CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   CONVERGENCE IN FLUENT (http://www.cfd-online.com/Forums/main/10274-convergence-fluent.html)

 Fer November 14, 2005 07:13

CONVERGENCE IN FLUENT

Hi all!

I'm making 2D simulations with Fluent. The case is that the problem seems to converge at 3000 iterations (you know, low+stable residuals and almost constant solution). My problem is that if I let Fluent simulating after that iteration the residuals increase progressively, while the solution remains the same. I tried solving this fact by making lower the default under-relaxation factors that I used during all the process: firstly the residuals decreased suddenly but then they continued with the previous increasing trend. I think that it's not a grid problem.

I would be very grateful if anybody could give me some advice.

Fer

 cfd101 November 14, 2005 21:13

Re: CONVERGENCE IN FLUENT

Is it all the residuals or just the pressure-correction equation residual which tends to increase.

thanks.

 Fer November 15, 2005 03:26

Re: CONVERGENCE IN FLUENT

All the residuals trend to increase. The fact is that the continuity, k and epsilon (I'm using k-e standard model to get a solution and then RNG to get better results) residuals are about 2 magnitude orders higher than velocity residuals.

Yesterday I probed making lower the under-relaxation factors given by default but that wasn't the solution. Finally, I probed by using a first order and first order upwind solution (instead of using the second order): that worked quite good and after 800 iterations all the residuals trend to decrease very hard. Could you tell me if that's a good solution to solve my problem? and also, does first order solution option give good results (I'm modeling the flow arround an automobile in 2D)?

Thanks for all

Fer

 AnotherCFDUser November 16, 2005 17:41

Re: CONVERGENCE IN FLUENT

Does first order solution option give good results

Depends upon the size of the grid. Have a read of any introductory text on CFD and it will explain what is meant by first and second order discretization schemes. Once you understand this you will be able to answer your own question and will be on your way to becoming a better CFD analyst.

 zxaar November 16, 2005 20:10

Re: CONVERGENCE IN FLUENT

usually fluent suggests to use first order scheme to get good solution and then to switch to second order scheme. Anyway, for second order schemes the value of scalar at face is estimated by using gradients (as compared to first order where it is cell center value from either side of face). Now these gradients are restricted, so that the face value should not exceed local max-minima. If the mesh is coarse or severely nonorthogonal at some places, these restriction will hamper the smooth convergence,, that you get in case of second order scheme. So my advise will be to check your mesh and look out for the two issues mentioned above.

 zxaar November 16, 2005 20:11

Re: CONVERGENCE IN FLUENT

that you get in case of second order scheme

as

that you get in case of first order scheme

 Fer November 17, 2005 03:34

Re: CONVERGENCE IN FLUENT

Thanks all!

In fact, I proved with a finer mesh before (170000 vs 110000 elements) and I had no problem with convergence using second order scheme. In that case, the simulation was quite more slowly (obviously) but the solution obtained is almost the same for both cases.

In my case, I have simulated the 2D car that I'm studying for a wide range of flow velocities (from 10 to 50 m/s) with that RNG+Non-Equil_Wall_Functions and with a first order scheme. The results gave very similar Cd values (between 0.29 and 0.30) in all cases and also coherent contours; the y+ in the car walls had values in (30, 300) mainly and the pressure gradients where quite low. My question is: are these results a good criteria to confirm that the simulation is well done?