Transient Angle of Attack Simulation Not Displaying in Post
 

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.

Update
 

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?

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

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.

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).

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.

this is what glenn meant for the rotating frame

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.

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

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!

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

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

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.

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.

It was unspecified in the problem description.

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

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.

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.

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.

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?

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!


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

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.

Fair enough. I'll give it a shot.

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

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.

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

Glenn

Ouch. Careful - he reads these boards, too!

That's why I said it with a big grin on my face. I don't take myself too seriously and hope your prof doesn't take me too seriously either. But I would like to know why he wants to run a turbulence model on a simulation which is unlikely to have any turbulence in it.

Recently, I have been using this thread (http://www.cfd-online.com/Forums/cfx...interface.html) to model my problem.

Glenn - you mentioned in that thread to use 2 domains if there is no heat transfer, so I did. Here is my method:

Geometry

Import the NACA 0012 profile with Point.
Use a spline to connect the points on the upper half of the profile.
Extrude the half-profile.
Use a Body Operation to mirror the half-profile to create a full profile.
Freeze the full airfoil profile.
Create a sketch of the rectangular domain.
Extrude the sketch of the rectangular domain.
Use the Body Operation "cut material" to cut the airfoil profile out of the rectangular domain.
Create a sketch of a circle around the airfoil.
Extrude the circle with the "add frozen" operation option.
Define both of the "2 Parts, 2 Bodies" as "Fluid" domains.

http://picasaweb.google.com/lh/photo...eat=directlink

http://picasaweb.google.com/lh/photo...eat=directlink

Mesh

I left all the meshing parameters at default value except for the Options, for which I have chosen a 1-element thick 2D extruded mesh along the z-axis.

I also created 5 Regions - inlet (at the lowest x-coord), outlet (highest x-coord), left right (at the +/-z surfaces), top bot (at the +/-y surfaces), and airfoil domain
(the remaining 5 2D regions).

http://picasaweb.google.com/lh/photo...eat=directlink

http://picasaweb.google.com/lh/photo...eat=directlink

When I generate the volume mesh, I get a warning:

http://picasaweb.google.com/lh/photo...eat=directlink

Setup

Transient Analysis with 30 [s] Total Time, 30*1 [s] Timesteps, and 0 [s] Initial Time.

2 Domains:

Airfoil Domain:
http://picasaweb.google.com/lh/photo...eat=directlink
Fluid
Air @ 25 C
Rotating @ 0.25 [rev/min] about Z
No heat transfer or turbulence

Rectangular Domain:
http://picasaweb.google.com/lh/photo...eat=directlink
Fluid
Air @ 25 C
Stationary
No heat transfer or turbulence

Domain Interface:

In the airfoil domain, I can choose the inside of the cylinder as my region list:
http://picasaweb.google.com/lh/photo...eat=directlink

However, when I try to choose the outside of the cylinder as the other region list in the rectangular domain, the region is unavailable. Instead, I just choose the inside of the airfoil:
http://picasaweb.google.com/lh/photo...eat=directlink

Global Initialisation:

Stationary, Cartesian Velocity: u = 0.65, v = w = 0
0 Pa Relative Pressure

Any ideas? Why do I get that warning when I mesh? How can I create an interior/exterior cylinder interface?

Update:

I ran it rotor-stator style with no pitch change and GGI connectivity.

It's running, but ...

For some reason, the airfoil cutout is not moving with the moving domain. Here are some screenshots at 0, 5, and 10 [s]:

http://picasaweb.google.com/lh/photo...eat=directlink
http://picasaweb.google.com/lh/photo...eat=directlink
http://picasaweb.google.com/lh/photo...eat=directlink

Any ideas? How do I get the airfoil to rotate with the cylinder? Is there a way to remove the cylinder outline so that it does not appear in the animations, pictures, etc.?

Thanks!

Hi,

It's a bit hard to be sure but I suspect you have the following problems:

1) You have not cut the rotating domain containing the airfoil out of the rectangular domain. Domains cannot overlap, and joint at their edges with interfaces.
2) You appear to not have chopped the airfoil out of the rotating domain. Have you done an imprint faces or something like that? You need to cut it out of the rotating domain.
3) You have not set the thing up in 2D meshing mode properly. You need to set it up as a 2D extruded body.

Also if you do a super coarse grid you should be able to zip the WB project up and post it as an attachment to a post on the forum. Then we can really see what's going on.

Glenn

josh, without being 100% sure and re-iterating my post i think you are trying to use the mesh of the wing and you are treating it (the wing mesh) as being part of your simulation in which this is wrong.
all bodies (the stationary and rotating fluid space) need be in the same part in workbench (and share the same topology - but this is not important in this case as you will use ggi interface) however you dont need to use the wing inner mesh for this simulation. you only need the wing profile and that should be rotating together with the rotating fluid space.

in lame terms in workbench at the end of the day you need to have two bodies. one is the the stationary fluid space and one is the rotating fluid space. in this body the wing profile is a cut that goes all the way through your extrusion.
prior meshing you can join the two bodies and create a single part but this is not necessary as you will use ggi.

Correct. The cylindrical domain is an Extrusion with the "Add Frozen" Operation option. If I just do an Extrusion with the "Cut Material" option, the cylindrical domain does get cut out, but so does the airfoil! Here's a picture:

http://picasaweb.google.com/lh/photo...eat=directlink

The airfoil is a cutout from the original rectangular fluid domain. I created a solid airfoil first, then a rectangular domain around it (by freezing the airfoil), then used a Body Operation>Cut Material to cut the frozen airfoil out of the domain. I then created the cylindrical domain around the airfoil using the Body Operation>Add Frozen operation. Here is a zoomed-in picture of the airfoil cutout from the rectangular domain (the "Rectangular Fluid Domain" body is highlighted in the tree outline):

http://picasaweb.google.com/lh/photo...eat=directlink

Notice, however, that the airfoil does not appear to be a cutout when the "Airfoil Surrounding" body is highlighted:

http://picasaweb.google.com/lh/photo...eat=directlink

Is this the correct method, or have I screwed the pooch?

I think it's correctly setup:

http://picasaweb.google.com/lh/photo...eat=directlink

http://picasaweb.google.com/lh/photo...eat=directlink

I'd love to, but cannot find a way to upload a .zip file.

Thanks for all the help, guys.

I do not want to treat the wing mesh as part of my simulation. I am unsure of why this occurs, but I want to stop it.

What do you mean "in the same part in workbench"? Do you mean that, in Geometry, they should appear as "1 Part, 2 Bodies"? How do I accomplish this?

If you look at my pictures, I do have 2 bodies. Here is the rectangular fluid domain:

http://picasaweb.google.com/lh/photo...eat=directlink

And here is the airfoil surrounding area:

http://picasaweb.google.com/lh/photo...eat=directlink

I know something's wrong ... the rectangular domain should not encompass the cylindrical airfoil surroundings, and the airfoil should appear as a cutout in the airfoil surroundings. I'm just not sure how to do this properly (my above reply to Glenn describes my method of geometry creation).

your questions have a fundamental problem, not completed the tutorials

:cool:

I tried to complete all of them. There are certain files that, for whatever reason, were missing, so I was not able to complete all of them. I was, however, able to create each of the geometries and most of the meshes - the problems usually only arose in Setup or later.

My problem is I don't understand your questions/statements.

well you can do your the geomerry in many ways.
one of them is open workbench and to create a square extrusion with a hole in the middle.
freeze the part
create a plane on one side, then on the tree outline, click on the newly created plane and insert sketch projection - click on the part and you will have a sketch with the part profile. make a new sketch on the same plane and make a circle and your wing profile. extrude that sketch and freeze the part.
now you have two parts and this is all you need for your simulation.

to create one part with two bodies click on the two parts and then in the tools menu chose form new part.

create a 2d mesh and there job done

Thank you for your help and patience, George and Glenn.

I understand it's frustrating to help those who are simply looking for a quick answer without putting in any effort. I have worked on this simple problem for nearly a month now and I feel bad for my supervising professor. I have tried so many techniques - I did not even think of creating two cylinder sketches/protrusions and freezing them.

Thanks again.

Josh

P.S. - How do you open Geometry?

... just kiddin'.

Hey guys -

Thanks for everything. The simulation worked well.

I'm just curious ... how much will the rotating fluid-fluid domain affect the results on the airfoil? Is it relatively insignificant?

I don't understand your question.

I'm asking if the interface (between the rotating fluid domain around the airfoil and the stationary rectangular prism fluid domain) will affect certain parameters (e.g. the pressure distribution).

So, basically, if there wasn't an airfoil profile in the rotating domain and I had a pressure contour displayed in CFD-Post, would the pressure contour display be constant (i.e. not changing in colour) for the rotating domain?

Hi,

The implementation of the GGI interface in CFX is pretty good and should not affect things. The test you describe is a good and simple test for you to do to prove to yourself that it works - doing the test for yourself is the best way of being sure things are correct.

Glenn Horrocks

Thanks Glenn. I did some tests and it looks pretty damn accurate.

Thanks to everyone who helped.