# Wing in compressible flow convergence problem

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

February 25, 2017, 21:52
Wing in compressible flow convergence problem
#1
Member

Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 91
Rep Power: 6
Hi,

I am simulating compressible flow over a 737 wing approximately 20 m long (see pictures) at cruise conditions:
Pressure Farfield boundary conditions
Mach = 0.745
Angle of attack = 2.5 deg
Absolute pressure = 24998 Pa
Temperature = 220 k
Turbulence = Spalart-Allmaras
Coupled scheme
Second order for all the spatial discretizations
Pseudo Transient

My solution only converges to 3e-1. It doesn't even get to my target broad convergence value, which I set to 1e-3. Moreover, my results seem to be off. Although the 737 wing is real scale (and thus large), how can I get such high values for the coefficients? Lift coeff is 29!
Drag coeff = 2
Lift Coeff = 29

I am using a mesh which I believe is fine (see pictures).
Total number of elements = 6,203,332
Total number of nodes = 2,597,576
Wing face elements size = 5e-2 m
Inflation layers = 36 layers, 5e-4 m first layer thickness, 1.05 growth rate

So why my simulation is not converging? Do I need a finer mesh or finer inflation layers? Or something else could be causing the problem?
If you look at my residuals plot, you see that the values are stable although not converged to my target. Are the results still reliable if they are stable but not converged? I am very confused. Anything helps.

Thank you all!
Attached Images
 wing.PNG (29.9 KB, 36 views) wing_2.PNG (38.4 KB, 37 views) mesh.PNG (68.4 KB, 32 views) mesh_2.PNG (126.1 KB, 43 views) mesh_3.PNG (47.1 KB, 31 views)

February 25, 2017, 21:53
#2
Member

Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 91
Rep Power: 6
here are my plots
Attached Images
 Residuals plot.PNG (20.0 KB, 71 views) Lift coeff.PNG (16.9 KB, 42 views) Drag coeff.PNG (16.3 KB, 38 views)

 February 26, 2017, 19:53 #3 Senior Member   Lucky Tran Join Date: Apr 2011 Location: Orlando, FL USA Posts: 4,041 Rep Power: 49 For coefficient values: Make sure you have set all the reference values. For convergence: Your solution looks fine. Only the residual for the turbulent viscosity is high. Run the mesh check utility. A fine mesh is not necessarily a good mesh. It looks like there is a sharp transition between your inflation layers and core mesh, so that you end up with a very large volume change. This can limit your convergence. Also check if the skewness is high in these regions. This could easily be fixed by using a larger growth rate. e.g. 1.1 instead of 1.05. Also plot a contour of velocities and see if your prism layers cover the entire boundary layer, they should. But when generating fine meshes it's easy to make the prism layer thickness too thin. frossi likes this.

February 26, 2017, 20:00
#4
Member

Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 91
Rep Power: 6
Thank you for your answer. I made a more balanced mesh with a better transition between inflation layers and core mesh. I will see the results after the simulation is done.

For coeff values:
For what concerns the reference values, I am a little confused on how to use them. I used the default compute from farfield mesh, and this is what I got (see picture). The values for pressure, velocity, temperature, etc all makes sense, but the values of area and length are both set to 1. Is this the reason my my CL is off? To what should I set this values?

For convergence:
I thought the unconverged residual was continuity (white line). Isn't turbulent viscosity already converged (purple line)?

Thank you again for your patience.
Attached Images
 reference.PNG (10.9 KB, 33 views)

February 26, 2017, 21:04
#5
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,041
Rep Power: 49
Quote:
 Originally Posted by frossi Thank you for your answer. I made a more balanced mesh with a better transition between inflation layers and core mesh. I will see the results after the simulation is done. For coeff values: For what concerns the reference values, I am a little confused on how to use them. I used the default compute from farfield mesh, and this is what I got (see picture). The values for pressure, velocity, temperature, etc all makes sense, but the values of area and length are both set to 1. Is this the reason my my CL is off? To what should I set this values? For convergence: I thought the unconverged residual was continuity (white line). Isn't turbulent viscosity already converged (purple line)? Thank you again for your patience.
Make sure all the reference values on that page are correct. You don't need all of them. If you understand what lift and drag coefficients are (their definitions), then it is obvious that there are reference values and it will obvious which are the reference values you need. I don't care what boundary you used when you clicked "compute from" because what matters is that you must specify the correct reference values so that it is consistent with your definition of drag and lift coefficient. I can't tell you what the correct reference values are since I don't know what definition of drag and lift coefficient you are using.

The continuity residual is not scaled the same way as other variables (it's dependent on the initial guess). If you have a good initial guess, you'll have high continuity residuals. I would ignore the continuity residual. If you're okay with the turbulent viscosity then you're already done.

February 26, 2017, 21:38
#6
Member

Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 91
Rep Power: 6
Thank you so much!!! This is the best answer I ever got on this topic and it finally clarified a lot!!!

So, I define lift coeff with the standard CL formula:
CL = LIFT / (0.5 * density * velocity^2 * WingArea)
where WingArea is the projected area of my wing = 52 m^2
Based on this definition of CL, my CL is calculated using wing area instead of wing length. So for the reference values I would input 52 m^2 for area (since that is my wing area) and 0 for length (since I don't need it for my CL). Is this reasoning correct?

For the residuals:
When you say
Quote:
 Originally Posted by LuckyTran The continuity residual is not scaled the same way as other variables (it's dependent on the initial guess). If you have a good initial guess, you'll have high continuity residuals. I would ignore the continuity residual. If you're okay with the turbulent viscosity then you're already done.
Does it mean that continuity is not an important factor when assessing convergence? I am using a pressure based solver.
To test my hypothesis, I ran a simulation using a density based solver, but this time continuity converged, while z-velocity, x-velocity and turbulence didn't converge (see picture).
1. Should I ignore continuity in both solver types when it comes to assess convergence?
2. And what are the most important plots that I must look at to consider my simulation reliably converged?
3. What solver (pressure or density based) would you recommend for solving high speed subsonic flows (Mach = 0.745)?

Sorry for the many questions but you are very clear and I am understanding a lot from your explanations. Thanks!
Attached Images
 Density based.PNG (23.1 KB, 27 views)

February 26, 2017, 23:29
#7
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,041
Rep Power: 49
Quote:
 Originally Posted by frossi Thank you so much!!! This is the best answer I ever got on this topic and it finally clarified a lot!!! So, I define lift coeff with the standard CL formula: CL = LIFT / (0.5 * density * velocity^2 * WingArea) where WingArea is the projected area of my wing = 52 m^2 Based on this definition of CL, my CL is calculated using wing area instead of wing length. So for the reference values I would input 52 m^2 for area (since that is my wing area) and 0 for length (since I don't need it for my CL). Is this reasoning correct?
Yes, you've got it! Only the reference density, reference, velocity, and reference area are used in force coefficients.

If you initialize your flow with the exact solution, the continuity residuals get stuck at 1. Or if you reset your residuals right now, you'll see something similar.

Your plot of solution vs iteration is the best indicator of convergence.

You can use the pressure based solver, and I recommend it. It's much easier to use and pretty robust. The density based solver really saves you when you have shockwaves, but the pressure based solver can also handle those problems as long as you are careful. Start with the pressure based solver. If you want to switch to the density based solver after, you can.

February 27, 2017, 00:19
#8
Member

Ferruccio Rossi
Join Date: Jun 2016
Location: Melbourne, FL USA
Posts: 91
Rep Power: 6
Ok, got it.

Last thing , could you please clarify what you mean with:
Quote:
 Originally Posted by LuckyTran If you initialize your flow with the exact solution, the continuity residuals get stuck at 1. Or if you reset your residuals right now, you'll see something similar.
So I should I never look at continuity when assessing convergence?

and when you say
Quote:
 Originally Posted by LuckyTran Your plot of solution vs iteration is the best indicator of convergence.
What plots in particular should I make sure reach my convergence target for the simulation to be considered converged (x,y,z-velocity, turbulence, etc..)?
And what residual value is considered solid convergence (1e-4,1e-5...)?

February 27, 2017, 01:14
#9
Senior Member

Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,041
Rep Power: 49
People always ask for black and white answers and I am afraid I must never make them happy. I always answer yes and no.

It's a big mistake in the way we do education because people are always used to a problem with only one method and they know the solution and there's exactly 1 solution. In real life, you have a problem, no method, and no known solution.

Quote:
 Originally Posted by frossi Ok, got it. Last thing , could you please clarify what you mean with: So I should I never look at continuity when assessing convergence? and when you say What plots in particular should I make sure reach my convergence target for the simulation to be considered converged (x,y,z-velocity, turbulence, etc..)? And what residual value is considered solid convergence (1e-4,1e-5...)?

Residuals tell you the imbalances leftover when you say stuff = 0, and the stuff is not zero. Nothing is exact in numerics, so the user is always the one that defines the tolerance within which something is satisfied. You get to choose the residual levels. Residuals don't tell actually anything about convergence (because they don't tell you what the solution is). But you would think (intuitively) that if the solution is satisfying my governing equations more and more, that it's converging to a solution. This is a nice intuition to have, until you one day run into a problem that's bi-stable (a problem with two solutions).

The problem is the continuity residual is scaled in a way that's not very meaningful. If you have a horrible initial guess, the continuity residual drops rapidly. If you have a beautiful initial guess, it's stuck. It's a rather dumb residual unless you intentionally make a very bad initial guess. So if I make a an awesome initial guess, I can get to the answer in 200 iterations with a continuity residual of 1E-01; whereas you make can a horrible initial guess, arrive at the same answer in 20,000 iterations, and end up with a continuity residual of 1E-10. We both have the same solution but we have different continuity residuals! And if you look at how much the continuity residual has dropped, you would think that the person who makes the worst initial guess and wastes the most time computing has the "more converged" solution. Who would you rather hire?

For what purpose are you doing CFD? Are you doing CFD for the sake of watching residuals drop or are you doing CFD to get some sort of result? Some sort of sought-after-parameter? Whatever that reason is, monitor that variable because that's what you care about most. You want that result to converge.

But if that is too painful, then the next best things to check the basic variables, the variables that Fluent is actually solving for: x-velocity, y-velocity, z-velocity, pressure, temperature, turbulence, etc. But then you have to get creative and decide where to monitor these things. Again, you should decide. It needs to make sense. Obviously don't monitor the solution on your neighbor's machine. Monitor something in your solution. If you don't know where to look, then look anywhere (or everywhere).

My best advice is to just let Fluent iterate forever. Disable all the checks for convergence and just let it iterate forever. Go away from the computer. Your first few simulations should be done this way. Come back when you're bored (at least a whole day later, over a weekend is a good time to let it do this). Hopefully your simulation did not diverge and blow up. If it did, fix it. If it didn't, now you can sit down and view the results. Look at what happened to your monitors and residuals. And now decide where do you think the solution was converged?

 February 27, 2017, 01:20 #10 Member   Ferruccio Rossi Join Date: Jun 2016 Location: Melbourne, FL USA Posts: 91 Rep Power: 6 Thank you for your time. Your posts have been really useful. Much appreciated!

 Tags convergence, drag, lift, residuals, wing

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post nabidinhomessi Main CFD Forum 5 December 14, 2015 08:11 atheresia FLUENT 3 February 10, 2014 04:00 cinwendy FLUENT 0 April 17, 2013 03:19 challenger85 CFX 0 December 29, 2009 09:01 nick CFX 3 April 25, 2008 10:00

All times are GMT -4. The time now is 11:13.

 Contact Us - CFD Online - Privacy Statement - Top