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

Boundary condition with velocity profile

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 6, 2013, 03:41
Default Boundary condition with velocity profile
  #1
New Member
 
Gerrald Gelderblom
Join Date: Nov 2012
Posts: 24
Rep Power: 4
DoubleG is on a distinguished road
Hi all,

I have to model a rotor in a large tank. What my approach is, is that I first model the rotor in small rotating frame, and than I want to use the velocity obtained at a surface around the rotor as boundary condition for further analysis.
For this I make the assumption that the behavior in the tank does not influence the velocity field just around the rotor, which assumption is met 'good enough'.

How can I use the velocity field obtained from a certain simulation as bc in another one? And is it also possible to do this when the mesh doesn't correspond between the two analyses? And is it also possible to apply also turbulence intensity, pressure and whatever more together with a velocity field?

Thanks,
Gerrald
DoubleG is offline   Reply With Quote

Old   August 6, 2013, 05:32
Default
  #2
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,087
Rep Power: 15
RodriguezFatz will become famous soon enough
Hi Gerrald,
This is pretty easy in Fluent (as long as your simulation is steady state):
You need to export a "profile" in your first simulation and import it to the other one.
After simulting go to: file->write->profile
You can select the desired surface and values to export. Normally, I just export all values of my outlet.
In you second simulation go to file->read->profile.
Bear in mind that fluent interpolates the values from the absolute coordinates. Thus, if your outlet from simulation 1) lies at position y=1m and your inlet from simulation 2) lies at position y=0m you need to tell that fluent. I think the form is self-explanatory. Just ask, if you have questions.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   August 6, 2013, 09:08
Default
  #3
New Member
 
Gerrald Gelderblom
Join Date: Nov 2012
Posts: 24
Rep Power: 4
DoubleG is on a distinguished road
Thank you for the answer.

The only problem is that I don't get any form when I read the profile. I need to rotate and translate my results, but I can't find how to do this. Can you explain a little bit more about this procedure?

Additionally: I read the profile to a mesh where the surface of the profile is not available. Does that matter? Or does it just force all quantities, even without the surface?

Thanks in advance,
Gerrald
DoubleG is offline   Reply With Quote

Old   August 6, 2013, 10:05
Default
  #4
Senior Member
 
RodriguezFatz's Avatar
 
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,087
Rep Power: 15
RodriguezFatz will become famous soon enough
You need to go to Boundary Conditions->Profiles->Orient...
Here you can use a translational ("Direction Vector") and rotational ("Rotation Matrix [RM]") transformation. I think I found help in the fluent manual. If I recall corectly, this is a bit cumbersome. You need to translate every single value you want to use.

"...Additionally...". I don't think I understand what you mean. You can only set these profiles value as boundary conditions to an existing surface, as far as I know.
__________________
The skeleton ran out of shampoo in the shower.
RodriguezFatz is offline   Reply With Quote

Old   August 9, 2013, 08:22
Default
  #5
New Member
 
Gerrald Gelderblom
Join Date: Nov 2012
Posts: 24
Rep Power: 4
DoubleG is on a distinguished road
Thank you Rodriguez, that was helpful! I managed to define the RM and TM correctly now.

Forget the second point. Now I used the velocity profiles as boundary condition at a surface.

My idea behind the question was to avoid the use of boundaries, because fluent uses a lower order scheme at boundaries. I thought it would maybe be possible to force velocities at a certain location in a fluid domain using profiles, even when at that specific location no surface is present. But this is not possible, since the profiles are interpolated based
I still try to do so, but now though defining a new fluid domain at the location of the rotor, and in that domain I want to apply a source of momentum.
DoubleG is offline   Reply With Quote

Reply

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
Low Mixing time Problem Mavier CFX 5 April 29, 2013 00:00
How to apply pulsatile velocity in boundary condition? Sama FLUENT 7 October 7, 2011 07:44
Velocity Gradiant Boundary Condition Aghakhani FLUENT 0 December 9, 2009 17:19
Profile Data Velocity Boundary Condition Changes?? Maria Angelica CFX 9 June 14, 2006 02:44
NON-UNIFORM VELOCITY INLET BOUNDARY PROFILE MURAT Main CFD Forum 0 December 30, 2003 22:08


All times are GMT -4. The time now is 22:10.