[Josh]

Hello -

Before I begin, I have read the manual and have done all of the tutorials.

I am running a 2-dimensional (2-D Extruded Mesh) simulation of a NACA 0012 airfoil. I used the "Flow from a Circular Vent" tutorial to help model both a steady state and transient analysis. I created a fluid domain for the surrounding rectangular prism (15 m long, 4 m high, 1 m wide (but with symmetry and 2-D mesh extrusion)) and a solid, steel domain for the airfoil (1 m long) itself.

In the Transient Analysis, I configured CFX-Pre so that the Fluid Domain remains stationary while the Airfoil Domain rotates about the z-axis (the x- and y-axes represent the 2-dimensional Cartesian plane; hence a rotation about z changes the angle of attack) at some prescribed angular velocity (I have tried various, from 0.05 rad/s to 1 rad/s). The fluid domain has an axial velocity of 0.65 m/s.


Although both the steady state and transient analyses run and converge successfully, I have the following problems in CFX-Post:

1. The airfoil has not physically (visibly) moved, even when I click on various timesteps (from 0 s to 30 s).
2. The changes in pressure, velocity, and streamlines around the airfoil are qualitatively negligible.
3. The animation tool does not produce results for the streamlines.

Basically, I'd like to create a nice animation of the angle of attack slowly increasing from 0 degrees to 15 degrees and model the change in pressure or streamlines.

Thanks for your help.

[Josh]

Hello -

I managed to run the airfoil simulation with a changing angle of attack. I changed the airfoil from a "Solid" to an "Immersed Solid". The animation now produces a moving airfoil. My problem now is this:

Because I have 2 domains (immersed solid airfoil and fluid), the airfoil appears in both. In one, the airfoil is the domain and it is rotating. In the other (the fluid domain), the airfoil is just a boundary within the domain. In CFX-Post, the airfoils from both domains are present (the rotating and stationary). This causes a problem because the results are treated as if there are 2 airfoils - 1 rotating, 1 stationary at 0 degree AoA.

How can I eliminate the stationary airfoil?

[ghorrocks]

Hi Josh,

Immersed solid is unlikely to be a good approach for airfoil modelling. It does not allow capturing of the airfoil boundary layer very well. What Re number is it running at? What Mach number? Any other physics of importance?

If you could post an image of your geometry that would be good.

I recommend you model this with the airfoil being a cut out section in a fluid domain. Then the easiest way of implementing the airfoil motion sounds like putting it is a rotating frame of reference and join it to the outer stationary frame of reference with a GGI on transient rotor/stator mode. You can do this with mesh motion but that is much more complicated and will be a far slower simulation.

Also it sounds like your domain is quite close to the airfoil. If you are trying to get the infinite field results you will have significant error. Do a sensitivity analysis to find how far the outer boundaries need to be away from the airfoil.

Glenn Horrocks

[ckleanth]

first theres a few model the profile movement and these are described here http://www.cfd-online.com/Forums/cfx...-sloshing.html

I'm not sure if you have made this error but if you use imersed solids the mesh for the fluid and imersed solid component must be separate and independant.

[Josh]

Thanks for the replies.

Here are some details ...

Geometry

I did model the airfoil as a cutout from the fluid domain. I used "Point" to import my airfoil, created a spline of half the airfoil profile, extruded the half-profile, and used a Body Operation to mirror the half-profile to create a full, symmetrical profile. I then froze that full airfoil profile, created a second sketch of the fluid domain surrounding the airfoil, and extruded that. Finally, I used another Body Operation to cut the airfoil out of the fluid domain, which created 2 Parts, 2 Bodies. My geometry profile can be found below:

http://picasaweb.google.com/counse/C...eat=directlink

Mesh

Pictures of my mesh scheme can be found in the same album:

http://picasaweb.google.com/counse/C...eat=directlink

I have 6 regions: Inlet, Outlet, Left, Right, Default 2D Region (the top and bottom), and Airfoil.
My Default Body Spacing is 0.1 m.
I used Line Control around the airfoil with a radius of 0.6 m, length scale 0.01 m, and expansion factor of 1.2.
I used inflation on the airfoil with 40 layers, expansion factor 1.02, first layer thickness option with y+ = 1, Re = 10^4, and 1 m reference length.
My meshing strategy in the options category was a 1 layer extruded 2D mesh. The extruded periodic pair was between the left and right sides (along the z-axis).

Setup (Pre)

The inlet velocity is 0.65 m/s, so the Reynolds number is Re = 10^4
The Mach number is M = 1.91 x 10^-3

As per Tutorial 4 (? - whichever has flow through a circular vent with smoke), I created 2 analyses - a steady state and a transient. Really, the only difference is that the airfoil in the transient analysis is rotating (while the steady state airfoil remains stationary).

The transient analysis type has no coupling, a 60 s total time, 48*1.25 timesteps, and initial time of 0 s.

The domains are the airfoil and the fluid.
The airfoil domain is solid (changed it for you, Glen), steel, and rotating about the z-axis at -0.001 rad/s with no mesh deformation. The only boundary is the default domain (the airfoil).
The fluid domain has the following boundaries: symmetry on the top, bottom, left, and right; inlet with u = 0.65 m/s and medium intensity turbulence; outlet with 0 Pa average static pressure; smooth, no-slip wall on the airfoil. k-omega turbulence is used.

In the Solver Control, a second order backward Euler scheme is used with min. coeffs 1 and max. coeffs 2 and RMS 1E-4 residuals for the convergence criteria.

In the Output Control, pressure and velocity are output every 1 s.

Solver

Both the steady state and transient analyses complete and converge successfully.

Post

The stationary airfoil remains. When I click on various timesteps, I see both the stationary (0 degree AoA) and transient airfoil. The stationary one interferes with the transient one (i.e. the streamlines and pressure contours go around both).

[Josh]

Originally Posted by ghorrocks

Then the easiest way of implementing the airfoil motion sounds like putting it is a rotating frame of reference and join it to the outer stationary frame of reference with a GGI on transient rotor/stator mode.

I have searched up and down through the Help file and online for a way to do this for objects that aren't actually rotor/stators. The tutorial was unhelpful as it was based on a pre-existing geometry.

Can someone please set me in the right direction? I'm struggling to figure this out.

Thanks again for your help.

[ckleanth]

this is what glenn meant for the rotating frame

[Josh]

Thanks for the drawing, George. I do understand the theory, just not the method. I'm not sure how to rotate the area around the airfoil.

[ckleanth]

you need to create two meshes, one is the outside (preferable hex) and one surrounding the wing profile (easiest is tetra with inflation but you could put some more effort and create a nice mesh to capture the flow).

in cfx you can define the mesh movement in many ways:
for steady state use one domain and rotate the inner mesh in cfx pre according to your requirements.
for transient you can do this in a few ways:
one is mentioned in the sloshing link I posted above
another way is to use two domains the outer mesh is the stationary frame and the inner mesh is the rotating frame ( this is what glenn was on about)
another uses subdomain to define the motion but distorts the mesh

[Josh]

I tried Glenn's method (2 Domains - the solid airfoil and the fluid surroundings). In Post, I only saw rotation if the airfoil domain was treated as an immersed solid. Even then, as the airfoil rotated (it was colored blue), another stationary airfoil was present. Hence there were 2 airfoils whose streamlines and pressure contours were intertwined.

I think the reason for this is that although I have a solid airfoil domain, the airfoil is also a boundary in the fluid domain, so the solver treats the simulation as if there are 2 airfoils.

How do I properly define the 2 domains to avoid this? Or is this caused by something else?

I would do the moving mesh method, but Glenn said it's complicated and causes long simulation times. Since my summer student contract expires soon, I don't know if I have time to learn and implement something that complicated.

Thanks for any help!

[ckleanth]

i think your problem is the way you created the mesh. as I said if you use imersed solids the mesh for the fluid and imersed solid component must be separate and independant (in simple terms if you used workbench to create the geomerty the wing and the fluid space are two independant parts.

all other cases require all bodies need be in the same part and share the same topology

[ghorrocks]

Originally Posted by Josh

The inlet velocity is 0.65 m/s, so the Reynolds number is Re = 10^4
The Mach number is M = 1.91 x 10^-3

.....
The fluid domain has the following boundaries: symmetry on the top, bottom, left, and right; inlet with u = 0.65 m/s and medium intensity turbulence; outlet with 0 Pa average static pressure; smooth, no-slip wall on the airfoil. k-omega turbulence is used.

In the Solver Control, a second order backward Euler scheme is used with min. coeffs 1 and max. coeffs 2 and RMS 1E-4 residuals for the convergence criteria.

1. This is a very low Re number for an airfoil. I doubt this airfoil will have any turbulence transition so forget about turbulence modelling, switch to laminar flow.
2. Your Ma number is very small, meaning compressible effects are insignificant. I trust you are doing an incompressible analysis because of this.
3. Your solver control is unlikely to be optimum. Get rid of the min coeff loops requirement and put the maximum to maybe 10.
4. Your convergence tolerance is lax. You might need to tighten it up.
5. Your grid is unsuitable for a laminar flow simulation. You do not need as much boundary layer refinement for a laminar flow case.
6. Your grid along the chord of the airfoil is too coarse. You can see the angle between adjacent elements. You will never get accurate results like this, you need more elements along the length of the chord.
7. All of these parameters (chord mesh, boundary layer mesh, convergence, timestep size) needs to have sensitivity analysis done on it to establish your degree of accuracy.

Glenn Horrocks

[Josh]

Originally Posted by ckleanth

i think your problem is the way you created the mesh. as I said if you use imersed solids the mesh for the fluid and imersed solid component must be separate and independant (in simple terms if you used workbench to create the geomerty the wing and the fluid space are two independant parts.

all other cases require all bodies need be in the same part and share the same topology

What if I don't use an immersed solid? Like Glenn said, that's a poor way to model airfoils, so I decided against it. If I don't use an immersed solid, should I still have 2 domains (solid airfoil and fluid surroundings), or should I just have 1 domain (airfoil cutout in fluid domain)? If it's the latter case (as you suggest in your 2nd paragraph), how do I create 2 different meshes for just 1 domain?

Thanks again! I really appreciate your help.

[Josh]

Originally Posted by ghorrocks

This is a very low Re number for an airfoil. I doubt this airfoil will have any turbulence transition so forget about turbulence modelling, switch to laminar flow.

This is very low because I am modeling a low Reynolds UAV. Despite the likelihood of laminar flow, the professor and client requested k-omega turbulence modeling. They are interested in Reynolds numbers of 10^4 and 5x10^4 at angles of 0, 5, 10, and 15 degrees.

Originally Posted by ghorrocks

Your Ma number is very small, meaning compressible effects are insignificant. I trust you are doing an incompressible analysis because of this.

It was unspecified in the problem description.

Originally Posted by ghorrocks

Your solver control is unlikely to be optimum. Get rid of the min coeff loops requirement and put the maximum to maybe 10.

This was a typo. It should be 10. Not sure why I wrote "2". Long day, I suppose.

Originally Posted by ghorrocks

Your convergence tolerance is lax. You might need to tighten it up.
Your grid is unsuitable for a laminar flow simulation. You do not need as much boundary layer refinement for a laminar flow case.

Very true. I am uninterested, at the moment, in quantitatively accurate results. I just want to figure out how to make my airfoil rotate from approximately 0 degrees to approximately 15 degrees. Once I solve that problem, I will refine everything.

Originally Posted by ghorrocks

Your grid along the chord of the airfoil is too coarse. You can see the angle between adjacent elements. You will never get accurate results like this, you need more elements along the length of the chord.
All of these parameters (chord mesh, boundary layer mesh, convergence, timestep size) needs to have sensitivity analysis done on it to establish your degree of accuracy.

I changed my airfoil to simply be a cutout from the fluid domain so that the geometry is now 1 Part, 1 Solid. Thus, the elements along the chord should no longer matter.

My main problem still persists. I cannot model an airfoil with changing angle with a transient analysis. I tried:

1) Using 1 Domain, which was then rotated at a certain angular velocity. This, however, did not produce results that displayed a changing angle. In other words, I could not animate the airfoil changing in angle.

2) Using 2 Domains, 1 stationary (fluid surroundings) and 1 rotating (solid airfoil). This, just as before, did not produce results that displayed a changing angle.

3) Using 2 Domains, 1 stationary (fluid surroundings) and 1 rotating (immersed solid airfoil). Although this did display an airfoil with changing angle, the original solid airfoil at 0 degrees remained, as well, causing interference (in other words, there were 2 airfoils - 1 rotating, 1 stationary at 0 degrees).

If I model the geometry as 1 Part, 1 Solid (like you suggested with merged topology and with the airfoil acting as a cutout from the fluid domain), how can I make the airfoil, and not the whole fluid domain, rotate?

I really appreciate your help. I've tried reading the manual for 2 weeks now and have done all the available tutorials, but to no avail.

[ckleanth]

Originally Posted by Josh

What if I don't use an immersed solid? Like Glenn said, that's a poor way to model airfoils, so I decided against it. If I don't use an immersed solid, should I still have 2 domains (solid airfoil and fluid surroundings), or should I just have 1 domain (airfoil cutout in fluid domain)? If it's the latter case (as you suggest in your 2nd paragraph), how do I create 2 different meshes for just 1 domain?

Thanks again! I really appreciate your help.

I never said you need to use the immersed solid, I'm just telling you whats wrong with your problem definition and your mesh when you used the immersed solids option

to use the stationery/rotating frame reference you obviously need to use two fluid domains.

purely for informational purposes if while creating your mesh you have a shared topology (thats the default option in workbench) which basically means you use the same nodes at the mesh interface, you can use more than one mesh in a domain.

[Josh]

Originally Posted by ckleanth

I never said you need to use the immersed solid, I'm just telling you whats wrong with your problem definition and your mesh when you used the immersed solids option

to use the stationery/rotating frame reference you obviously need to use two domains.

I want to do the stationary/rotating frame style. When using 2 domains, though, my airfoil appears as both a domain AND as a boundary within the fluid domain. Any ideas on how to prevent this?

[ghorrocks]

Originally Posted by Josh

This is very low because I am modeling a low Reynolds UAV. Despite the likelihood of laminar flow, the professor and client requested k-omega turbulence modeling. They are interested in Reynolds numbers of 10^4 and 5x10^4 at angles of 0, 5, 10, and 15 degrees.

Why run a turbulence model when the flow is not turbulent? Do you like deliberately introducing an error into the simulation? Unless you have an airfoil which has a turbulence transition at Re=5e4 (which seems very unlikely) then you will get more accurate results and a simpler simulation by using a laminar flow model.

If you insist on using a turbulence model then the only model which makes sense is SST with the turbulence transition model - and I bet it never trips to turbulence anyway!

Originally Posted by Josh

Very true. I am uninterested, at the moment, in quantitatively accurate results. I just want to figure out how to make my airfoil rotate from approximately 0 degrees to approximately 15 degrees. Once I solve that problem, I will refine everything.

Well then why use a boundary layer mesh at all? Make a coarse grid with no inflation layers at all just to test the motion of the grid.

As for your difficulties in getting the thing to move, have a look at any of the rotor/stator tutorials in the CFX examples. All we are suggesting here is to make the rotational speed a CEL expression rather than a constant and make it sweep out the motion you intend.

Glenn Horrocks

[Josh]

Originally Posted by ghorrocks

Why run a turbulence model when the flow is not turbulent?

I asked my professor about this on Friday. Just as with a flat plate, the turbulence model is required near the trailing edge of the airfoil where length begins to play a significant role in turbulence development.

Originally Posted by ghorrocks

Make a coarse grid with no inflation layers at all just to test the motion of the grid.

Fair enough. I'll give it a shot.

Originally Posted by ghorrocks

As for your difficulties in getting the thing to move, have a look at any of the rotor/stator tutorials in the CFX examples.

The tutorials, as I recall, were not very helpful because they used pre-existing files that my professor chose not to install on this computer. Still, I'll take another look at them and get back to you.

Thanks for all the help.

Joshua

[ghorrocks]

Originally Posted by Josh

I asked my professor about this on Friday. Just as with a flat plate, the turbulence model is required near the trailing edge of the airfoil where length begins to play a significant role in turbulence development.

Unless your airfoil has a turbulence transition (maybe the design has turbulence trips? Or a airfoil design feature to trip turbulence?) then the airfoil is laminar and if you use a turbulence model you are just reducing the accuracy of your simulation. Don't take your prof's word as gospel - I think he's wrong. But do the background work and show whether he is right or wrong. If you can show the flow is laminar it will simplify the simulation substantially as there is no need for turbulence models.

Originally Posted by Josh

The tutorials, as I recall, were not very helpful because they used pre-existing files that my professor chose not to install on this computer. Still, I'll take another look at them and get back to you.

Your prof seems to have a track record of making bad decisions

Glenn

[Josh]

Originally Posted by ghorrocks

Your prof seems to have a track record of making bad decisions

Ouch. Careful - he reads these boards, too!