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

VAWT transient cfd problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 25, 2011, 17:05
Question VAWT transient cfd problem
  #1
Member
 
Arslan
Join Date: Jan 2011
Posts: 35
Rep Power: 6
ArslanOZCAN is on a distinguished road
Hi guys.

I need to make transient cfd analysis of a vertical axis wind turbine in 2-D with sliding mesh method. I prepared a mesh and i think it is not the problem.

I prepared 2 different meshes. 1-Rectangular area with a hole in it. 2-Circular area containing airfoils. I opened these 2 meshes in FLUENT with append case file command. I will set rotational speed to the circular mesh. Now here are the questions;

-In mesh interfaces, should i use periodic or coupled?
-When i define mesh interfaces it sets 2 new wall boundary conditions.What are they and should they remain as wall?
-When i start solving it says turbulence viscosity is over than 1e05 in ... cells. And the number off cells increasing. What can be the problem.

Waiting for your commands...
ArslanOZCAN is offline   Reply With Quote

Old   January 26, 2011, 04:32
Default
  #2
New Member
 
Join Date: Mar 2010
Posts: 18
Rep Power: 7
red_lemon is on a distinguished road
-periodic I think but difficult to say without seeing grid
-walls need to become sliding interface so change to interface type and setup using define>mesh interface. Coupled wall will be thin non conformal wall
-check the grid is scaled correctly
red_lemon is offline   Reply With Quote

Old   January 26, 2011, 04:52
Default
  #3
Member
 
Arslan
Join Date: Jan 2011
Posts: 35
Rep Power: 6
ArslanOZCAN is on a distinguished road
I attached the picturese of my grid.
When i change these 2 walls to interface, it doesn't let me to add them in mesh interfaces. It says "CemberDis(name of the circle) is allready in another interface". When i just change them into interface and initiliaze the case it says "there are unassigned interface zones".

I checked and my grid is scaled correctly.

Waiting for your answer, and thank you...
Attached Images
File Type: jpg SlidingMesh.jpg (96.9 KB, 64 views)
File Type: jpg SlidingMeshZoom.jpg (91.0 KB, 52 views)
ArslanOZCAN is offline   Reply With Quote

Old   January 26, 2011, 07:25
Default
  #4
Senior Member
 
Phoevos
Join Date: Mar 2009
Posts: 103
Rep Power: 8
fivos is on a distinguished road
Set the interface (from define -> grid interfaces) defining the two interface sides from the two meshes. In your case there is no need to select coupled or periodic so leave them un - ticked.

After setting the interface two new boundaries will be created, which are, by default, walls, as you have noticed. They are created because of the way fluent treats interfaces :
- It finds the intersection of the two adjacent interface boundaries
- The intersection is transformed to something like an "interior" boundary, to let information pass through
- The rest is transformed in wall. You can change this if you want by changing the newly created boundary to whatever you like.

Since in your case interfaces completely overlap (and you should make sure the interfaces do so), they will be transformed to the "interior" boundary and no wall will be created. You can simply omit the new boundaries, just as I said before, make sure that interfaces "touch" each other. Also try previewing the mesh motion to see if everything is all right.
Try running a few timesteps. Check if fluid flows through the sliding mesh by checking velocity, pressure contours etc in the sliding mesh.

For the turbulence viscosity, maybe you have to try lower relax factors, or smaller time step. It might vanish later on as simulation proceeds. How many cells have this problem (as a percentage of the total cells)? Where are these cells (plot turbulent viscosity from contours and see where they are)? What turbulence model do you use (initial conditions?, boundary conditions ?)?

Another comment on your mesh : I have seen from the first picture that your mesh at the stationary domain gets bigger near the interface. Why you didn' t use the smaller resolution used in the rest domain ?

Last edited by fivos; January 26, 2011 at 07:53.
fivos is offline   Reply With Quote

Reply

Tags
cfd, fluent, sliding mesh, transient, vawt

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
Future CFD Research Jas Main CFD Forum 10 March 30, 2013 13:26
ill-posed CFD problem ? Noel Main CFD Forum 9 March 28, 2007 11:37
transient problem susan Main CFD Forum 3 December 5, 2002 13:06
Transient Problem Sundar Main CFD Forum 2 May 7, 2002 09:20
What is the Better Way to Do CFD? John C. Chien Main CFD Forum 54 April 23, 2001 08:10


All times are GMT -4. The time now is 11:26.