## Fluids

#### How extract Cd and Cl and find the angle?

• José Mantovani
Subscriber

Hello everyone!

I make a simulation of 2D aerodynamic profile analysis with rotate mesh region to do a attack angle without need use velocity components method. I use the uniform and normal velocity and the airfoil rotate. The simulation is transient. Like in image below.

I can see the Cl chart over the flow time or iterations and the same for Cd. But is there any possibility, taking manually, for me to plot Cd or Cl by angle? Why can I do this with each timestep estimating the angle and seeing what the result is at each step, but this is a time consuming manual process. Is there any way?

Thanks for help and opportunity!

Mantovani.

• José Mantovani
Subscriber

I set it up, the region mesh which rotate, with -0.2875 rad/s.

The Cl x timestep (or iteration) graph demonstrates a behavior very similar to a possible Cl x alpha graph for the same profile. I wanted to know how to relate the iterations / time step to the angle. I thought of doing this manually, opening each file saved from the transient solution by checking Cl and Cd and measuring at what angle the profile is.

If the only way to do this is manually, how can I measure the angle at which the profile is?

Thanks one more time!

Mantovani.

• jabanto
Ansys Employee

Hello Jose

My understanding is that you performed several simulations on the profile by rotating the mesh in the preprocessor with an angle representing the angle of attack. I assume when you said 'rotating the mesh' you actually rotated the geometry and mesh it, so you remeshed the geometry if you used Workbench. This is a good approach to estimate CL=f(alpha), or CD=g(alpha) compared to the traditional way by defining the boundary conditions at the inlet by velocity components or by direction vector. I think you want to get a table or plot of CD, or CL, or CM versus angle of attack. Unfortunately you can get such table or plot only manually running Fluent in standalone mode, outside workbench. In order to get that table or plot in a more automatic way you can use Fluent in workbench with parameterization, where the angle of attack (alpha) is a geometry parameter, and by defining a Table of Design Points in Workbench, the aerodynamic coefficients, output parameters from Fluent, will be transferred to workbench to complete the Table of Design Points. This methodology however requires a remeshing process in ANSYS Meshing, but I think this is what you did. The other possibility (more efficient) is, keeping the same mesh, you could define an input parameter to rotate the mesh in Fluent, however this option is not supported yet as a regular feature.

I hope this helps.

Juan Abanto, ANSYS customer support

• cfd_learner
Subscriber

As far as I understand, this is a rotating airfoil problem, rotating with 0.5 rad/s. I don't know exactly whether UDF can solve your problem that instead of plotting coefficients with time , it may plot into AoA.

You need to convert Time Step into angle like:

1 s = 0.5 rad (28.6479 deg)

accordingly, you can convert your time step into the angle. This could be done manually after finishing simulation either in Excel or in CFD Post (by defining a new variable).

Or, try to override Fluent plots by defining UDF (I don't know exactly how to do this), but I thic=nk it is possible.

Hope it works.

• José Mantovani
Subscriber

Hello guys, thanks for helping!

To make it easy for you to understand how I did it, was this. I created a C-type domain, with the aerodynamic profile with the leading edge aligned at the XY origin, the chord length is 0.575 m. So I created a circle with the center halfway down the chord length 0.2875m.

Then I made the mesh and such, and in FLUENT, I set the rotation as follows in the image below.

So, by logic, I thought. Well if I set a time step of 0.005s in 400 time steps, I'll have a 2s flow. As I set 0.2875 rad / s in 2s, my domain will have turned 33 °. So I tried to correlate the flow time with the angles by imagining that the FLUENT would rotate it in a regular way over the time steps. However, I would only be interested in the range between 0 ° and 20 ° so in the time step coinciding with 20 ° I plotted a graph as below.

The red curve has the result from the simulation in the FLUENT to the given Reynolds number and the blue curve from an analysis in the XFLR5 software to the same Reynolds value. The problem is that the simulation in FLUENT changes so we can see stolen angle, as far as I can imagine, or because the correlation of flow time with the angle is wrong or properly due to coarse mesh.

I decided to try to simulate this way, because when I impose the angle of attack through the velocity components and use a fixed mesh, the values are not satisfactory, the values do not assume as the XFLR5 or an experimental date for that airfoil. The best I could do was this, however as you see this graph in my opinion is not acceptable because it moved the stall angle compared to the XLFR5.

I believe the biggest problem to simulate this type of profile, in the case the S1223, because it is not a symmetric profile so I do not even know if there is possibility to create a structured mesh for it. I find on the internet several tutorials, but they use only symmetric profiles (which is very easy, right?), I'm trying because I need this for my SAE Aerodesign team, and I want to share with everyone here in the community and abroad, because there are no tutorials for non-symmetric profiles.

I simulated again this time setting to 0.1745 rad / s which in 2s would give me 20 °. I have not worked on the results yet, I will do this and share it with you. Now that I have exploded more visibly how I did the simulation, can you give me any more ideas?

Thanks for opportunity, attetion, and helping!

Mantovani.

• klu
Ansys Employee

Hi Jose,

I do not think there are problems with the dynamic mesh approach itself. However I would suggest:

1. Confirm whether the settings used in XFLR5 and Fluent are fully comparable, for example air properties, velocity components, etc.

2. Double check if the angles in XFLR5 and Fluent are identical.

3. Check if the turbulence model is appropriate.

4. Make sure the mesh is good enough to obtain correct CL and CD. A mesh independence study would be recommended.

5. Make sure that definitions of CL and CD are the same in both XFLR5 and Fluent.

6. Confirm the simulation is converged at each time step. You might simply run a steady analysis on one particular angle and compare the results.

Lastly, please attach the case and data files of one angle for further investigations if necessary.

Thanks.

• cfd_learner
Subscriber

Apart from the above reply, check this also:

I don't understand why you are using dynamic meshing? It looks like a steady-state problem. A more convenient way is to define Design Points in Ansys WB by creating "AOA" a parameter in Design Modeler. This will make your life easy. In the parametric analysis, you only need to change geometric AoA and define output parameters like CD, CL from Fluent. This way you can plot directly Lift and Drag curves with AoA in Ansys.

Using dynamic meshing may create stretched cells causing lack of accuracy and the convergence at each time step may also not be appropriate. So, go for parametric analysis. The same workload in this case compared to dynamic meshing.

I don't know what Turbulence model you are trying whether it is necessary to use or not, check this! SA turbulence model is appropriate for Aerodynamic predictions.

Hope it helps.

• José Mantovani
Subscriber

Thank's for help and suggestion my friends!

I tried to generate a structured mesh for this profile (now to use fixed mesh, imposing attack angle on velocity inlet components) but the region behind the profile gives me an error. Can you give me a glimpse of how I can generate a structured mesh for this non-symmetric profile? Funny that I did a test for a symmetric profile (NACA00012) and I had the same error ... I think it's a bug, I do not know. While not responding I try here.

Soon more if I can not, I'll create a topic in the mesh generation tab.

One more time, very very very thank's for help and opportunity.

Mantovani.

• KikoAzor
Subscriber

Hello José, Can I ask you and advice, please? I am new to CFD community, so maybe my explanation will not be correct. It seems like I am facing the same problem as you did..  I am working on my diploma thesis, and for it I am simulating flow over a 2D airfoil (with ice accretion and clean). I am managed to do it according to one video on youtube https://www.youtube.com/watch?v=G0zAHv0rEa8 ... I am trying to simulate a rotating 2D airfoil (like it's in different angles of attack), by creating to interface zones one is fluid, and the other one is inside of it - rotating - inside this one is my airfoil as a rotating wall... I managed to do the simulation and everything, I just cannot get the right numbers of drag coefficient, lift coefficient and moment coefficient... which is actually essential for my diploma... In the picture, you can see that the numbers of Cl are too high which it usually ranges from 0 to 1,8 max... Do you know how I could get the right number or where could be the problem? Thank you so much! I would be very very grateful if you could give me some hint...