contact element die+grease+copper

[richardforever]

Hi everyone,
I have several doubts in how implement the ansys code to simulate a thermal contact interface between two different materials. My model is a die attached to a copper structure with a thin layer of a thermal grease. I have used conta 172 + targe 169 to model that and I have turned the keyopt on that I think are appropiate with this:

ET,3,CONTA172
KEYOPT,3,1,2
KEYOPT,3,2,1
keyopt,3,5,3
KEYOPT,3,12,5
R,3,,,,,,,
RMORE,,,,,,,
RMORE,,5,,,,,
ET,4,TARGE169

As you can see I just wanna introduce the TCC parameter in order to that the program know how the heat pass through the material and the resistance opposes to the heat flow.

Should i have to introduce more real constant. How is the way to proceed?. Thanks for the helpful responses.

 

[rickfischer51]

Assuming you value for TCC is 5, that looks correct.

When you have a question like this, dont ask, just try it. Build a simple model with a couple of blocks and one contact element and try it. You learn more by doing than by asking.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[richardforever]

Thanks for the advice Rick. Really I have started to build a simple model with two blocks of different materials (it's a simplified model of the complete model which has several fins). The problem has convection at the bottom edge with h=51 W/m2ºC and T=50ºC which I have implemented through plane77 for the solid and surf 151 with an extra node for the convection. Reviewing the err file I realised that something has gone really wrong.
First it is supposed that it's a non linear problem and I get an message saying that using 1 iteration per substep may result in unconverged solutions for nonlinear analysis.
Secondly i have used node 5000 to put temperature of 50ºC and i get the warning:"Specified degree of freedom constraint TEMP at unused node 5000". Does it mean that i cannot do that?.
And the more strange messages are the following ones: "There are 1 small equation solver pivot terms. This may be a
transitional effect caused by the Newton-Raphson logic." ( my problem is static problem) and "The value of TEMP at node 79 is 1.1258999E+15. It is greater than the current limit of 1000000. This generally indicates rigid body motion as a result of an unconstrained model."

As you can see I'm stuck in this. I show you my imput file:
FINISH
/CLEAR
/PREP7
RECTNG,,0.01,0.0025,0.01
RECTNG,,0.0225,,0.0025
ET,1,PLANE77
KEYOPT,1,1,0
KEYOPT,1,3,0
ET,2,SURF151
KEYOPT,2,3,0
KEYOPT,2,4,0
KEYOPT,2,5,1
KEYOPT,2,6,0
KEYOPT,2,8,2
KEYOPT,2,9,0
ET,3,CONTA172
KEYOPT,3,1,2
KEYOPT,3,2,1
KEYOPT,3,5,3
KEYOPT,3,12,5
ET,4,TARGE169
!Thermal Contact Conductance
TCC = 5 !14 Thermal contact conductance
R,3,,,,,,,
RMORE,,,,,,,
RMORE,,TCC,,,,,
R,1
R,2
UIMP,1,DENS,,,3500
UIMP,1,KXX,,,50
UIMP,1,C,,,500
UIMP,2,DENS,,,8900
UIMP,2,KXX,,,393
UIMP,2,C,,,385
ASEL,,LOC,Y,0.0025,0.01
AATT,1,1,1
ASEL,,LOC,Y,0,0.0025
AATT,2,1,1
ALLSEL
APLOT
ESIZE,0.025/10
AMESH,1
AMESH,2
!Mesh target surface 1-2
ASEL,S,AREA,,2
NSLA,S,1
NSEL,R,LOC,Y,0.0025
NSEL,R,LOC,X,0,0.01
ESLN
TYPE,4
REAL,3
ESURF
!Mesh contact surface 1-2
ASEL,S,AREA,,1
NSLA,S,1
NSEL,R,LOC,Y,0.0025
ESLN
TYPE,3
REAL,3
ESURF
!SURF 151 elements
LSEL,R,EXT
LSEL,R,LOC,Y,0
NSLL,,1
ESLN
N,5000,,-0.01
TYPE,2
REAL,2
ESURF,5000
ALLSEL
SAVE
FINISH
/SOLU
!To solve the problem as a static linear problem
ANTYPE,STATIC
SOLCONTROL,OFF,OFF
NSUBST,1,1,1
NEQIT,1
LNSRCH,OFF
NLGEOM,OFF
BFA,1,HGEN,5333333.3
!Convection
ESEL,,TYPE,,2
SFE,ALL,1,CONV,,51
ALLSEL
D,5000,TEMP,50
! Visually check the charges
/PBC,TEMP,1
/PBF,HGEN,,1
/PSF,CONV,2
EPLOT
SAVE
SOLVE
CNCHECK
FINISH
/POST1
/SHOW,PNG
SET,LAST
ESEL,S,TYPE,,1
ALLSEL,BELOW,ELEM
NSLE,S
PLNSOL,TEMP,,0
FINISH

 

[rickfischer51]

1. Ansys likes to print that message for no good reason. It sees contact, but is too dimwitted to see that keyopt,3,12,5 is bonded contact. Ignore it.
2. Node 5000 is not connected to the model. It has no elements associated with it. You can do it, but it doesn't do anything and it usually doesn't make a lot of sense. See #4 below.
3. The low pivot ratio is just a warning. it may go away when you fix the model. See #4 below.
4. You have applied heat generation with no place for the heat to go. You have no SURF151 elements, so there is no place to apply the convection. There was a warning at the output window that no surface elements were created because no exterior face of the selected elements had all its nodes selected. Type SFELIST at the command line and you will see you have no SF loads, ie no convection. Confirm this with ESEL,S,TYPE,,2 and EPLOT. The 50 degree temp on node 5000 is not attached to the model. So, the software calculates an essentially infinite temp at node 79.

When debugging a model, check your filename.err file for warnings and errors. They go by pretty fast in the output window and are easy to miss.


Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[richardforever]

Thank you very much for the help.
I have solved the problems described above but I still have several ones. The result of the distribution of temperatures seems to be a bit exaggerated for me. I have compared with another model where instead of using conta172+targe169 I have introduced the thickness, the area and properties of the thermal grease layer to have something to compare where I obtain T_max = 404.149ºC and T_min= 397.402ºC and the model that I'm trying to solve gives me T_max = 8433.36ºC and T_min = 397.379ºC. My main concerned is about the mesh because I think that it can be the source of the problem but I'm not sure. I have realised that if I introduce:

ESIZE,0.025/40
AMESH,1
AMESH,2

the mesh is fairly regular but I think that for my contact problem is not really good because doesn't allow to mesh with accuracy the region of interest where the contact is found.
However if I introduce:

SMRT,6
ALLSEL
AMESH,ALL

a huge amount of points are created in the contact zone but I obtain more errors of the following type:
"Shape testing revealed that 12 of the 701 new or modified elements violate shape warning limits."
If I see the mesh I can see that is not very regular and the element's shape already meshed are not square at all (they have strange shapes).
I don't know what does "warning limits" means and which option to mesh the model is more appropiate for this kind of problem.
Thanks for advance.

 

[rickfischer51]

Run the problem with simple loading. Remove the HGEN and put a high temp at the top, say 500 deg, and run both your models. Now you have a simple linear conduction problem. Do a simple finite difference hand calc with 3 elements (A1, grease, A2)in Excel and compare it to your models.

You need to transition gradually between areas of coarse mesh and fine mesh. An all tri mesh may help. I'm not a fan of Smartsizing. Look at the MOPT command, and the various XREFINE commands (LREFINE, EREFIND, NREFINE, etc). Mesh the grease area first, then try free meshing the two large areas. You might need to slice A1 and A2 into smaller areas to better control the transition.

I would be leery of meshing the grease with one element through the thickness. The temp at each node is an average of elemental values extrapolated to the nodes from the integration points. With one element through the thickness, you do not have any nodes with temperatures calculated purely with grease properties. In a previous life when I ran mold filling simulations, we got bad gate freeze-off prediction when we modeled the gate with one element. With five elements, we got pretty good agreement with the real world. I suspect the same might apply here.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[richardforever]

Something with the simulation is going wrongly. I have already put temp of 500 deg at the top and with "smartsizing" the temperature drops very quickly from the top to the bottom (500 deg at the top to 68.63 deg at the bottom ) which is something illogical because the temperature cannot do that so fast. It is supposed that it will keep at a temperature near of 500 deg.

Regarding to the mopt command i understand that it is focus specially on models where the outter areas must have a fine mesh while the inner areas have a coarse mesh. In my case the contact element is a line of nodes, it is not an area so I think in this case this is not useful or I have not understand how to do what you told me. And by the way which command I have to use to slice areas? Is it supposed that after that i have to glue them to mesh them or not?

The last thing is that I have tried to do the lrefine command but an error appeared saying that "Invalid line (1) selected for mesh refinement". I have just introduced the following command:
/PNUM,LINE,1
LPLOT
LREFINE,1,1,1,1

The error pop ups here and I don't know why. Really I am a bit in despair. Thank you for your responses and suggestions.

 

[rickfischer51]

1 Why cant it do it that fast? What is the basis for your expectations? What happens when you change k? Start with a simple one dimensional model and do hand calculations. then model the same thing with Ansys. When the two match, you have your Ansys technique correct.

2 to slice areas, look at boolians like ASBL and ASBA.

3 First you are telling it to refile line #1 to line #1 in increments of 1. that's nonsensical. try LREFINE,1,,,1. Second, did you specify meshing parameters with something like LESIZE? third, per the manual:

"You cannot use mesh refinement on a solid model that contains initial conditions at nodes [IC], coupled nodes [CP family of commands], constraint equations [CE family of commands], or boundary conditions or loads applied directly to any of its nodes or elements. This applies to nodes and elements anywhere in the model, not just in the region where you want to request mesh refinement. For additional restrictions on mesh refinement, see Revising Your Model in the Modeling and Meshing Guide."

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[richardforever]

I appreciate a lot your help.
In first place i have managed to slice the big areas (the area 1 has been split into 3 smaller areas and the area 2 has been split into 4 smaller areas) and i have used command ASBL to substract the areas (starting with creating lines from keypoints). So far everything has gone well. After that, I guess that i have to put "lesize" command on the line which my contact zone is. I have entered this:

LESIZE,11,,,10 !Line 11 is where the contact is found. As you can see i have split the line into 10 divisions

Really I don't know exactly what is useful for. But assumming that this will help me to mesh my model more accurately I keep on.
Then and not to use smartsizing I use this before of using lrefine:
ESIZE,0.025/60 !Define my element size
AMESH,ALL

At this point is where i think i have to use lrefine command (please correct me if I'm wrong). So I use:
LREFINE,11,,,1

But an error says me "No meshed areas are attached to a selected line (11). The LREF command is ignored. "
What am i doing wrongly if in order to introduce lref command i have to have the model meshed and ansys doesn't let me do that?
To finish about "mopt" command i have tried to put
MOPT,AMESH,DEFAULT
The help of ansys says that this is a triangle surface-meshing option but instead of this , that creates square meshed elements. I don't understand why. What mopt option would you think that could give me a exact solution?. Thanks a lot.

 

[richardforever]

I have already solved the problems commented above.
But I still have the problem that the solution that ANSYS gives me doesn't make sense.

1) Using a generation of heat of 20 W which is the power that the die dissipate:
I have done manual calculations ( the max temp for my model is 406,856ºC) According to the model done with the area and thickness of thermal grease (without conta + targe elements) gives me max temp = 404,149ºC so it seems that it's correct what i had done.
But the last model with conta + targe elements, doing the mopt, lesize and lrefine commands and splitting the big areas into smaller ones in order to mesh them correctly gives me a max temp of 8791.69 ºC for the silicon die and 389ºC for the copper ( it seems too much difference of temperature among them which i think is wrong plus the distribution of temperature is homogeneous in each material) only appears colour red for silicon and blue for copper.

2) Applying a temp fixed at the top of the die (500ºC) as you told me, the model with the area and thickness of the grease gives me max temp = 500ºC, min temp = 487,982 (something reasonable) and on the other hand the model with conta+targe elements gives me max temp= 500ºC and min temp = 67.45ºC. (again with a homogeneous temperature in each material)
Really in this situation i have doubts in how do manual calc cause i don't know how to treat the temp of 500 fixed at the top. Is it supposed that i convert into a heat flux/area in units of W/m2? How i do that?
Thanks and forgive the inconvenience.

 

[richardforever]

Definitely I think the problem is not about the mesh but about the definition of the contact.
I wrote the "CNCHECK" command in ansys and the following appeared. I don't know if the contact is well defined. Could you help me?

*** NOTE *** CP = 3.297 TIME= 12:42:21
Deformable-deformable contact pair identified by real constant set 3
and contact element type 3 has been set up.
Pure thermal contact is activated.
The emissivity is defined through the material property.
Thermal convection coefficient, environment temperature, and
heat flux are defined using the SFE command.
Target temperature is used for convection/radiation calculation
for near field contact.
Contact detection at: Gauss integration point
Average contact surface length 0.30303E-03
Average contact pair depth 0.32093E-03
Default pinball region factor PINB 0.25000
The resulting pinball region 0.80232E-04
Auto offset used to close gap/penetration -0.21467E-18
Initial penetration/gap is excluded.
Bonded contact (always) is defined.
Thermal contact conductance coef. TCC 5.0000
Heat radiation is excluded.

*** NOTE *** CP = 3.297 TIME= 12:42:21
Max. Initial penetration 2.168404345E-19 was detected between contact
element 466 and target element 460.

 

[richardforever]

I have resolved the problem!!!!!!!!!

The key was in the keyopt (2) of the conta172.
I had to change Penalty Stiffness factor to "MPC Contact". Doing this the distribution of temperatures is correct!!!!. Thanks for the help an sorry about my insistence.