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

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

 February 20, 2023, 09:25 H-energy imbalance and P-mass imbalance does not converge. #1 New Member   Anusai Ramankutty Join Date: Dec 2019 Posts: 9 Rep Power: 6 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?

 February 20, 2023, 11:28 #2 Senior Member   Join Date: Jun 2009 Posts: 1,770 Rep Power: 31 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.

 February 20, 2023, 13:00 #3 New Member   Anusai Ramankutty Join Date: Dec 2019 Posts: 9 Rep Power: 6 The total length of the domain is 160mm. The working fluid i am using is R1234yf

 February 20, 2023, 17:52 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,629 Rep Power: 142 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.

February 20, 2023, 23:01
#5
New Member

Anusai Ramankutty
Join Date: Dec 2019
Posts: 9
Rep Power: 6
Quote:
 Originally Posted by Opaque 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!

 February 21, 2023, 03:17 #6 Senior Member   Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,814 Rep Power: 27 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.

 Tags cfx, cht, flow, physical timescale, turbulence