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

Bad convergence perfermance of boiling heat transfer in chiller(plate HEx)

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 20, 2020, 05:21
Default Bad convergence perfermance of boiling heat transfer in chiller(plate HEx)
  #1
New Member
 
SHAN He
Join Date: Apr 2020
Posts: 17
Rep Power: 3
shanheplus is on a distinguished road
I'm try to simulate the heat transfer in the chiller, same as a layer of the plate heat exchaner. The refregerant is heated and boiled in the channel.

However, it is bad perfermance in convergence, especallly about the Equation of Continuilty.

My mesh is having good quailty because I test it in some simple conditions, it is easy to be convergence. And other option lists here.

Maybe you can give me some advice or experience to control the residual.

Thanks a lot.

---------------------
The FLUENT configuration is shown as following:


Model: RNG k-epsilon; Mixture two-phase with Lee model; Gravity; Steady;
Define the energy sources as UDF ---mass transfer · latent heat---

B.C.:
Inlet: R134a liquid under the saturation state in 0.3MPa. --- Mass flow inlet with 0.21 kg/s (totol liquid).
Outlet: 0.28MPa. -- Pressure out.
Wall: Heat flux = 12000 W/m2.
Other is no heat transfer.
-------------------
shanheplus is offline   Reply With Quote

Old   April 20, 2020, 05:24
Default
  #2
New Member
 
SHAN He
Join Date: Apr 2020
Posts: 17
Rep Power: 3
shanheplus is on a distinguished road
This is the control under-relaxation factors and Corrount Number=5. Energy=1. Density=0.1. (pressure and momentum=0.1) Body force = 0.5 Others less than the defaults 0.2;

And, it's also residul line.
Attached Images
File Type: png Snipaste_2020-04-20_17-22-07.png (71.1 KB, 7 views)
File Type: png Snipaste_2020-04-20_14-13-58.png (9.6 KB, 6 views)
shanheplus is offline   Reply With Quote

Old   April 20, 2020, 05:41
Default Courant
  #3
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 33
vinerm will become famous soon enough
Do not use a courant number of 5. Default is 200, user should not bring is below 10. If you are bringing it below 10, prefer using SIMPLE. Prefer pseudo-transient over Courant number based solver.

But most likely it is not the numerical setup rather the physical setup that could be wrong. What are your operating conditions, i.e., Operating Pressure and Operating Density values in the Operating Conditions panel in Fluent? Operating Density must be set equal to the density of R134a vapor. If you are modeling vapor as ideal gas, then both, operating pressure and operating density should be set to 0.

Secondly, if you are using Lee Model, why do you have an energy source UDF. What is the objective of this user defined source?
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 20, 2020, 06:05
Default
  #4
New Member
 
SHAN He
Join Date: Apr 2020
Posts: 17
Rep Power: 3
shanheplus is on a distinguished road
Oh, I don't notice the operating option, such as the density, pressure and temperature. I use many points to define the material-R134a, not idea-gas.

And, my operating pressure is 0.3 MPa ,which is equal to the saturation pressure. And the operating temperature is 273.8221 ,w which is T_sat. However, operating density even don't active in the latest cases. But I think I active it before, it's not convergence too. I will check then. How about the pressure and temperature setting?

Beside the operating option, I use the Lee Model. I think it is just mass-transfer model, there are no heat transfer amount. So I define the latent heat multiply by the mass to know how much heat transfer. (I read the theory guide about fluent, I just get the mass transfer equation.) So, it's no use or repeating?

Let me back to the Courant Number. I use many Co to test, such as 0.5/1/5/10/200. All are not so good, but the higher Courant Number is better, fitting your advice.

I'm confused.

Regard,
Thanks.
shanheplus is offline   Reply With Quote

Old   April 20, 2020, 06:50
Default Operating Conditions
  #5
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 33
vinerm will become famous soon enough
Operating pressure has got nothing to do with saturation pressure. There is nothing called an operating temperature. There is Boussinesq temperature but that is irrelevant if you are not using Boussinesq approximation to define density. Operating density appears whenever you have gravity enabled. For a multiphase case, gravity should always be enabled and operating density must be equal to density of the lighter phase, which is vapor for you.

As far as inbuilt models, such as, Lee or Thermal Phase Change Model are concerned, those are complete, i.e., all the important phenomena are included, including heat transfer. So, you do not require to include any source terms.

Once your physical setup is correct, you won't even face a numerical issue. Running with a Courant number of 200 or 20 won't make much difference once you set it up correctly.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 20, 2020, 07:09
Default
  #6
New Member
 
SHAN He
Join Date: Apr 2020
Posts: 17
Rep Power: 3
shanheplus is on a distinguished road
Thanks a lot, it's useful.
1 Temperatue: Yes, that is Boussinesq temp. And I'm not using Boussinesq approximation to define density. So this temp. Could be any number?
2 Pressure: I define the operating pressure is 0, because the temperatue I used is absolute pressure. That's right? (FIG.1)
3 Density: I know why I don't set the density. I check the formor setting which used the ANSYS 19. There are the set up button. However, I use the ANSYS 2020R1. There are no such option. Just choose the minium-phase-averaged / mixture-averaged / primary-phase-averaged... (FIG.2) That is a the new features.

Regards,
SHAN
Attached Images
File Type: png Snipaste_2020-04-20_18-59-18.png (30.5 KB, 3 views)
File Type: png Snipaste_2020-04-20_19-07-37.png (3.7 KB, 2 views)
shanheplus is offline   Reply With Quote

Old   April 20, 2020, 07:16
Default Setup
  #7
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 33
vinerm will become famous soon enough
1. Yes, you can leave Boussinesq temperature as it is.

2. If you are not using Ideal Gas, then prefer using a positive operating pressure value instead of 0.

3. These options have always been there, just not directly available to the user. You can select User Input and enter the density of vapor phase as value.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 20, 2020, 08:08
Default
  #8
New Member
 
SHAN He
Join Date: Apr 2020
Posts: 17
Rep Power: 3
shanheplus is on a distinguished road
Another queation. You said ". Since you are running a steady-state simulation, do not enable mass transfer in the beginning. Run without it and see if the flow and thermal energy conservation as well as numerical convergence is achieved. Once that is done, then enable mass transfer." in another thread.

That means firstly I don't active Lee model, when it have a good results such as convergence, I active Lee model then, and continue to calculate on the previous data? right?

Thanks a lot!
shanheplus is offline   Reply With Quote

Old   April 20, 2020, 10:07
Default Procedure
  #9
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 33
vinerm will become famous soon enough
Yes, you can use this procedure. However, you have to patch with a very small volume fraction of vapor to initialize evaporation. If there is no vapor, evaporation won't take place.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   April 23, 2020, 02:01
Default
  #10
New Member
 
SHAN He
Join Date: Apr 2020
Posts: 17
Rep Power: 3
shanheplus is on a distinguished road
I test the configuration that you suggested, for example, add the operating density and modify the operating pressure and temperature. Besides, I delete the UDF and just use Lee Model. And, I try to use the Coupled and SIMPLE. However, its results results look the same: bad density residual (0.2±0.1), high oscillation. I can not find why it is. Could you please give me some advice futher?

Then, the liquid and vapor R134a material properties are from NIST and both of them are properties with varing saturation temperature and pressure. That's right or not? I want to simulate the two-phase fuild flow with pressure 0.3MPa±0.1MPa.

Thanks!

Sincerely,
SHAN
Attached Images
File Type: png Snipaste_2020-04-23_14-00-14.png (40.9 KB, 7 views)
shanheplus is offline   Reply With Quote

Old   April 23, 2020, 14:37
Default Material Properties
  #11
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 33
vinerm will become famous soon enough
Do you want to include material properties as functions of both pressure and temperature. That can only be done via UDF. If you only want to use temperature dependent properties, then you can directly do that from GUI. As far as saturation temperature is concerned, that can be a function of saturation pressure. I will have to check whether that can be directly given as a function of pressure or whether you need UDF for that. I'd suggest you to start simple and keep everything constant.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm 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
This mesh contains patches of type empty but is not 1D or 2D oric OpenFOAM Running, Solving & CFD 36 November 28, 2016 07:12
Boiling heat transfer between the tube bundle camiliar CFX 5 September 10, 2013 00:25
Question about heat transfer coefficient setting for CFX Anna Tian CFX 1 June 16, 2013 06:28
increasing mesh quality is leading to poor convergence tippo CFX 2 May 5, 2009 10:55
CheckMeshbs errors ivanyao OpenFOAM Running, Solving & CFD 2 March 11, 2009 02:34


All times are GMT -4. The time now is 18:51.