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.