SimScale CAE Forum

CFD - Wing Flow Simulation

Hello- I have a wing construction that I would like to simulate a few different ways. The first way is with straight-on, zero-degree of attack flow, then try to work in transverse flow (outboard flow on bottom, inboard on top surface) to see the effect the tip shaping I have done has on the wing. I am aiming to tailor the vortice flow off of the wing tip, and this is a beginning for that process.
I have tried this a few times, and I am slowly understanding the process… but this is a large tool box full of tools that I am not fully versed in. Can anyone provide some direction from this point so I can get some useable data?
I have successfully uploaded the geometry as ‘t5’ and performed a surface splitting operation to it, it is in the public file ‘Wing1’. I then made a mesh as ‘t5 Mesh’.
Thank you in advance, I am looking forward to getting much more familiar with SimScale in this new year—

Dave

Hi @dtriano!

I think Darren (@1318980) has done quite a lot of simulations on wings if I am not mistaken so he might give you some good input on your project. Please also share the direct link to your project which makes it easier for us to know what project you are talking about.

Thanks and all the best!

Jousef

Thank you Jousef! The direct link is https://www.simscale.com/projects/dtriano/wing1/

D

Hi @dtriano!

While Darren will be able to give you a full description of how to go about doing this analysis, I can try start you off with the basics!

So generally speaking there are several parts to achieving your end results, all of which have their different quirks and potential problems. To simplify everything here are the general steps I take:

  1. Meshing of geometry
  2. Simulation of geometry
  3. Convergence of results
  4. Post-processing and data extraction
  5. Validation of results

On top of this, I usually go for a general simulation first to get my base results out then work from there to further increase accuracy rather than trying to get everything right from the get-go.

You must first also know what environment you are simulating in, is it compressible or incompressible flow? Do you have all your values for flow velocity? Ambient pressure? Density? All these will affect your simulation.

Meshing of geometry
This step is probably one of the most difficult to get right as you have to contend with numerous settings. For a wing like yours I’d recommend a few things:

  • A large enough bounding box to contain your wing and allow flow to develop before reaching your wing
  • Boundary layer inflation
  • Surface refinement for the wing
  • Region refinement encompassing the wing and another even finer region refinement for the area near at tip where your area of interest is

The meshing part is where things like the Y+ value for determining near wall functions to ensure accuracy all come in. Darren can better give input on this part. The meshing stage is where you usually determine accuracy of the simulation, if the simulation isn’t accurate enough, its usually the quality of the mesh that isn’t good enough. At least that’s what I’ve encountered.

Simulation of geometry
Simulation is slightly simpler if you are doing incompressible flow (which I will assume as such for the rest of this post), there are less considerations and convergence is usually easier since your geometry is also not extremely complex. You would probably want to start off with a steady-state simulation to get a general result out for validation later. Regarding the turbulence model, k-omega SST is a good choice for now. If you want to read more about turbulence models, you can do so here and here.

After deciding our simulation type we can move on to the initial conditions which is based off of what environment you want to simulate in and any other required initial conditions. Then we go on to the boundary conditions.

Boundary conditions are in essence the “rules of the simulation”. We need to define these conditions carefully to ensure our simulation is behaving as intended. So for your case, we need to define several things:

  1. Inlet velocity and direction
    Defined as the “speed” of your flow and whether it is a positive or negative value depends on where the wing is “heading” to, which from your project is the negative x-direction hence your velocity should be input in the x value but negative in value.
  2. Outlet condition
    We want your flow to progress “naturally” through the computational domain so you can set the outlet to pressure outlet with value of 0
  3. Bounding box condition
    Generally to represent “free air” I set the the condition for the bounding box to a wall with slip condition.
  4. Geometry condition
    This is the simplest, your geometry has to be solid so its just a no-slip wall.

Next we need to set your simulation control. The only things we need to change is the End Time Value, Write Control, Write interval, Number of computing cores and Maximum run time.

  • End Time Value
    This is hard to define at first, so I generally set an arbitrary number about 500s to see if the results converge well.
  • Write control
    Adjustable timestep is the one I usually use
  • Write interval
    Since this is a steady-state simulation you don’t really need that many in-between values, so saving just the start, middle and end with a value of 250s for 500s end time is alright
  • Number of computing cores
    32 cores
  • Maximum run time
    This is a preventive measure to stop “run away” simulations from eating up your core hours. Just set yours to about 80,000 and it should let your simulation run with no issues

Then we can define result control. Result control is a mixed bag as you have to know what you’re looking for. For my input, setting the result control will allow you to see if the values are converged. This I don’t have much of an input so I’ll let Darren help you out with this. In the meantime if you really want to run the simulation you don’t absolutely have to set this up.

Then from there you can start your simulation under Simulation Runs and leave it till it (hopefully) completes.

Convergence of results
Convergence is basically a way to see if your simulation is “unrealistic” or not. While it is hard and rather complicated to get “good” convergence, the criteria for it is based on either your given task’s acceptable convergence criteria or some general value that is acceptable to you. You can read more about it here. In general, 1E-4 is what most area deem convergence as “acceptable”.

Post-processing and data extraction
This is probably the most difficult part for me to help you on. I do my post-processing in ParaView and for my projects and what I’ve experienced my parts are not that complicated. But for yours, determining what values to obtain, where to obtain and compare them, how to obtain them in ParaView can quite difficult to do. Darren may be able to provide your some insight on this part.

Validation of results
There are a number of ways to validate a simulation/result. For your case, I would do a simple CL vs AOA validation and compare the results that you have simulated against a calculated or experimentally plotted result. If you trend is there and your values are relatively close to the referral case then you can deem that whatever results you have obtained from the solver is usable and a valid data point. If that is not the case then we have to look back to each of our individual steps and to see where this can be improved.

Hopefully I didn’t miss anything out and if anyone has any input regarding what I mentioned feel free to correct me! This should get you started somewhat and optimistically you’ll be able to at least get out a result even if it isn’t exactly accurate.

Cheers and feel free to ask anyone here for more help!

Regards,
Barry

3 Likes

Thank you Barry! I am trying to construct a new mesh with more space in the Cartesian box, inflated boundary layer, and at a higher quality level, then I will follow your directions and report back–

Best - DT

I had another go at it, which can be found at

https://www.simscale.com/workbench/?pid=4296772073540011421#tab_2-0

and the convergence plot can be seen at

https://www.simscale.com/workbench/?pid=4296772073540011421#tab_2-0

Please have a look and let me know if I am making progress…

Best - DT

Hi @dtriano,

Convergence for the second run looks good. The mesh might need some changes but you do need to validate your results first to see if there is any need for additional work and how far off you are.

Cheers.

Regards,
Barry