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

cell mass flux

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 12, 2019, 07:49
Default cell mass flux
  #1
Member
 
Anonymous
Join Date: Jan 2012
Location: Canada
Posts: 60
Rep Power: 9
Industrial_CFD is on a distinguished road
Hoping someone can shed light on something I have been trying to do with CEL.

I have a phase change simulation and I need to compute a term that is the ratio of the condensate leaving each CV to the condensation rate. This ratio is used to calculate a part of the total thermal resistance.

Any ideas? In FLUENT I could fairly easily sum the flux's on each cell face to compute the total condensate leaving the cell. In CFX I don't see a CEL function that is the equivalent.
Industrial_CFD is offline   Reply With Quote

Old   October 13, 2019, 10:24
Default
  #2
Member
 
Anonymous
Join Date: Jan 2012
Location: Canada
Posts: 60
Rep Power: 9
Industrial_CFD is on a distinguished road
I guess I am wondering if there is a clever way of doing this that doesn't rely on the cell mass flux, which doesn't seem accessible through CEL. If I have to use FORTRAN I may just write it all in FLUENT UDFs...

Any advice is very much appreciated!
Industrial_CFD is offline   Reply With Quote

Old   October 13, 2019, 18:11
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,808
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
You don't have access to those factors in CEL. You will need user fortran for that.

But in CEL often you don't need them as you would implement the function differently in CFX to take advantage of this. Can you explain the function you are trying to implement?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   October 13, 2019, 18:43
Default
  #4
Member
 
Anonymous
Join Date: Jan 2012
Location: Canada
Posts: 60
Rep Power: 9
Industrial_CFD is on a distinguished road
I am trying to include the effect of inundation on the resistance to condensation mass transfer. The method I would like to implement requires a ratio of (f/mdot) where f if the condensate leaving the CV and mdot is the CV condensation rate.

So I would ideally sum the mass flux's on the faces, but I am definitely hoping there could be a more clever way to do this
Industrial_CFD is offline   Reply With Quote

Old   October 14, 2019, 00:55
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,808
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
The real world does not have control volumes, control volumes are a numerical approximation of the analytical process. So what are the continuous analytical equations you are trying to implement?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   October 14, 2019, 06:49
Default
  #6
Member
 
Anonymous
Join Date: Jan 2012
Location: Canada
Posts: 60
Rep Power: 9
Industrial_CFD is on a distinguished road
In each cell I need the ratio of the condensate rate leaving the cell (kg/s) to the condensation rate in the cell (kg/s). It is a measure of accumulation that is used to correct the thermal resistance based on a Nu for filmwise condensation over a single tube, for tubes further down the bundle that are seeing condensate 'rain down' from the top of the condenser tube bundle
Industrial_CFD is offline   Reply With Quote

Old   October 14, 2019, 17:20
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,808
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
As I said in my first post, the only way of doing this as you intend is by user fortran.

But I don't think either the model you are trying to implement is physically invalid, or the way you are trying to implement it is not appropriate for CFX. Quantities like accumulation of condensate and transport of condensate down the tube bundle is normally handled by a multicomponent mixture model (or maybe multiphase model).
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   October 16, 2019, 17:01
Default
  #8
Member
 
Anonymous
Join Date: Jan 2012
Location: Canada
Posts: 60
Rep Power: 9
Industrial_CFD is on a distinguished road
So I have installed fortran and run the simple HVAC tutorial. I am very inexperienced with user fortran. I see that cell mass flux is in the variables file but not available for CEL. Is it possible to use user fortran to create an additional variable for each cell mass flux (x,y,z) component and then use it in my CEL expressions?
Industrial_CFD is offline   Reply With Quote

Old   October 16, 2019, 17:33
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,808
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I am not an expert on user fortran and so cannot help you. CFX user fortran is complex. There are several tutorials on it in the documentation and on the ANSYS customer webpage.

But, again, I say that you are probably not taking the right approach here and in CFX it would be implemented differently. I cannot say anything until you tell us the physical model you intend to implement.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   October 16, 2019, 17:54
Default
  #10
Member
 
Anonymous
Join Date: Jan 2012
Location: Canada
Posts: 60
Rep Power: 9
Industrial_CFD is on a distinguished road
Hi Glenn,

First - thanks for your time and interest.

The overall model is a two-phase Euler Euler (steam condensation). Condensate is dispersed (assume d = 1 mm). No interphase heat transfer (saturated conditions), with a user specified interphase mass transfer.

The simulation is modeling condensation over a tube bundle.

thermal resistances include the tube wall, cooling water, condensate inundation/vapor shear.

Rinundation = R*(a/mdot)^n where n varies with distance from the bottom to the top of the bundle.

a = total condensate leaving cell
mdot = condensation rate in the cell

I was planning on accessing the cell mass flux vector to compute the net mass flux leaving the cell to get "a". I have everything else I need with CEL.

For now I assume a uniform inindation thermal resistance just to get the model running
Industrial_CFD is offline   Reply With Quote

Old   October 16, 2019, 18:16
Default
  #11
Member
 
Anonymous
Join Date: Jan 2012
Location: Canada
Posts: 60
Rep Power: 9
Industrial_CFD is on a distinguished road
Forgot to add: tube bundle is modeled as a porous region with anisotropic losses. Not a tube level resolution. Only the effect of the tubes
Industrial_CFD is offline   Reply With Quote

Old   October 16, 2019, 22:29
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,808
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I assume:
* It is calculation of the Rindundation factor which is the subject of this question.
* It gives a thermal resistance from a film of fluid on the wall for a wall heat transfer model
* It will be added to other thermal resistances to give a total thermal resistance for a wall heat transfer model.

If these assumptions are wrong please let me know.

My comments:
The function R*(a/mdot)^n looks strange as it has no accumulation term. Shouldn't it include an accumulation term?

Answering your question regardless:
The condensate rate term can come from your user defined mass transfer.

The "a" term (condensate leaving the cell) - I assume this is by advection only. Can this be taken as condensate volume fraction * Velocity Magnitude?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   October 17, 2019, 08:40
Default
  #13
Member
 
Anonymous
Join Date: Jan 2012
Location: Canada
Posts: 60
Rep Power: 9
Industrial_CFD is on a distinguished road
It is a mass flow leaving the cell, so unfortunately it has to be in kg/s. My understanding is that in order to know this I would need the net mass flow in/out of each face. In a way this is an accumulation term, because it is comparing how much is leaving the cell vs. how much condensate is being created in the cell.
Industrial_CFD is offline   Reply With Quote

Old   October 17, 2019, 17:51
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,808
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
For the "a" term try volume fraction * velocity * area. I am not sure the solver will be happy with area as a volumetric variable but worth a try. Then "a" will be in kg/s.

Your second sentence is not what I mean. Yes, the difference between the in flow and out flow then gives you the accumulation, but only the accumulation for that time step. It has information about how much was accumulated in previous time steps. This needs to be integrated over time so the material can accumulate over multiple time steps. This is what I mean by not having any accumulation terms.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   October 18, 2019, 12:05
Default
  #15
Member
 
Anonymous
Join Date: Jan 2012
Location: Canada
Posts: 60
Rep Power: 9
Industrial_CFD is on a distinguished road
area needs a locator, so I think I am stuck trying user fortran.
Thanks again for your help/advice.
Industrial_CFD is offline   Reply With Quote

Old   October 18, 2019, 19:30
Default
  #16
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,808
Rep Power: 122
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Use the domain as the locator. Also, note I am not talking about the CEL expression area, I am talking about the variable area. It gives the area of the control volume, but I do not know exactly what area it returns when applied to a volume.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks 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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
My radial inflow turbine Abo Anas CFX 27 May 11, 2018 01:44
Multiphase flow - incorrect velocity on inlet Mike_Tom CFX 6 September 29, 2016 01:27
Basic Nozzle-Expander Design karmavatar CFX 20 March 20, 2016 08:44
Radiation interface hinca CFX 15 January 26, 2014 17:11
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 04:05


All times are GMT -4. The time now is 08:12.