Learning Forum

[smalbro93]

I am running a k-w SST model with the first boundary layer around D/1000 (D here is the depth of the Bluff body) and I want to run the simulation without Wall Function.n

[Rob]

If y+ is high enough you sort of ignore the wall functions, what are you trying to do? n

[smalbro93]

Do you mean Y+ low enough? I am trying to carry out a URANS simulation on a D/1000 mesh (Circular domain with a square cylinder in the center). The mesh is quite fine so I want to remove the wall function and model the flow. I can't find how to remove the wall function. nI was running the simulation earlier on the same mesh (D/1000 imported from pointwise) and received a Floating Point error (divergence detected) and I wanted to run it once without the wall function just to see if it's including the wall function is causing the problem since the mesh is quite fine.nI will be doing finer meshes also so I want to know how to model without using Wall Function. Thank you for your guidance.n

[Rob]

No, coarse that way the turbulence model won't really see the wall so wall functions don't really do anything. The solution isn't accurate near the wall but may not matter in some models. nIf you want to resolve the sub layer refine the mesh and the model will deal with it, that's what k-w is designed for. Wall functions are there to transition from near wall to far field, and k-w has built in functions for this (in k-e we define a wall function and it is on unless the mesh is very coarse). nDivergence is likely caused by something else. How well converged is each time step? n

[smalbro93]

Array Thank you for your response. nRegarding: If you want to resolve the sub-layer refine the mesh and the model will deal with it, that's what k-w is designed for.nBy refine, how fine are you suggesting? A y+ value less than 1? When do I know that k-w SST isn't using a wall function for the simulation?nRegarding: Wall functions are there to transition from near wall to far-field, and k-w has built-in functions for this (in k-e we define a wall function and it is on unless the mesh is very coarse)nThank you for the explanation. According to my understanding Wall Functions automatically model the flow transition from the near-wall to outwards. Based on this shouldn't the wall function be off unless the mesh is very coarse, i.e., it's off for fine mesh and on for coarse mesh? nRegarding the divergence issue:nI am really stuck with this one.nBackground: I had tried running the Unsteady Simulation previously with k-w SST. Mesh is quite fine, first layer height is 0.0001 m. U= 1m/s. For Courant No. = 1; from Courant No. = U x TimeStepSize / FirstLayerHeight we need a time-step size of 0.0001. Using this time step I was getting a courant number less than 5 but nowhere near 1. I tried running it will different models (K-W SST, k-e, tried running Steady Simulation, Laminar Model) but it always gave me Floating Point Error!nLast time, I again ran the Unsteady simulation with K-W SST but with a very low time step (TimeStepSize = 0.00001 sec) and the unsteady simulation continued without error. It was very slow (even without Data Sampling), I got 1.5 seconds worth of simulation in 3 days. The courant number was low (around 0.5) and the simulation was stable (running without error) but the Cd and Cl were nowhere stable (I mean Periodic). The residuals were almost constant, fluctuating around the same value (Pressure Continuity: 1e-4, X-Velocity, and Omega: 1e-7, and Y velocity: 1e-8.nIt was very slow so I decided to change the time step size to 0.0005 sec [it is the only thing I did and nothing else] and instantly it showed Floating Point Error! the courant number sky-rockets, residuals shot up to 1e+8, Cd and Cl shoot up to 4.5e+9, y+ around 90k. When I check the velocity (mean) contour, velocity shoots up to NAN(infinity).nI tried changing the timestep size back to TimeStepSize = 0.00001 sec (which had initially worked for 3 days) but then again it kept showing the error. I am not sure what is wrong. Any idea or help is appreciated.nAdditional Notes: The mesh has been imported from PointWise. My colleague is running the exact same mesh in OpenFoam and doesn't have any issues. I have imported PointWise mesh earlier to fluent and it worked flawlessly. The Domain is Circular.nP.S. Please let me know if any additional details are required. Thanks.n

[smalbro93]

I also tried changing schemes after reinitializing the problem again. But changing schemes and models doesn't help iit continuously gives me Floating Point Error. Changing Models and Schemes doesn't help at all.n

[smalbro93]

Before running the simulation I tried the below command to remove the wall function for k-w SST and the simulation runs without any Error! even at 0.0001 TimeStepSize:n(rpsetvar 'kw-set-wall-w? #t) nI don't understand it though.n

[smalbro93]

I suppose running the fine mesh with wall function was kind of conflicting? nI am also not sure what chain of actions or changes the above command makes to the simulation though.n

[smalbro93]

I tried leaving the Solution running. It ran without error but even after running for a day and a night (close to 6 seconds of simulation time), the Cd and Cl are weird and nowhere close to stabilizing (converging). I tried increasing the time-step again (from 0.0001 to 0.0005 and I get the same Floating Point Error).nDo you have any guesses as to what is wrong and what I can do?nThanks.n

[Rob]

We're both on holiday, so you may find we're not on much until next year. The US & APAC teams are around though.nnRe y+. It's there to help guide the FIRST cell height. To resolve the near wall flow you then need many more layers in the near wall region such that you have 15-20 layers INSIDE the viscous sublayer. A y+ of around 1 is a good starting point, but you may need to refine the mesh further (via adaption) once you know how thick the sublayer is. nWith a very coarse mesh I have my first cell centre outside the sublayer and probably outside the whole near wall velocity gradient so am ignoring all the near wall treatments. This isn't recommended for most applications, but is a useful approach when used with care and sufficient experience: you're not there yet! nThe stability issue is likely linked to the inflation: look for flow separation. If you have this in regions with high aspect ratio (ie where you have a low y+) you need to refine the mesh in the streamwise direction as you're not resolving the flow separation/reattachment sufficiently. n

[smalbro93]

Hi Rob, thank you for taking the time to answer the question. I understand it now. Thank you.n