how do i know that my moment has converged?

Pls help me in this.I need to monitor moment as my performance indicator

WAITING

solve->monitor->forces

and drop down the list to moment and specify the rotational axis.

yeah. that is what i did but how do i know when it has converged.Am i going to have a constant moment for a long time or what?

exactly..

so, if the moment is not constant(i.e it is changing) that means my moment has not converged

It either means you haven't reached a converged solution, or that you have an unsteady problem (typically due to vortex production in a region of separated flow... like behind a bluff body or off the separation on a wing).

Good luck, Jason

ok.i will try to leave d solution awhile and see if it'll d moment will constant

What could be responsible for this vortex production?

thanks

That depends on your model. Separated flow is the most common cause. Separated flows are naturally unsteady. For a bluff body, you'll typically get vortex shedding (like behind a cylinder). For airfoils the separated region will oscillate forward and backwards on the airfoil. The "steady state" solution for these is usually a time averaged value during testing (electronic data is typically recorded over a period of time then averaged, if the data is recorded from mechanical readouts, there is typically some damping in the system to account for small oscillations). Depending on what's causing the unsteady response, you can usually get a solution within a small oscillation (if it's oscillating in the 3rd or 4th significant figure, does that really matter? I'd be willing to bet my hard earned money that your CFD model has more error than 4 sig figs), but this depends on your choice of turbulence models, the extent of the separated region, and your mesh density and quality.

A poor mesh can also cause a "flapping" effect. I've seen it for a poorly meshed airfoil where the grid sensitivity was causing an oscillating pressure coming off the trailing edge of the airfoil that wasn't real. It wasn't separated, but it was a pressure oscillation. We refined the mesh and that problem went away.

If your values aren't converging (or at least oscillating about a small enough range), then you need to look at your solution and try to figure out where the problem is. You can create vertices and monitor the pressure at these vertices to try and locate the problem area if you have to. Try refining your mesh in the problem areas. If you're still having trouble, look into the different turbulence models. You may not have the best model chosen for your problem. If it's a large scale oscillation due to a large separation region (like behind a cylinder) then you may never get a steady state solution, and you might want to run it unsteady and use data sampling to get average and RMS values.

Hope this helps, and good luck, Jason

Thanks.My model is a mixing tank.I'm carrying out a kind of parametric sensitivity of the turbulence model which is standard k-e model.There has been issues around the use of this model but the computing requirements & robustness still makes it best.But I am trying to optimise the model by changing the constant(C1,C2, Cm) so as to see the effect on the predictions. Using the standard k-e model, the moment converged but changing some of these constants, the moment refuse to converge.I was wondering what could be responsible for this. The surpising thing is that the moment is not converging but the variation of the constants has a great impact on the constant.For instance, some combinations of C1, C2 & Cm gave me good predictions with least error values between the experimental and predicted values. But the moment did not converge. I am really surprised about this.

So u can see the issue now.

Waiting yr response

Now you're getting into areas where I'm not too familiar. I pick my turbulence models based on a knowledge database we have where we compare different turbulence models to different situations. I have never gone in to customize a turbulence model. I hope you've researched the turbulence model and what the different coefficients do. Also, you should do some research to see what other people have used for custom coefficients.

I have a feeling that some of the constants effect the stability of the model, which is why you're having trouble getting a converged value.

Also, do you know for sure that your mesh is optimized? Have you run mesh sensitivities with the default coefficients?

Hope this helps, and good luck, Jason

I have played a little with the k-epsilon constants, I could make converging the solution on a very bad grid.... this effect was due the increase of the turbulent viscosity ratio which is known to stabilize the flow(just like normal viscosity).

So it is always possible to modify the constants so that the magnitude and the distribution of the turbulent viscosity damp instabilities.

So I totally agree with Jason, this is dangerous, we should first verify our grid, y+, symmetry of the grid...etc before playing with the parameters.