Strange Results
 

Hey,

So I trying to learn ANSYS for my school's FSAE team; However, I am having two large problems while trying to simulate 2D flow over an aerofoil that is close to the ground for ground effect.

First, Whenever I attempt to run an animation of any sort (I have been trying time-step) it simply does not animate it. For example, it just plays an animation with 2 frames. One with no data, and one with all the data. Whenever I actually ran my calculations, I set "time step size" to 0.01, "number of Time Steps" to 150, and "Max iterations/ Time Step" to 20. We've been trying to figure it out for some time now and have had no luck.

Second, on every aerofoil I have run a simulation on it always gives me this strange almost vortex like pattern on the low pressure side of the aerofoil. Almost like balls of low pressure near the back. It shows strange flow separation patterns yet we are simulation the aerofoil at its optimum angle of attack for best cl/cd. I am not sure what mistakes we are making because this has been happening on every aerofoil we have simulated.

Thank you so much for any help.

Attachment 65706

Attachment 65707

You set up the number of timesteps fluent should calculate. It won't save the data from every timestep. You should try an automatic export in 'calculation activities'. It allows you to write multiple files according to your defined frequency.



We need more information to answer your question with the flowfield. For me, it looks like your flow is becoming from laminar to turbulent where your have your vortices. What kind of mesh do you use? Which turbulent model? How fast is your flow?



Greetings
sufjanst

I used a triangle mesh with 10 layers of small boxed near the surface of the airfoil. I do not know what a turbulence model is but my flow speed in 11.175m/s and my airfoil is at a 6 degree angle of attack. Again this is for a formula style car.

Thank you very much. I am a student and I am completely new to this so any help is great.

Also you solved my animation problem, thank you.



EDIT:

My Time (general setting) is Transient.
Viscous Model is Laminar
Under Method, my Transient Formulation is: Second Order Implicit
Initialize: Hybrid
Time Step Size: 0.01
Number of Time Steps 150
Max Iterations/Time Step: 25


Second EDIT:

Also another question is what relation does the Max Iterations/ Time Step have on your simulation? Does having more It/TS increase the accuracy of each time step by averaging multiple results? or is it something completely different?

It increases accuracy but nothing to do with averaging. Have you used any iterative solver before? For example maybe a root finding algorithm?

You are using an iterative solver to solve for the solution at each time-step. At every time-step, you need to make sure you converge to within some tolerance. The number of iterations per time-step is one such knob of ensuring this accuracy. If you don't care about accuracy then you can arbitrarily set it to any number like 1 and watch it blow up.

So how can I determine what value for this? Is 20 good or poor.

My "Scaled Residuals" graph never seems to converge even after 10,000 iterations. Is this because my number of iterations is too low and I am just running a ton of iterations via increasing number of time steps? I have attached a screenshot.

Also, is the effect I described in my original post "Vortex Shredding"?


EDIT: Should I even be running a 2D airfoil sim as transient?

What are the physics you are using for your problem? The residuals not reducing could be due to many things; it could be a poor mesh, it could be trying to solve a turbulent problem with the laminar solver...

I am new to this. By physics are you referring to viscous model? In that case I am doing Laminar. I am very unfamiliar with the turbulence models and I cant seem to find anywhere to learn relatively easily.

Well, there you go. Indeed the viscous model is the most important thing to properly set. If you have a turbulent flow, the laminar model is not going to do it for you. If you don't know a lot about turbulence models, you should try and learn something about those, before just randomly assuming a model. It's extremely easy to set up a simulation in FLUENT - the challenge of CFD is in setting up a simulation that actually has physical meaning, and for that you'll need to know what's behind the buttons you are clicking.

Of course, you don't need to delve into all the details of turbulence (that is a career in itself), but you should know the basics; how do turbulence models work, what are strengths and weaknesses of various models, and which one suits the physics of my problem best. Compare it with driving a car - you don't need to be able to build one from scratch, but it's damn useful to know what the various buttons on the dashboard do if you want to use it, and to have a general understanding of the different parts under the hood if you want to do so professionally.

I figured that was the case. My only problem is i have yet to find a good source to explain them. I guess ill just look harder. Thank you.

There's plenty of sources out there (probably, the challenge is not to drown in sources). I like Versteeg and Malalasekera as an introduction to CFD; it's old but it has the basics. If you want to go more into turbulence itself, Pope is a popular one. But if you want to stick more on the introduction level, and want to know which turbulence models best suit your goal (after picking up the basics from an introductionary CFD book or course), you can get a long way with wiki (both the wiki here and wikipedia) + a few journal papers on similar cases. Good luck!

[QUOTE=Lukeyfish;707501]So how can I determine what value for this? Is 20 good or poor. /QUOTE]


1) Residuals certainly help

2) Create a point monitor (you find it in surfaces) and monitor the velocity or pressure at this point. The value of that monitor should converge after # iterations to some precision. E.g. you should see it eventually converge to say 11.01 m/s, 11.02 m/s, 11.01 m/s, etc. If you see 11 m/s, 15 m/s, 10 m/s then you know you are in trouble.



I noticed you have a time-step of 0.01s which seems quite arbitrary and this is probably way to big to capture any transient phenomenon if there is any. I'm not sure why you are running a transient simulation and not a steady one if you don't expect vortex shedding. If you run transient though, then check the Courant number variable and make sure the maximum is <10 or so (a lot of people will tell you to go much lower like 0.1 or 0.5). 11 m/s and time-step of 0.01 means your smallest cell size would need to be 100mm to have a small enough Courant number. I'm guessing your cells are way finer than that and you need to make your time-step much smaller if you want to see anything. When you run with a very large time-step and a very large Courant number, it's acting more like a steady solver than a transient solver.