Thermal Contact Solid-Shell

[HVSmith]

Hi - I've recently been investigating thermal conduction in a simple model comprising a solid and a 3D thermal shell, a visual representation of which can be seen in the attached file.

I've done some reading about thermal contact, especially this thread:

http://www.eng-tips.com/viewthread.cfm?qid=158397

and this link:

http://ansys.net/input/therm_cont.inp

The code I have implemented is here:

ET,1,SHELL131
KEYOPT,1,3,2
KEYOPT,1,4,1
R,1						
SECTYPE,1,SHELL
SECDATA,1E-6,1

ET,2,SOLID70
R,2
MP,DENS,2,8000
MP,C,2,502.1
MP,KXX,2,16.26

BLC4,-L/2,-L/2,L,L  					
ASEL,S,AREA,,1
AESIZE,ALL,L/20						
AMESH,ALL

BLOCK,-L/2,L/2,L/2,L/2+L/10,-0.5E-3,0.5E-3
VSEL,S,VOLU,,1
VMESH,ALL

ASEL,S,AREA,,1
ESLA,S
NSLA,S,1
CM,FOIL,NODE
CM,FOIL_E,ELEM
IC,FOIL,ALL,300

VSEL,S,VOLU,,1
ESLV,S
NSLV,S,1
CM,TOPSUPPORT,NODE
CM,TOPSUPPORT_E,ELEM
IC,TOPSUPPORT,ALL,300

ET,3,TARGE170
R,3
KEYOPT,3,1,0

ET,4,CONTA175
R,4
KEYOPT,4,1,2
KEYOPT,4,2,1
!KEYOPT,4,5,3
KEYOPT,4,5,1
KEYOPT,4,9,1
KEYOPT,4,11,1
KEYOPT,4,12,5

TCC=100
RMODIF,4,14,TCC

TYPE,3
ESEL,S,TYPE,,1
NSLE,S,ALL
ESURF

TYPE,4
ESEL,S,TYPE,,2
NSLE,S,ALL
ESURF

Results obtained appear to show that some conduction is occuring in the top block (SOLID70) but only at one edge. The effect is also quite small so requires a re-scale of the contours to see.

From an initial look is anyone able to say whether:
a) contact and target surfaces are what I require to model conductive heat transfer between the solid and the shell?
b) the code I have, above, is likely to be correct? And if so why the conductance would only appear to happen at one corner?

I also am struglling to work out how to calculate TCC for the system, so for now I input a large constant which I hope leads to almost "perfect" conductivity.

Thanks for any insight you can lend, much appreciated
HVSmith

 

[flash3780]

You should really be using multi-point constraints to attach a shell to solid elements, KEYOPT(2)=2. You might also explicitly state that the contact normals are defined by the target surface, KEYOPT(4)=0.

I'd recommend giving section 9.2 of the Ansys Contact Technology Guide a gander.

Here's a link to it:

http://www1.ansys.com/customer/content/documentation/120/ans_ctec.pdf

 

[flash3780]

Also, thermal contact conductance is a material property (the inverse of thermal contact resistance). If two surfaces are welded or are otherwise represent a single piece, it should be effectively infinite.

 

[HVSmith]

Thanks. I've taken on board your advice over the keyopts and the contact technology guide, both very useful.

I've also added in a keyopt(5)=5 on targe170, this seemed sensible from further reading.

In the contact technology guide it states that for shell-solid contact keyopt(1) > 0 are ignored. This has confused, and worried, me quite a lot, since I was using keyopt(1)=2 for TEMP DOF. Keyopt(1)<0 would imply UX,UY,UZ but this is for a thermal analysis, so TEMP should surely be used as a degree of freedom?
Are you able to shed any light on this matter for me?

I've re-scaled the contours in the attached plot to show the result I am getting. Initially both elements are at 300K, so I can see that there is a conduction effect occuring between them, however, it still seems skewed to one side, for some reason. I thought there might be a method of increasing the amount of point contacts, to smear this out, is this even possible? Or the cause?

Thanks
HVSmith

 

[flash3780]

If you refine your mesh, does the asymmetric behavior go away?

 

[HVSmith]

Yes, of course - thanks!
Rookie mistake there...sorry to take up your time, thanks for the advice!
HVSmith