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

H-energy imbalance and P-mass imbalance does not converge.

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

Like Tree2Likes
  • 2 Post By Gert-Jan

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 20, 2023, 09:25
Default H-energy imbalance and P-mass imbalance does not converge.
  #1
New Member
 
Anusai Ramankutty
Join Date: Dec 2019
Posts: 9
Rep Power: 6
anu4anusai is on a distinguished road
I have a CHT analysis being done, where I have small gaps upto 55 microns in the fluid domain. I also have rotating domain at 140000rpm.

I get high Mach number notice if I keep the physical timescale to be higher than 1e-5, and if I keep it as 1e-6, the imbalances in h-energy and p-mass in the fluid does not converge .

Can anyone suggest how I can fix this?
anu4anusai is offline   Reply With Quote

Old   February 20, 2023, 11:28
Default
  #2
Senior Member
 
Join Date: Jun 2009
Posts: 1,770
Rep Power: 31
Opaque will become famous soon enough
I assume you are solving the problem using double precision, correct?

Also, what are the dimensions range in your case? m vs microns, or mm vs microns?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   February 20, 2023, 13:00
Default
  #3
New Member
 
Anusai Ramankutty
Join Date: Dec 2019
Posts: 9
Rep Power: 6
anu4anusai is on a distinguished road
The total length of the domain is 160mm. The working fluid i am using is R1234yf
anu4anusai is offline   Reply With Quote

Old   February 20, 2023, 17:52
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,629
Rep Power: 142
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Have yo read the FAQ on this? https://www.cfd-online.com/Wiki/Ansy...gence_criteria
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 20, 2023, 23:01
Default
  #5
New Member
 
Anusai Ramankutty
Join Date: Dec 2019
Posts: 9
Rep Power: 6
anu4anusai is on a distinguished road
Quote:
Originally Posted by Opaque View Post
I assume you are solving the problem using double precision, correct?

Also, what are the dimensions range in your case? m vs microns, or mm vs microns?
Yes, am using double precision!
anu4anusai is offline   Reply With Quote

Old   February 21, 2023, 03:17
Default
  #6
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,814
Rep Power: 27
Gert-Jan will become famous soon enough
I would first run at lower speed and make sure global energy and mass balances are correct. Then speed up step by step.
Have you read this FAQ carefully: https://www.cfd-online.com/Wiki/Ansy...gence_criteria
Point 2 tells you that (boldly said) flow is pressure driven (= fast) and energy is momentum driven (=relatively slow). Given your small time steps, the development of temperature and related equations, develop much slower through your domain than the flow itself. Therefore I consider it convenient to switch off momentun and turbulence for a few iterations and only solve energy equation with a large timestep. You can do this by defining Expert Parameters. Set:

- solve fluids = false
- solve turbulence = false.

You can do this on the run (add expert parameter section in the top ribbon), you don't have to stop the calculation for this. When changing these parameter from true (default) to false, you can change the timescale to e.g. 1e-3, to let temperature develop in the existing (and now frozen) flow field fast.
When you see that the energy imbalance have dropped significantly, you can go back to previous settings, again on the fly. Don't forget to reduce timestep! Otherwise it will crash soon.
You can repeat this procedure a couple of times to get everything converged within reasonable time. However, your end solution should always be based on iterations where all equations are solved simultaneously, with the same timestep!
Opaque and zacko like this.

Last edited by Gert-Jan; February 25, 2023 at 10:24.
Gert-Jan is offline   Reply With Quote

Reply

Tags
cfx, cht, flow, physical timescale, turbulence

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
Activating gas radiation leads to energy imbalance seph FLUENT 1 August 2, 2022 13:33
Mass imbalance problem in multiphase water and steam CFX case Antech CFX 1 October 26, 2020 05:03
Turbomachinery Mass imbalance sheaker CFX 12 September 5, 2019 09:09
Energy imbalance seojaho CFX 6 June 21, 2016 21:35
ATTENTION! Reliability problems in CFX 5.7 Joseph CFX 14 April 20, 2010 16:45


All times are GMT -4. The time now is 10:42.