general momentum source with constant velocity in the outlet

ASBR · July 20, 2021, 13:35

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.

ghorrocks · July 20, 2021, 19:30

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 · July 21, 2021, 10:37

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,

Opaque · July 21, 2021, 14:35

What value did you use for the Source Coefficient?

ASBR · July 21, 2021, 14:50

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.

Opaque · July 21, 2021, 14:59

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 · July 23, 2021, 09:08

Thanks Opaque. now it is seems working better.

July 20, 2021, 19:30		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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.

July 21, 2021, 14:35		#4
Opaque Senior Member Join Date: Jun 2009 Posts: 1,804 Rep Power: 32	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.

July 21, 2021, 14:59		#6
Opaque Senior Member Join Date: Jun 2009 Posts: 1,804 Rep Power: 32	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.

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

July 21, 2021, 10:37		#3
ASBR New Member AS Join Date: Jul 2021 Posts: 4 Rep Power: 4	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,

July 21, 2021, 14:50		#5
ASBR New Member AS Join Date: Jul 2021 Posts: 4 Rep Power: 4	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.

July 23, 2021, 09:08		#7
ASBR New Member AS Join Date: Jul 2021 Posts: 4 Rep Power: 4	Thanks Opaque. now it is seems working better.