extreme temperatures on winding
 

Hello everyone.

I am simulating heat transfer in electric power generator and I had to use anisotropic copper to define its winding. But I obtained very strange result of temperature distribution. There are few little areas where the temperature is very low (-150°C) and very high (480°C).

Also the convergence of thermal energy is quite normal but after 200 iterations it becomes to diverge. Does anyone know what could be cause of this issue??

Thanks for any suggestions.

hi
 

Hi Keeper

I think because of diverging solution, you are getting such strange temperature values.
Try to improve the mesh quality and reduce the time step for better convergence .

unfortunately I am limited by the mesh size, my model contains 2.5M nodes and this is reasonable maximum which I can calculate with..but I will try to decrease timestep, thank you very much for suggestion...but anyway it is strange that those areas appear just after 200th iteration when solution starts to diverge

Convergence is one possibility but another common cause of this problem is the application of heat sources and sinks. If they are not correctly applied you get regions which get far too hot and cold.

How have you applied the heat to this simulation?

I defined domains and created subdomains on them where I set up heat sources. Below there is part of CCL.


SUBDOMAIN: WINDING HS
Coord Frame = Coord 0
Location = B5653
SOURCES:
EQUATION SOURCE: energy
Option = Source
Source = 98919 [W m^-3]
END
END
END


Those loses are calculated from electrical loses in winding and recalculated to 1 m^3.

Assuming the red and blue regions are your temperature extreme regions then it looks pretty certain something is wrong. Is there a GGI nearby? Is it intersecting properly? What could be causing this? If no external cause is present then it is most likely a divergence problem.

yes there is GGI but it is without any overlaping area..as you can see on the picture the wireframe shows each domain..the end winding is seperated into four domains. I also used anisotropic definition for this domain. Please see below CCL for material definition. It is strange that it appears only in one domain.

MATERIAL: CopperStatorOut12
Material Group = CHT Solids, Particle Solids
Option = Pure Substance
Thermodynamic State = Solid
PROPERTIES:
Option = General Material
EQUATION OF STATE:
Density = 8933 [kg m^-3]
Molar Mass = 63.55 [kg kmol^-1]
Option = Value
END
SPECIFIC HEAT CAPACITY:
Option = Value
Specific Heat Capacity = 3.85E+02 [J kg^-1 K^-1]
END
REFERENCE STATE:
Option = Specified Point
Reference Specific Enthalpy = 0 [J/kg]
Reference Specific Entropy = 0 [J/kg/K]
Reference Temperature = 25 [C]
END
THERMAL CONDUCTIVITY:
Option = Orthotropic Cylindrical Components
Thermal Conductivity Axial Component = 296 [W m^-1 K^-1]
Thermal Conductivity Theta Component = 5 [W m^-1 K^-1]
Thermal Conductivity r Component = 4.7 [W m^-1 K^-1]
AXIS DEFINITION:
Option = Two Points
Rotation Axis From = 0 [m],0 [m],-0.265 [m]
Rotation Axis To = 0 [m],0 [m],-0.5 [m]
END
END
END
END


Could the point on the axis affect the results?? I mean is it the same when defining axis like:
from (0,0,0) to (0,0,1)
and
from (0,0,0.25) to (0,0,1)??

To me it looks like a mismatched GGI or some other local problem. Does not seem to be the axis location, but you have not given much detail and so cannot be sure.

it is also strange when ruuning simulation with isotropic material then those errors don't appear..
anyway thank you very much for help..what kind of details would you need to know more??

If this runs fine isotropic then I suggest it is a convergence problem, not a GGI problem. Try converging tighter.

ok ghorrocks thank you very very much for your help

I dont entirely concur. It could have something to do with the large difference in conductivity (axial and non-axial), along with a mesh density mismatch at the GGI interface or a mesh density issue in the respective planes.

Few things you should try:
1) Ensure your interface mesh sizes are about equal
2) Keep material othrotropic but put in the same conductivity (probably use the axial conductivity) for all directions and see if the issue still occurs
3) If 2 works fine, try dropping your non-axial conductivity bit by bit, if the problem occurs when the differences in conductivity becomes large, you most likely have a mesh density issue.

Good point. Definitely worth trying.

thanks a lot singer I will try to follow your steps

Hi, keeper. I met a similar problem in FLUENT. I am hoping I can get some references from you. Did you solve the problem eventually 7 years ago? If yes, could you please tell me if it is mesh problem or not?

Regards