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

general momentum source with constant velocity in the outlet

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

Like Tree2Likes
  • 1 Post By ghorrocks
  • 1 Post By Opaque

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 20, 2021, 13:35
Default general momentum source with constant velocity in the outlet
  #1
New Member
 
AS
Join Date: Jul 2021
Posts: 4
Rep Power: 2
ASBR is on a distinguished road
Hi,

I am modeling a recirculatory flow (ANSYS-CFX), just to simplify is like a flow in a pipe with "O" shape geometry. I defined a subdomain in this geometry, and I also inserted a general momentum source in this subdomain. My question, if someone can help me, is there some way to set the general momentum source to keep a constant velocity in the outlet of the subdomain?
OBS: I can not use in-let and out-let because it is a recirculatory flow, so, new material can not enter inside the domain, also, no material can flow out the domain.




Thanks very much for any help.
Attached Images
File Type: png Momentum source schemy.png (164.7 KB, 8 views)
ASBR is offline   Reply With Quote

Old   July 20, 2021, 19:30
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,820
Rep Power: 132
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Why can't you use an inlet/outlet pair? The flow rate in will equal the flow rate out, so there is no net flow in or out of the domain. If you want to specify the velocity profile at a plane this is the obvious way to do it. The only reason I can thin why you would not want to do this is because it is accumulating heat or some other scalar which you want to track over time.

But to answer your question: You can define the region (or just the exit plane if you like) to be a momentum source, and set the source term to give a specified velocity over the whole plane.
ASBR likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   July 21, 2021, 10:37
Default
  #3
New Member
 
AS
Join Date: Jul 2021
Posts: 4
Rep Power: 2
ASBR is on a distinguished road
Thanks ghorrocks,

In fact i have an accumulating scalar in my simulation.
From Ansys guides and foruns dicussions, I toke the follow information:
The momentum source is implemented as force/unit volume, so the value that I used in the set up was:

(Flow rate -m3/s)*(fluid density - kg/m3)*(flow velocity - m/s)/V(m3).

But, from this consideration I obtained a very low velocity, in comparison with the value that I used to calculate the momentum source. Therefore, the velocity profile was different from the desired one. Do you have any sugestion to this?

Thanks,
ASBR is offline   Reply With Quote

Old   July 21, 2021, 14:35
Default
  #4
Senior Member
 
Join Date: Jun 2009
Posts: 1,441
Rep Power: 27
Opaque will become famous soon enough
What value did you use for the Source Coefficient?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   July 21, 2021, 14:50
Default
  #5
New Member
 
AS
Join Date: Jul 2021
Posts: 4
Rep Power: 2
ASBR is on a distinguished road
I used 10^5 for the source coefficient. Also, I performed some simulations with low values (~10-10^2), but it is still difficult to correlate momentum source value with velocity.
ASBR is offline   Reply With Quote

Old   July 21, 2021, 14:59
Default
  #6
Senior Member
 
Join Date: Jun 2009
Posts: 1,441
Rep Power: 27
Opaque will become famous soon enough
10^5 may be a bit small.

The final equation you want is

Large Coefficient * Solved Variable + (Neighbor Contributions * Solved Neighbors)= Large Coefficient * Intended Variable

If you solve for Solved Variable, and the Neighbor Contributions/Large Coefficient is small, you get want you want.
ASBR likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   July 23, 2021, 09:08
Default
  #7
New Member
 
AS
Join Date: Jul 2021
Posts: 4
Rep Power: 2
ASBR is on a distinguished road
Thanks Opaque. now it is seems working better.
ASBR is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Import .csv - velocity profile - error eSKa CFX 9 April 3, 2021 13:38
polynomial BC srv537 OpenFOAM Pre-Processing 4 December 3, 2016 09:07
[swak4Foam] Error bulding swak4Foam sfigato OpenFOAM Community Contributions 18 August 22, 2013 12:41
[swak4Foam] funkySetFields compilation error tayo OpenFOAM Community Contributions 39 December 3, 2012 05:18
"parabolicVelocity" in OpenFoam 2.1.0 ? sawyer86 OpenFOAM Running, Solving & CFD 21 February 7, 2012 11:44


All times are GMT -4. The time now is 06:21.