Second Order Upwind: Residuals
 

In a pipe sudden expansion simulation, with first order upwind i have no problems with residuals, but when i switch to second order upwind the residuals remain constants at 10e-1. Why? What i have to do?
Thanks!

Increase residual limit or increase number of iterations?

Residual limits are at 10e-12
Increasing number of iterations is not useful because the residuals remains constant after a certain number of iterations. Constant at 10e-1.

Did you try solve the same problem for different mesh?

Yes, i have tried. But the result is the same. Sometimes it is worse than others.
Did you think that could be the mesh?

Did you start the second order case from the first order solution?
This might have happened if you directly run a second order simulation and the solution is not able to converge.
Try using the 1st order solution as the starting point for the 2nd order.

Done! I start second order after running first order...
http://www.ninarello.it/order2.jpg

Hi,
That's unfortunate.
Did you try changing the under-relaxation factors?
Looks like the solution is not able to converge by the sudden change in descretization.
Try reducing the URFs to get a delayed but better convergence. After the residuals go down, you may set them back to default.

If this doesn't work, may be you should not let the first order solution converge to the low residual limit. Say, set the limits to 10e-2, run first order, and stop after converging, and then run in second order.

BTW, is this not turbulent? You are tracking only momentum and velocities?

Can we have a look on your mesh? Could you post a pic of it? I guess the problem might be in the mesh or boundary conditions...

regards

I post you same images with info:
http://www.ninarello.it/grid.jpg

http://www.ninarello.it/grid2.jpg

http://www.ninarello.it/geometry.jpg

This is a rar with the case and date file:
http://www.ninarello.it/Progetto.rar

no other proposals?

I often encountered such a behavior. Usually, a transient analysis is necessary, as the transient effects are "washed out" due to the diffusive upwind scheme....

monitor a value of interest to see when your simulaiton converges...

good luck

I see those cells quite stretched. Have you tried to make pore divisions of your domain in X-direction? I remember that in a project I made a boundary layer in a wind tunnel floor with cells too streched in the flow direction and simulation diverged all the time: when I made cells more "square-shaped" simulation absolutely converged.

By the way, your Y-direction cell divisions seems to be all right.

I suggest you to try this. Good luck!

I have to try to refine mesh along x direction, but i don't understand what about transient analisys...

---deleted---

strange...when i run the simulation it converges very well with your settings...

only thing i noticed is that you have reversed flow on your pressure outlet, but residuals look fine...

Hi xdanielx,

At which iteration has you switched to 2nd order?

agree with xdanielx,at the 539 iterations,residuals reach convergence.then adjust pressure discretization to 2nd oreder,it reach convergence at the 772 iterations.

Can i change under relaxed factor for pressure from 0.3 to 0.1? With this value residuals decrease...
I don't know why the simulation converge with my settings to you but not to me ... Can it be the PC?

Stupid question but, are you using double precision when you start Fluent?

Have you tried also to switch to 2nd order more before those 1200it? I don't think this may be the problem, but who knows :eek:... When you reach 1e-3 in 1st order (I guess at 200it) you are ready to change to a higher order. I have changed to 2nd order even at the 50th iteration (when you're in a hurry :rolleyes:...)

This may seem a bit strange,i advise you slove the case you upload again.

Yes i'm using double precision...
Your results at the number of iterations you indicate aren't the same of mine... I don't know why!
Changing URF of pression from 0.3 to 0.1 i have the result i want, but is it a correct method?
And what means to decrease URF?
Excuse for my bad knowledge... :(

Maybe it is completely wrong approach, but what happens if you try to use transient solver?

Why i have to use a transient solver if the problem is steady?

I'm didn't say you have to, I said that maybe something unexpected happens if it breaks so early. I don't know ;)

I repost the former question:
Changing URF of pression from 0.3 to 0.1 i have the result i want, but is it a correct method?
And what means to decrease URF?

Does anyone know it?

i was about to ask you to reduce mom urf little bit. Or reducing pressure urf would help but might not be the case always.


urf of pressure results in slower update of pressure.
pressure_new = pressure_old + urf * change in pressure.

anyway the main reason of your problem is your grid. it is not refined enough to handle fast change that is coming in flow direction. If this situation happens the gradient of u,v,w varries very fast. And often breaking local maxima minima. When you use second order scheme there is a contribution of this term in momentum equation. If your gradients are false this term might be shooting up and down. By reducing pressure unerrelaxation the change due to pressure change is restricted (which is main change per iteration) and behaviour of second order contribution is controled better.

for steady state using low urf is no cheating. Its just a way to get converged solution.

A few years later, which is the solution to this problem? I encounter the same difficulties and I did all the above things proposed..

Achillieas, I don't think it is an unusual experience to get crappier convergence when switch to a less robust discretisation scheme but I don't think it is something special with a pipe expansion (as the testimonies above afirm) . Therefore I would advise you to do as in every case - describe as much as possible about your case, display the mesh and ask for help.