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

Using different turbulence model with connecting fluid domain

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

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 17, 2022, 05:11
Default Using different turbulence model with connecting fluid domain
  #1
Member
 
William
Join Date: Jun 2020
Posts: 70
Rep Power: 5
CFXer is on a distinguished road
Hello.

I'm simulating some fluid dynamics.

Domain 1 and 2 are connected by domain interface, same fluid passes through.

Domain 1 should be calculated as "turbulent" and Domain 2 should be estimated as "laminar".

But when I used domain interface of each "turbulent" and "laminar" interface, error occurred.
+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Equation subsystem: "Wall Scale - 1" has not been found on both s- |
| ides of interface "outheader_outlet_header". Check that you have |
| set consistent physics across all domains that use this interface- |
| . |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine DEF_ALGM_SUBSYS_ZIF |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+


I have to use Turbulent / Laminar interface.

How can I do this? someone please help me.
CFXer is offline   Reply With Quote

Old   October 17, 2022, 05:32
Default
  #2
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
I have seen turbulent and laminar settings together in 1 CFX-simulation, but only in an application where both were defined in 2 unique domains separated by a solid. You are connecting both domains directly using an interface. I don't think this is possible in CFX. If I would like to do this, I would go to Fluent, where this can be achieved by setting a volume as Laminar zone, even if it connected to a turbulent zone.

But alternatively, use the SST model which converges to a laminar solution if the conditions a laminar. At least, I have seen parabolic velocity profiles in a straight tube corresponding to laminar conditions. Not sure if this will be achived in your application....
Gert-Jan is offline   Reply With Quote

Old   October 17, 2022, 17:50
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Some suggestions:
* Use the SST turbulence mode as Gert-Jan suggests. If you use SST on a laminar flow in most cases it still gives you a result very close to the laminar result. SST handles zero turbulence nicely (unlike k-eps).
* Use the transitional turbulence model with specified intermittency. This allows you to explicitly set which areas are laminar and which are turbulent.
* Do the laminar and turbulent bits as separate simulations, replacing the interface with a boundary condition. This will only work if you can approximate the interface with a relatively simple boundary.
* You might be able to get this to work by setting the non-constant domain physics expert parameter, but I suspect it will not work as the boundary will cause undefined turbulence parameters.
Opaque 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   October 18, 2022, 08:46
Default
  #4
Senior Member
 
Join Date: Jun 2009
Posts: 1,804
Rep Power: 32
Opaque will become famous soon enough
Q: what are you trying to achieve by splitting the turbulence model spatially?

The turbulence model requires boundary conditions at inlets, outlets, walls, etc. When the model is split, it requires a boundary condition at the split interface.

Ignoring how to implement them in the model, how would you realize the value of those conditions?

Perhaps it is best to describe your modeling goals, and let others in the forum pitch in some suggestions.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   October 23, 2022, 20:05
Default
  #5
Member
 
William
Join Date: Jun 2020
Posts: 70
Rep Power: 5
CFXer is on a distinguished road
Quote:
Originally Posted by Opaque View Post
Q: what are you trying to achieve by splitting the turbulence model spatially?

The turbulence model requires boundary conditions at inlets, outlets, walls, etc. When the model is split, it requires a boundary condition at the split interface.

Ignoring how to implement them in the model, how would you realize the value of those conditions?

Perhaps it is best to describe your modeling goals, and let others in the forum pitch in some suggestions.

Thank you for all of yours reply.

My simulation is heat exchanger with plate structure.

I uploaded my domain structure to the image.

In plate parts, when I applied turbulence model, the heat transfer coefficient did not work.

So, I applied non-turbulence(laminar) model to the porous domain, It works very well.

So, I should apply fluid domain with turbulence model in header, porous domain with laminar model in plate.

Separate simulation could not be applied because the header and plates are related strongly.
Attached Images
File Type: png 12.png (9.6 KB, 8 views)
CFXer is offline   Reply With Quote

Old   October 23, 2022, 20:18
Default
  #6
Member
 
William
Join Date: Jun 2020
Posts: 70
Rep Power: 5
CFXer is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Some suggestions:
* Use the SST turbulence mode as Gert-Jan suggests. If you use SST on a laminar flow in most cases it still gives you a result very close to the laminar result. SST handles zero turbulence nicely (unlike k-eps).
* Use the transitional turbulence model with specified intermittency. This allows you to explicitly set which areas are laminar and which are turbulent.
* Do the laminar and turbulent bits as separate simulations, replacing the interface with a boundary condition. This will only work if you can approximate the interface with a relatively simple boundary.
* You might be able to get this to work by setting the non-constant domain physics expert parameter, but I suspect it will not work as the boundary will cause undefined turbulence parameters.
Thank you for your kind reply.

After I set the transitional turbulence model, how can I set it?

In case of fully turbulent, intermittency = 1.0 or just fully turbulent,
and laminar, intermitency = 0?

And could this method apply the heat transfer based on laminar condition?

Thank you in advance.
CFXer is offline   Reply With Quote

Old   October 24, 2022, 02:37
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Before we get into the transitional turbulence model, let's just follow up Opaque's comment as your answer puzzles me.

What did not work when you made the whole thing turbulent? Please attach the output file. This is the best way to get it working (if it is applicable), so we should try to get the fully turbulent approach working first.

Can you describe why you are using a porous domain for the plates? Please show an image of your model.
Opaque 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   October 24, 2022, 02:42
Default
  #8
Member
 
William
Join Date: Jun 2020
Posts: 70
Rep Power: 5
CFXer is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Before we get into the transitional turbulence model, let's just follow up Opaque's comment as your answer puzzles me.

What did not work when you made the whole thing turbulent? Please attach the output file. This is the best way to get it working (if it is applicable), so we should try to get the fully turbulent approach working first.

Can you describe why you are using a porous domain for the plates? Please show an image of your model.
Between the hot and cold plate, the heat transfer occurs.

I used porous domain to reduce the computing cost.

So, I used friction factor and Nusselt number correlation between hot and cold fluid.

When I did a simulation with fully turbulent model, the heat transfer coefficient goes to very high value, so input correlation doesn't work.

I think it is because of the turbulence model's heat transfer characteristics.

When I turn off the turbulence model with only porous plates model, the heat transfer coefficient work very well.
Attached Images
File Type: png 23.png (7.8 KB, 11 views)
CFXer is offline   Reply With Quote

Old   October 24, 2022, 03:01
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Then isn't your problem how to get the heat transfer accurate in a turbulent simulation?
__________________
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 24, 2022, 03:02
Default
  #10
Member
 
William
Join Date: Jun 2020
Posts: 70
Rep Power: 5
CFXer is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Then isn't your problem how to get the heat transfer accurate in a turbulent simulation?
Yes it is.

You are right
CFXer is offline   Reply With Quote

Old   October 24, 2022, 03:08
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,703
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
So then your question is how can you make the heat transfer more accurate.

Have a look at the FAQ on accuracy: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Key points are:
* What Reynolds Number and/or Rayleigh Number are the tubes running at?
* Have you done a mesh refinement study? You really need to do this if you want to be accurate.
* What turbulence model are you using? Why? And what turbulence boundary conditions have you applied?
__________________
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 24, 2022, 04:51
Default
  #12
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,827
Rep Power: 27
Gert-Jan will become famous soon enough
Do I understand corectly that you are using a porous region to separate hot and cold parts? As if it is a wall?
Gert-Jan 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
sliding mesh problem in CFX Saima CFX 46 September 11, 2021 07:38
[swak4Foam] swakExpression not writing to log alexfells OpenFOAM Community Contributions 3 March 16, 2020 18:19
Question about adaptive timestepping Guille1811 CFX 25 November 12, 2017 17:38
Waterwheel shaped turbine inside a pipe simulation problem mshahed91 CFX 3 January 10, 2015 11:19
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 04:05


All times are GMT -4. The time now is 05:04.