Hello... I've run a steady flow simulation but the solution doesn't converge well. The pressure seems to oscillate and not stable during the run. Some friends suggest me to run the transient simulation and see if it helps.

Can anybody explain to me why transient simulation may give a better converged solution in this case? What's exactly the difference between terms in the transient & steady solver that makes solution converged better?

Is the term "d(rou)/dt" in continuity equation & "d(rouU)/dt" in momentum equation treated/formulated differently in steady & transient solver?

Thanks for your help. Cheers,Sally

Hi, Sally, If the solution converges yet the solved variables are oscillating, then it's a unsteady simulation for sure.

If there's is no change in dt, then it's steady otherwise it's unsteady.

What are you looking at? -Edward

Hi Edward,

I'm working on air flow being sucked into a 90-deg bend channel with increasing cross sectional area from inlet to outlet to decelerate flow. From experiment, I observe strong reversed flow & separation downstream.

I manage to get solution converged using k-e or k-w model. However, solution isn't favorable. So I try reynold stress model developed by Launder et al but static pressure at some monitor points in the domain start to show some oscillation during the run and they don't die away after 1000 steps. Residual isn't gone down for such reason (I guess).

Anyway, I don't think you can get a converged solution when the variable is oscillating. Friends suggest the flow is unsteady.

Boundary condition aren't changed at all but running the transient simulation managed to reduce solution residual. So I wish to know the reason behind this. Assume that we can freeze the time, the flow is supposed to behave steadily at that frozen time. I don't understand why steady solver doesn't drop the residual while transient solver does when boundary condition is constant.

Thanks, Sally

A converged solution does not mean that it is a correct solution!! It is very likely not a steady flow if you can observe strong reversed flow & separation.

Thanks,William... There's stall region inside the channel. However, I set boundary condition to be constant for the simulation, not a time function.

The flow pattern will vary even though boundary condition is set constant => that's unsteady effect => that's why steady flow solver doesn't give converge solution because the flow variables in the flow domain keep changing.

So if I run transient simulation with constant boundary condition, the solution residual drops futher because transient simulation takes into account "d(rou)/dt" in continuity equation & "dU/dt" in momentum equation while steady simulation assume these terms to be zero.

Is my understanding right?

Thanks,Sally

Unconventional wisdom:

Turn off all convection stabilisation (no upwind etc), select small time-steps (with say Courant limit), ensure that you have reasonably small elements, start the transient-solver.

Take regular 'peeks' at the emerging solution to make sure it is not giving garbage. Continue watching throughout the solution phase. Compile the snapshots into a movie & learn about the physics of the flow.

Have fun... Oh, I trust that you have the computer power & the patience...

diaw...

Hi diaw.... why "Turn off all convection stabilisation"? Isn't that thing supposed to make simulation stable?

Anyway, Is my reason to run transient simulation for constant boundary condition sound right?

Thanks,Sally

Sally wrote:

why "Turn off all convection stabilisation"? Isn't that thing supposed to make simulation stable?

Anyway, Is my reason to run transient simulation for constant boundary condition sound right?

--------

diaw replies:

Hi Sally... here's my take...

Why would you want to 'stabilise an unsteady process' any further than to compensate for numeric direct scheme shortfalls? I would go in at pure Central Discretisation & see how well you fare... if there are problems, then start looking as 'small doses' of numeric stabilisation. Then, at least you can be the best judge of whether your flow problem is indeed steady, or unsteady.

Why should a 'constant boundary condition' not produce an 'unsteady solution'? Basically if you go far enough up any inlet, you should arrive at some 'steady boundary condition' eg. eventually even to clear air, or reservoir etc... does that imply that there will not be transient conditions anywhere downstream? Obviously it does depend on how you specify the B/C, you can experiment with solution sensitivity to the B/C.

I hope that this clarifies my thoughts...

diaw...

Look at a vortex street. There you have steady boundary conditions and an unsteady flow field.

Why do you want a stable solution when your flow problem is not stable at all? Do you really want an artificial wrong solution?

>>>William Blake: Why do you want a stable solution when your flow problem is not stable at all? Do you really want an artificial wrong solution?

I believe that most of us, through our engineering training, have been conditioned to believing that most 'normal flows' are stable. It seems to difficult to venture out into the world of unstable (non-analytical) solutions.

-----

Sally, think on this thought... what if most pipe-based flows exhibited the evidence of 'unsteadiness' at velocities less than 1 mm/s? How would that change your approach to your problem?

diaw...

hi, Sally, The previous guys are right. just run the simulation longer. 1000 steps, that just a quick coffee break for me. Be careful on imposing inlet boundary conditions on your sim. -Edward

Yes Sally, you're reasoning is sound. Forcing a model that has transient features into steady state manifests itself as periodically oscillating residuals. Running transient should substantially reduce the residuals at each time step.

A coarser grid and/or more dissipative numerical schemes will have a tendancy to diffuse out the transient features.

have not read all the messages in the thread. some reply may have already appeared. the transient terms del/del(t) in the cont and mom eqns are often kept in the formulation and accordingly discretised. one has to go for unsteady solver with requisite delta t (time step) which also acts as a kind of relaxation parameter. i think there are many papers - the one immediately coming to mind is by vahl davis. normally u v w etc dont require any further relaxation. read patankar carefully - i think the last 25-50 pages or so. convergence criteria has to be carefully chosen.

Hi... I have a question about your comments here: "the transient terms del/del(t) in the cont and mom eqns are often kept in the formulation and accordingly discretised."

Do you mean that del/del(t) is kept in formulation of steady flow solver? I think they have been dropped in the discretised formula for steady flow solver. If these two transient terms are still present in steady flow solver, then I'll be more confused about the difference between steady & transient solver. I only have a textbook from Versteeg & Malalasekera, 1995 and I haven't found the inclusion of the transient terms (see below) in solution algorithms for steady flow (Chapter 6)

Discretised transient term in continuity equation: V(rou-rou_o)/deltat should disappear for steady flow

Discretised transient term in momentum equation: V(rouxUi-rou_oxUi_o)/deltat should disappear for steady flow

"one has to go for unsteady solver with requisite delta t (time step) which also acts as a kind of relaxation parameter"...

Can you explain a bit more about this statement? It seems to touch the question that I'm asking earlier... but I still don't quite understand your meaning here.

Thank you very much for your help.

"A coarser grid and/or more dissipative numerical schemes will have a tendancy to diffuse out the transient features."

I'm on your side with this statement. The nasty convergence problem appears when I use the fine mesh. The only way I can get a converged solution is to implement the transient solver.

Sally wrote:

"A coarser grid and/or more dissipative numerical schemes will have a tendancy to diffuse out the transient features."

I'm on your side with this statement. The nasty convergence problem appears when I use the fine mesh. The only way I can get a converged solution is to implement the transient solver.

---------

diaw: How do you damp out vibrations in elastic media (solids)? ... You add mass...

For a fluid cell: dm = density * dVolume

Think about what it means as pertains to your simulation.

diaw...

You can keep the temporal derivatives in a flow solver and still solve for steady state. If you approach a true steady solution then the temporal gradients will drive to zero. In the case of a steady flow the time step serves as nothing more than an iteration/relaxation step. However, if the flow should be unsteady (due to boundary conditions, external gradients, etc.) then obviously the time derivatives have physical meaning and relevance. Most of the flow solvers I am familiar with are actually coded up to handle the unsteady terms, although some provide an option to turn those terms off if the user KNOWS that the simulation will be steady. The rule of thumb that I follow (and most of the analysts I work with) is to use the unsteady formulation simply because for most of our work steady flows don't really exist. If you are running a solver that does not include the temporal derivatives and you are getting oscillatory behavior, then the solution is wrong. However, that does not mean that the real flow is unsteady, unless you have eliminated all other sources of error (code, boundary conditions, etc.)