[niteshrajput]

Hello all,

I am new to pointwise and CFD field. I am doing analysis on flow around NACA 0012. I have generated o-type mesh around the airfoil with diameter 20*c (c= chord length). But I was wondering changing the diameter will affect the results. The main purpose of increasing the diameter would be increasing the number of cells or there are other things that come into picture changing the diameter to 15*c or 25*c.

Please reply. Waiting for your response.

[pdp.aero]

Originally Posted by niteshrajput

Hello all,

I am new to pointwise and CFD field. I am doing analysis on flow around NACA 0012. I have generated o-type mesh around the airfoil with diameter 20*c (c= chord length). But I was wondering changing the diameter will affect the results. The main purpose of increasing the diameter would be increasing the number of cells or there are other things that come into picture changing the diameter to 15*c or 25*c.

Please reply. Waiting for your response.

Hello,

Generally speaking, for comparing the CFD-based analyses, you might do domain study or grid study. In the domain study, we are changing the domain's size or its shape in order to compare the results. In this case, when we obtained approximately same results while we have been changing the domain's size, we could say that the results are not depending on the domain's size, so they are accurate enough to be used. In the grid study, we are changing the grid's size to show that by increasing the number of cells the results won't change, and they are not depending on number of cells. However, when you are using a structured grid, by increasing the domain diameter, you are increasing the number of the cells or the mesh resolution, and consequently different results will be obtained. Please note, generally, the results which are aerodynamic coefficients in your case won't change a lot, if the equations have been converged appropriately in the case of an airfoil. However you might double check on the Cp distribution, the shock location to make sure that your equations are really converged.

This is the ways that generally are introduced to make an accurate simulation, but the fact is the governing equations that you are iterating and the computational methods that you are implementing for your simulation affects the results which will be obtained by the change of the resolution or size of the domain. For example, if you are running in Fluent, because of the limiter implemented by solver to ease the convergence, in case you are using compressible solver with 2nd-order discretization, you will find better results by using bigger domains. The reason is, in the bigger domains, the reflected shocks from the far filed will be eliminated and you will recover the pressure very well. Following this further, in the high order methods you would be obtained pretty accurate results with the coarse grid.
For the two-dimensional compressible Euler or RANS equations, in particular NACA 0012 with Mach 0.8 and AoA 1.25 degree, using AUSM, Roe, HLLC, JST or even CUSP and other methods, you could acquire pretty accurate results with structured O-topo domain which has 20C diameter, albeit with appropriate initial distance in your boundary layer grid (e.g. 1e-05 m) in case you are running RANS. Besides, you would compare your results with the AGARD on the NACA 0012 case, and make your experience for running a CFD simulation.

Good Luck,
PDP

[niteshrajput]

Hello and Thank you so much.
I would surely do that grid study for convergence.
I am using unstructured o-topo mesh. Also I am comparing my results with AGARD Report , M = 0.3, Re= 2.7*e6. What would you suggest to be the turbulence model. I used SA method but results were not very much accordance with the AGARD. I tried using Laminar, in this case the results were following the trend of report but there was a lot of wavy spikes in the results, it wasnt a smooth curve for Cl values and also for Cm values.

[pdp.aero]

Originally Posted by niteshrajput

Hello and Thank you so much.
I would surely do that grid study for convergence.
I am using unstructured o-topo mesh. Also I am comparing my results with AGARD Report , M = 0.3, Re= 2.7*e6. What would you suggest to be the turbulence model. I used SA method but results were not very much accordance with the AGARD. I tried using Laminar, in this case the results were following the trend of report but there was a lot of wavy spikes in the results, it wasnt a smooth curve for Cl values and also for Cm values.

Your Reynolds number is beyond the laminar (e.g. beyond the 5e+5), so you need to use a turbulence model. My suggestion is K-omega (SST) because its convergence is accurate for most external flow's test cases, speaking from the experiences. However, obtaining the convergence with this model would be difficult. Therefore, using the structured grid with approximately 40K cells and 50C domain's diameter would improve your results.

Please note that you are calculating your Reynolds number correctly based on your flow condition, I mean the pressure, temperature and other factors. Besides, more information about your solver would be helpful for me. Further, in case you are iterating the steady-state solver, you would change into the unsteady with approximately big time step. The sway, fluctuation or wavy spikes in your Cp distribution or Cl and Cm's convergence history probably emerges because of the unstructured grid. Using the structured mesh will improve the results.