problem getting shock-wave to show
 

Hi, im using fluent to solve for the 2d transonic flow around a RAE2822 airfoil. I have meshed the geometry using ICEM. When solving the case in Fluent I am unable to get the shock-wave to show (I have the solution to the problem and am aware of where the shock should be). I am able to get the residuals to converge (even the continuity which takes a long time) when using the explicit relaxation factors of 0.5 for both the pressure and momentum and under-relaxation factor of 0.6 and 0.8 for the density and modified turbulent viscosity (all other factors were left at 1). Also im using a second order upwind discretization scheme for all properties. Interestingly as a side note, if I leave the relaxation fators at the default setting the solution doesnt coverge but if i plot the pressure contours after about 60 iterations (b4 the solution diverges) the shock is present. I was wondering if there could be any cause for my shock to not be present besides perhaps the grid needing modification. Im asking because im prety sure the grid is appropriate for the problem its a structured grid C-grid with 2 stages. It has a spacing of 0.003 off the wall and has 120 nodes across each of the airfoils upper and lower surfaces (airfoil chord normalized to 1ft). Thanks for any and all help

shock capture
 

so i have now been able to capture the shock by switching the solver from the coupled pressure based to the density based. After about 500 iterations i am able to get a fairly clear shock formation along the suction side. However, the shock is at the wrong location its ahead of where it should be by about 10% of the chord length. I started with the S-A turbulence model and have now switched to the SST transition model to c if it would provide more accurate results however it again captures the shock about 10% ahead of where it should. any ideas? thanks in advance

hi,

Check if you have specified the flow conditions that match the Mach Number and Reynolds Number of the experimental data.

Try splitting the domain into few more blocks and cluster nodes near the anticipated shock location.

Try shifting to higher order flux types.

Cheers

fixed one problem but now another arose
 

Thanks for your advice k_k. I noticed that using the pressure solver I needed a very large ammount of nodes across the airfoil and especially in the shock capture zone. So I switched to the density based solver and it really helped so i have only 120 nodes across my airfoil and i am able to capture the shock quite well. Also I noticed I had an error in the geometry file so Ive corrected that. With the grid refinement, solver change and geometry change Ive been able to get the shock to within 3% of the chord length of where it should be.

However, now when runing the case ive noticed the scaled residuals begine to oscillate a great deal as higher itteration numbers are approached. Ive found that by changing the off the wall spaceing I can control this oscillation slitghtly and found an off the wall spacing of 7.5e-4 to be best (spacing increases at a rate of 1.2 outward). At this value the residuals will oscillate slightly but as they approach a converged solution. Any smaller the off the wall spaceing, once the residuals converge to 1e-2 they will oscillate around this value. Any larger the spacing and very large oscillations will begin to occur. I was wondering what else could be the cause of these oscillations and how i could control them? Additionally, why would a smaller off the wall spacing hinder the convergence? Shouldnt it help considering in transonic flight the gradients in the +y direction are exceptionally large.

hi,

the first node location from the wall has to be decided on the Reynolds Number, boundary layer characteristics and Y+, and should not be selected arbitrarily.

Usualy, the ratio between the size of the smallest to the largest cell determines the rate of convergence. Because, the solution developes relatively slow in smaller cells.

There are many factors that kick off oscillations of the residuals.

1. If the problem is very tough and highly unsteady
2. Some turbulence models suffer at certain range of wall y+
3. Inconsistency of the grid.

I suggest you to start the solution with very low CFL number if you are running a steady case. You can shift to higher CFL numbers after few 100 iterations.

Cheers