CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Transient Angle of Attack Simulation Not Displaying in Post

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   July 28, 2009, 20:30
Default
  #21
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   July 29, 2009, 12:57
Default
  #22
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
Recently, I have been using this thread (2D rotating ellipse (domain interface??)) 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?

Last edited by Josh; July 29, 2009 at 14:13.
Josh is offline   Reply With Quote

Old   July 29, 2009, 13:32
Default
  #23
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
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!

Last edited by Josh; July 29, 2009 at 14:12.
Josh is offline   Reply With Quote

Old   July 29, 2009, 19:02
Default
  #24
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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
ghorrocks is offline   Reply With Quote

Old   July 29, 2009, 20:06
Default
  #25
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
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.
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   July 30, 2009, 10:03
Default
  #26
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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.
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

Quote:
Originally Posted by ghorrocks View Post
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.
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?

Quote:
Originally Posted by ghorrocks View Post
3) You have not set the thing up in 2D meshing mode properly. You need to set it up as a 2D extruded body.
I think it's correctly setup:

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

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

Quote:
Originally Posted by ghorrocks View Post
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.
I'd love to, but cannot find a way to upload a .zip file.

Thanks for all the help, guys.
Josh is offline   Reply With Quote

Old   July 30, 2009, 10:36
Default
  #27
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
Quote:
Originally Posted by ckleanth View 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.
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.

Quote:
Originally Posted by ckleanth View Post
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.
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?

Quote:
Originally Posted by ckleanth View Post
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.
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).
Josh is offline   Reply With Quote

Old   July 30, 2009, 12:18
Default
  #28
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
your questions have a fundamental problem, not completed the tutorials

__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   July 30, 2009, 12:26
Default
  #29
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
Quote:
Originally Posted by ckleanth View Post
your questions have a fundamental problem, not completed the tutorials

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.
Josh is offline   Reply With Quote

Old   July 30, 2009, 12:47
Default
  #30
Senior Member
 
ckleanth's Avatar
 
George
Join Date: Mar 2009
Location: Birmingham, UK
Posts: 257
Rep Power: 9
ckleanth is on a distinguished road
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
__________________
Top 4 tips
1. Knowledge is everything and Ignorance is dangerous.
2. Understand your limitations and try to eliminate them.
3. Get yerself a bike and hoon the chuffer. You will soon learn why dogs like to hang their heads out the car window.
4. Please before asking any questions on how to run simulations in CFX, go though all the tutorials
ckleanth is offline   Reply With Quote

Old   July 30, 2009, 15:28
Default
  #31
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
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'.
Josh is offline   Reply With Quote

Old   July 31, 2009, 10:43
Default
  #32
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
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?
Josh is offline   Reply With Quote

Old   August 2, 2009, 00:17
Default
  #33
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I don't understand your question.
ghorrocks is offline   Reply With Quote

Old   August 4, 2009, 09:20
Default
  #34
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
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?
Josh is offline   Reply With Quote

Old   August 4, 2009, 19:13
Default
  #35
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,646
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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
ghorrocks is offline   Reply With Quote

Old   August 5, 2009, 09:16
Default
  #36
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 8
Josh is on a distinguished road
Thanks Glenn. I did some tests and it looks pretty damn accurate.

Thanks to everyone who helped.
Josh is offline   Reply With Quote

Reply

Tags
airfoil, angle of attack, animation, rotating domain, transient

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Transient animation performance in CFX 5.5 POST Sjoerd Romkes CFX 8 February 5, 2013 15:53
introducing angle of attack on ICEMCFD HEXA icem beginner FLUENT 2 December 6, 2008 16:34
Initialisation in transient simulation with ASIs Phil D CD-adapco 7 January 30, 2008 08:44
modelling inviscid 2D flow at high angle of attack Ferdinando FLUENT 2 October 30, 2007 18:26
Automatic post processing of Transient simulation Aziz CFX 2 June 24, 2005 14:37


All times are GMT -4. The time now is 23:52.