CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   Main CFD Forum (https://www.cfd-online.com/Forums/main/)
-   -   flat residuals (https://www.cfd-online.com/Forums/main/91155-flat-residuals.html)

 shilpamkar August 2, 2011 05:05

flat residuals

Hello,
I am simulating a cylinder(H-6cm,D-4cm) with an inlet on the top surface and outlet on the curved surface. the conditions i use are
mass flow inlet-0.04kg/s
outflow
mesh tri/Pave
residuals-1e-6
However, i get flat residuals after 1e-4 and the solution does not converge for a second order scheme. but for a first order scheme it does converge. how can i make the second order solution converge below 1e-4.

 Docfreezzzz August 2, 2011 15:16

Have you investigated the solution results for the 2nd order run? Is it possible that the 2nd order solution has unsteady characteristics? Also, you may have a very poor grid which is stalling convergence for the higher order method. I would suggest visualizing the solution and possibly posting a picture here for more help.

Nick

 shilpamkar August 3, 2011 00:10

Yes I have. there is about 10% difference between soln for the two orders.the grid seems fine.maximum skewness is 0.78. have tried using QUICK too, also reduced the URFs but it just doesnt help. wht does solution having unsteady characteristic mean?

 Docfreezzzz August 3, 2011 10:27

I was not referring to the grid quality but rather the refinement in high gradient regions. A course grid can often be harder to converge with higher order methods. By unsteady characteristics I mean does the solution appear to be shedding vortices, etc.? If the problem you are trying to solve does not have a true steady-state solution then I would expect the residuals to stagnate as you are seeing.

 shilpamkar August 4, 2011 02:05

I have tried with refined meshes. doesnt help. also I actually dont understand by 'solution shedding vortices'. As I understand the wht u r talkin abt is flow past d cylinder. my flow is in d cylinder. nd how do I know whether my problem has a true steady solution or not.Currently, I am trying an unsteady simulation.taking a lot of time. running since a day. do u think this will help?

 cfdnewbie August 4, 2011 02:33

a) what kind of scheme are you using? FV? Explicit or implicit?

b) If your O1 solution looks steady, and your O2 doesnt, then it means just that the O2 captures more "waves" (physical or otherwise) than O1 which irons out everything of interest - the physics as well in my opinion ;)

c) Try the following: find out where the max, change in residual is from one iteration to the next, i.e. what drives your residual. Is it a bad grid cell maybe? boundary conditions?
You didn't mention whether the flow was qualitatively converged for your O2 solution or not...
Does it get get worse when you refine the mesh?

 shilpamkar August 4, 2011 08:44

yes the residuals worsen as I refine the mesh. the solution does change.Qualitatively, I get the same velocity contours for both the orders being quantitatively different. boundary condition is mass flow inlet and an outflow.
how do u know whethr d soln has qualitatively converged or not.not able to figure out.

 Docfreezzzz August 4, 2011 10:48

Can you post a slice of the velocity contours through both inlet and outlet here? I'm still suspicious that your O2 solution has an unsteady character to it that is not resolved via the O1 solution.

Actually, it is possible that your outlet BC is incorrect. Is it a backpressure outlet condition? If not (and maybe even if it is), this could set up a pressure wave which the inlet mass flow condition would track resulting in a case which does not converge. Do you have a method of tracking what the instantaneous pressure is at the inlet. If you could plot that for us, I'm sure you would see an oscillation as the inlet BC tries to track the interior pressure banging around.

One thing you might try is restarting the O2 case with the O1 solution, which will have a great deal of oscillation damped already. Something that I do frequently.

 cfdnewbie August 5, 2011 03:01

If your problem worsens as you refine the grid, that is because you are capturing more waves on a finer/higher order grid....
so there are two options:
a) your problem is inherently unsteady, that means that the solution with O1 is plain wrong

Again, find out WHERE the residuals change/fluctuate, that will give you your answer. In addition, run the problem with much higher order (like 6 or 8) and see what happens...

hope this helps :)

 cfdnewbie August 5, 2011 03:03

Quote:
 Originally Posted by Docfreezzzz (Post 318889) One thing you might try is restarting the O2 case with the O1 solution, which will have a great deal of oscillation damped already. Something that I do frequently.

wouldn't that only help with the initial phase of the flow, i.e. the disturbances due to initialization? If the physics are indeed unsteady, then after some time the fluctuations will start to build up again, right?

Restarting from O1 sounds like a cheap way of doing multigrid, good trick btw :)

cheers

 Docfreezzzz August 5, 2011 12:53

@cfdnewbie. Yes, it's just going to damp some of the higher frequency error in the initial flowfield. Multigrid is hard with unstructured grids so I find myself doing this a lot. I'm trying the shotgun approach to this problem because I haven't seen a solution plot posted. Debugging a case in the dark is pretty challenging. If it is indeed unsteady you'll likely have the same problems but as this thread develops its looking more and more like something might be misbehaving with the BCs. Hopefully, shilpamkar gets it straightened out.

 shilpamkar August 8, 2011 01:02

hey sorry for the late reply. actually was not wel.so not in touch. i have tried using first order solution as the initial guess for the second order. however, it does not help.i tried doing the unsteady simulation. It gives me a 3% difference as compared with the unconverged solution of second order. it took me three days for the simulation.qualitatively it gives me the same velocity contour. do u think going for unsteady soln is the right choice?

also,regarding the BC I have given the outlet to be an outflow. can u pls tel me how the BC can affect the solution.

i m completely new to this nd would love to get some information on how to go about defining conditions form a problem.also can u suggest me some books or any material for studying FVM.do u think it is necessary to know evrythn abt FVM in order to get a hold on solving using FLUENT.

 shilpamkar August 8, 2011 01:06

also pls tel me how to use adaptive time stepping.the various parameters that hv to be chosen on wht basis.

 Docfreezzzz August 8, 2011 13:13

I'm not very familiar with FLUENT so questions regarding the particulars, including adaptive time stepping, etc., are probably lost on me. I only use custom CFD applications in my work. However, you shouldn't need to know how to write a solver, or exactly how FVM work for that matter, to run FLUENT successfully. I'm not sure how FLUENT inputs are specified but what is the CFL number you are running? Do you have local timestepping on? What is the size of the mesh (elements, points)? What is the size of the machine you are using (cores)? Three days sounds like a very long time even for a full rotor simulation which is considerably more complex that what you've described.

If the condition you have chosen for the outlet BC is based on characteristic variables then it is non-reflective and should damp oscillations in pressure. However, this will (depending on implementation) overspecify an internal flow problem and cause issues with convergence. If the outlet is a backpressure based outflow condition it could be causing reflections of pressure waves internally. This is more common. I've not used massflow inlets but I'd bet they behave the same. Could you post a plot of the massflow at the inlet vs. time for me? This would be the most help to diagnose the BCs. A picture is worth 1000 words.

 shilpamkar August 9, 2011 01:22

hey the mass flow inlet is constant wid time. it gives me a flat plot. also i shall try uploading certain pics. the size being too large ws not able to.can you give ur mail id if u dont hv any problem so that i can send u some plots as well.tht would be much easier.

 Docfreezzzz August 9, 2011 12:16

My e-mail is webmaster at cfdengineer dot com. You should try resizing the images and posting here as you would likely get more help from that approach. The more eyes that look at a problem, the more likely the solution will be found.

 Docfreezzzz August 10, 2011 13:11

After looking at the e-mail you sent me, your grid has a very weird character which is likely causing the problem. Modelling inlets as simply a segmented portion of the boundary condition does not work very well in my experience. Simply adding a short extension from the wall in the (i.e. a tube) will likely give you better results. For that matter, at the outlet as well. Also, if you actually are concerned with the physics of this problem I would add a significant inlet area as you are likely going to see some recirculation near those 90 degree corners.

The problem is mostly numerical in nature b/c you are artificially creating very high gradients in between those inlet/outlet regions and the wall. And, if you are using viscous BCs the situation is even worse. Those viscous layers will never look realistic. A good rule of thumb is that if you expect non-uniform flow in a region, go back upstream to the closest region from which you expect uniform flow and start the geometry from there.

Let me know how this turns out for you.

 shilpamkar August 12, 2011 06:38

"The problem is mostly numerical in nature b/c you are artificially creating very high gradients in between those inlet/outlet regions and the wall. And, if you are using viscous BCs the situation is even worse. Those viscous layers will never look realistic. A good rule of thumb is that if you expect non-uniform flow in a region, go back upstream to the closest region from which you expect uniform flow and start the geometry from there."

Can u pls elaborate on this. I could not get much out of it. I am trying the addition of tube to the inlet as well the outlet. will the length of the inlet as well as the outlet tube affect the solution. Really want to get this done as soon as possible. have been trying since a long time.

 Docfreezzzz August 12, 2011 14:03

You are forcing uniform flow in a region where it is not likely that physics dictates that. Inlets modeled as you have always give me problems. Basically make your inlet farther away. The length of the inlet will affect the solution only if you are running viscous walls and then only b/c of the flow developing as it moves down the pipe. In short, you will most likely need the inlets or your results will be questionable to begin with. The outlet tube length shouldn't have a huge effect other than backpressure on the mixing chamber.

Good luck.

 All times are GMT -4. The time now is 02:15.