
[Sponsors] 
May 7, 2015, 20:35 
Unstable conduction in solids during CHT simulations

#1 
New Member
Alan
Join Date: Apr 2015
Posts: 11
Rep Power: 3 
Hi,
Just wondering if anyone could have a look at a problem I'm having getting a CHT simulation to converge/reach steady output values? The residuals and values of interest (a number of different heat fluxes) behave well to begin with and almost reach a level/stability that I would be happy with. Then at 2050 iterations (depending on the mesh/timescales) the Tenergy residual begins to increase again and heat flux through the top boundary (fixed heat transfer coefficient and external temperature on a solid domain) and at a conductive (solidsolid) interface near there begin to fluctuate. The fluctuation grows and spreads until the whole simulation looks like a heartrate monitor. I've stopped the run at the beginning of this instability and seen a number of hot spots on what should be cold boundaries. Results from later on in the unstable simulations involve hot spots many times hotter than anything in the model should be. These spots are nowhere near any fluid, but are near a fairly complex geometry involving 45 different solids with different properties. The top domain is a thin (0.6mm) steel sheet (in the context of a 10x0.8x0.45m geometry) too, which is meshed with thin platelike elements. I'm not sure if the problem could be my mesh in this top domain? I thought the heat transfer equations should behave fairly well given a semidecent mesh  maybe mine isn't semidecent? I've tried a range of solid timescales but this just shifts the onset of instability. I've also tried refining the mesh in the region of the hotspots but that brought on instability after only 10 iterations (instead of ~30). I've attached some images that show an initial hotspot, and the coarser and finer mesh in this area. Any help would be great  I'm at a bit of a loss with this one... Cheers, Alan 

May 7, 2015, 23:55 
another image

#2 
New Member
Alan
Join Date: Apr 2015
Posts: 11
Rep Power: 3 
Here is an image of the strange temperature behaviour later on in the simulation


May 8, 2015, 03:06 

#3 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,834
Rep Power: 100 
This is a little strange, heat transfer simulations are normally quite robust.
The first thing I would make sure you are running in double precision mode. Single precision mode can converge for a while and then bezerk, so double precision can assist this. Secondly, your mesh is very coarse so I would refine it considerably. Strange things will happen with a mesh that coarse. 

May 8, 2015, 20:43 

#4 
New Member
Alan
Join Date: Apr 2015
Posts: 11
Rep Power: 3 
Thanks. I have been using double precision, and will try a finer mesh now. I'm bit limited though as I'm already at 34million elements with these meshes.


May 9, 2015, 01:58 

#5 
New Member
Alan
Join Date: Apr 2015
Posts: 11
Rep Power: 3 
I'm still not having any luck  a finer mesh brings on the unstable behaviour even sooner. I've attached images showing the finer mesh and plots of energy residuals and my heat fluxes of interest.
Does anyone have any other ideas? 

May 9, 2015, 06:44 

#6 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,834
Rep Power: 100 
Have you tried smaller time steps? Local Time scale factor?
Please attach an image of what you are modelling and your CCL file. 

May 9, 2015, 21:43 

#7 
New Member
Alan
Join Date: Apr 2015
Posts: 11
Rep Power: 3 
Thanks for looking at this for me; I've attached the files.
Overnight I've remeshed the area (back to a coarser mesh) and set reference states for the solid materials that I had specified in the area (I'm not sure if this has any effect on steady state simulations with fixedheatcapacity materials but I'm trying anything I can think of at the moment). The result is that now the instability grows much more slowly  at 70 iterations my values of interest are only fluctuating by a few percent. This is ok for my purposes, but the instability is still there and growing, and the RMS Tenergy residual is still at ~0.08 so the issue still exists. I'd be interested to know if anyone can explain where I'm going wrong. Some explanation of my geometry: The top and bottom thin, grey domains are steel (0.61mm thick), the two blue domains are air (ideal gas), the top, black domains are 3mm plastic sheets (user defined material) and the light and dark beige domains are insulation (uncompressed and compressed, respectively  both user defined materials). The whole geometry is 10m long and is uniform in that direction except for the triangular ridges and black, plastic domains on top. Boundary conditions: I'm setting symmetry on the two long faces of the air domains and openings at each end of each domain specifying a pressure drop along the geometry. Air coming in is cold. The top surface of steel and plastic has a fixed heat transfer coefficient and cold temp. The bottom steel surface has fixed heat transfer coefficient and hot temp. All interfaces should be allowing heat transfer and all other boundaries are adiabatic walls. 

May 9, 2015, 22:10 

#8 
New Member
Alan
Join Date: Apr 2015
Posts: 11
Rep Power: 3 
I've tried different solid timescales (down to 100s) but haven't changed the fluid timescale from 8s since the fluid is all pretty well behaved. Smaller solid timescales seem to just delay the onset of instability.


May 10, 2015, 06:08 

#9 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,834
Rep Power: 100 
* You have the viscous dissipation model on. It seems highly unlikely that is going to significantly contribute to this simulation, so turn it off.
* Try it with buoyancy turbulence option off. * Where does your physical time step of 8s come from? * Your last comment suggests that the reference conditions are making a difference. This means: 1) You need to make sure your reference pressure and temperature are set for all materials and are appropriate (I see your boundary temperatures are between 0 and 20C, so your reference temperature should be in this range); 2) You obviously have marginal numerical stability so you are going to have to be careful, so small time steps and high mesh quality will be required. * I would also recommend saving a results file at the time the simulation first goes unstable. Have a look at what happens at that time  is it when the inlet flow first reaches the outlet? Or a hot plume hits the top boundary? Or some other flow thing happens? The instability could be triggered by a physical process. 

May 11, 2015, 01:08 

#10 
New Member
Alan
Join Date: Apr 2015
Posts: 11
Rep Power: 3 
Ok, I've tried running the problem without viscous dissipation and buoyancy turbulence and with auto fluid timescaling (=~0.01s). The result is that the same growing instability in the conduction remains, but is now superimposed over the new, slowerconverging system behaviour (due to smaller fluid timestep)  Tenergy residuals still diverge at more or less the same rate.
The problem really does seem to be isolated to my solid domains  this is where the instability begins (an image showing the onset of temperature instability at the point where it initiates is in my first post). Zooming right in on plots of heat flux in this area, the instability is there from the begining, just extremely small (it shows as a slight zigzag with a period of 2 iterations). By changing mesh and solid timescale I have only been able to slow the growth of this instability. I have a feeling that the improvement I mentioned in my last post may be from the new mesh rather than the introduction of reference states for my materials, though I could be wrong. It's just a feeling I have given the changes I've seen so far with different meshes and the fact that heat capacity shouldn't have any bearing on steadystate behaviour (though maybe it does affect CFX's use of timescales/timesteps?). I'm trialing a number of different meshes and solid timescales for now (with viscous dissipation still removed  thanks). Any other suggestions would be very welcome. 

May 11, 2015, 02:35 

#11 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,834
Rep Power: 100 
I suspect the root cause of this problem is the extremely thin solid body compared to a large domain size. Large changes in geometry scale can be very hard to converge. So is it possible to not model the thin solid and replace it with a thermal resistance boundary condition? You have to write this boundary condition yourself but it is pretty easy using CEL and works well.
This is likely to be a big improvement in model stability. 

May 11, 2015, 03:03 

#12 
New Member
Alan
Join Date: Apr 2015
Posts: 11
Rep Power: 3 
I think the resistance of the thin domain could be neglected entirely actually (being steel and so thin), it is really included to capture the lateral conduction along the boundary which could have a significant effect. Maybe I will need to leave it out though.
I think I'm going to eliminate the triangular ridges and model the top steel sheet as a thicker, flat sheet. I'll post here whether that helps or not. Thanks again for your help. Any more thoughts are welcome of course 

May 11, 2015, 03:18 

#13 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,834
Rep Power: 100 
A simple back of the envelope calculation will determine whether transverse conduction is important. It is sounding like you do not need to model the thin steel sheet at all and that will probably fix your problem.


May 12, 2015, 22:30 
Problem solved

#14 
New Member
Alan
Join Date: Apr 2015
Posts: 11
Rep Power: 3 
Hi,
I just thought I'd post a solution here in case anyone has a similar problem. So I tried simplifying my geometry and increasing the thickness of the top, steel sheet but the problem remained. I then started subtracting features and worked out that the problem was to do with the interaction of the sweep method and some split faces in that top domain (the elements were given a slight kindofskewness  changing what should be 90degree angles to approx. 75105 degrees). I couldn't get the sweep method to behave better, but after changing the sweep settings from rectangles to triangles, to make all elements prisms instead of hexa elements, the problem disappeared. I guess the hexa elements are more sensitive to this 'skewness' or the high aspect ratios? 

May 13, 2015, 05:52 

#15 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,834
Rep Power: 100 
In my experience hexas are not more sensitive to skewness. But the quality of the prisms you generated is likely to be much better than the distorted hexas you had. And high quality prisms are definitely better than low quality hexas.


Tags 
conjugate heat transfer, convergence problem 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Can CFX do CHT simulations with a solid domain rotating in a stationary fluid domain?  acro  CFX  15  September 23, 2016 11:16 
How to model transient conduction between two solids?  cliffdub  OpenFOAM Running, Solving & CFD  14  December 15, 2015 13:32 
chtMultiRegionFoam, conduction with a contact resistance between two solids  romain.h  OpenFOAM Running, Solving & CFD  1  October 8, 2013 01:25 
Hardware selection for steady/unsteady incompressible, turbulent and cht simulations  maddalena  OpenFOAM  2  July 13, 2011 08:55 
conduction between 2 different solids  matt  FLUENT  5  November 9, 2006 09:57 