is (rotor draws the fluid in through inlet with prescribed pressure, generates pressure inside and vents the fluid out again through pressure boundary). In such a case you have to monitor the flow rate and when it is settled, the case is converged. Sometimes people argue what level of residuals is sufficient. What is a numerical accuracy of 0.1% good for if you have 20% uncertainty in the assumptions, boundary conditions and physical models in the solver... Remember, even the best converged solution will be correct only for the boundary conditions you specify. Reality may be different...

Besides residuals, you need to go to Report-flux to verify the mass and energy conservation for your system.

LW

Hi lingo,

Martin and LW are completely right. There are several convergence indicators and residual plot (although it is sometimes insufficent)is only one of them. In addition, I agree with Martin about effect of boundary conditions (and mesh resolution) on accuracy of the solution.

Regards, Mustafa

Thanks a lot .I want to simulte a minitype centrifugal pump(radius of impeller is 16mm)with an inlet and an outlet.I select segregated,implicit ,RNG k-e model and standard wall function,set the inlet as velocity-inlet and outlet as pressure-outlet.The residual level is 1e-3. My new problems are: 1) As to k-e model ,I should adopt 2nd order flow solution.Now it is difficult to converge in 1st order ,so it it more difficult to converge in 2nd order.How to converge?Can I lower under-relaxtion? How important convergence is? 2)In my example,the number of grid cells (same type ,i .e 80000,180000)also affect the computational results. Expect your advice and help!

If you want a reliable solution of a pump problem you have to run it transient with sliding mesh.

Hello,

You ask how important convergence is? Never use results from an unconverged simulation.

Your boundary conditions are a bit strange. A velocity inlet is not a good inlet condition for a pump I think. Now you're imposing a flow. Do you now the exact correlation impellerspeed - flowrate - outletpressure? Probably not.

Joern suggests to use a sliding mesh. Probably this is the only way to have good results, but you may try the multiple reference frame first. This will give you a good idea of the flow, and can learn you about the desired grid-density.

How big is your mesh now?

good luck,

Laika, still orbiting