Surface to surface contact

[AntCrespo]

Hello,

I'm trying to model a thermal problem where I have a shape that I have built by composing instances of two different parts designed in abaqus CAE, so that one part rests on top of the other.
I want to heat up the base of the lower part and have the heat conducting into the upper part. I have tried estabilishing a surface to surface contact between the two contacting parts, with a contact interaction property that I chose to be a conductivity. Since the two parts are of the same material, that made sense to me, but still no heat is going from one part to the other.
I looked it up in the manual but couldn't find anything very helpfull. The manuals seem to focus a lot on mechanical problems and less on thermal ones...
Can anyone help, please?

 

[EngForm78]

AntCrespo,

Is the problem steady state? Are you using standard or Explicit? Is the temperature applied as a field varible?

A standard steady state solution should be straight forward with the right material properties.

EngForm78

 

[corus]

If you're not bothered about thermal resistance at the contact then just tie the surfaces together. If the parts are displacing then you want a coupled thermal displacement model. You define the conductivity based upon the distance apart, I believe.

corus

 

[AntCrespo]

Thanks for replying.
The problem is not steady state and I'm using standard. Also, I'm using CAE and inputing the heat as a thermal load into the bottom surface of the lower part. Actually I apply the thermal load during the first two steps and let it cool off for 5 or 6 smaller steps because I need to watch the evolution of the cooling thermal field.
Thermal resistance should not be a problem, I want the two parts to be a single "physical" object. At this point I'm not interested in displacement analysis yet. And you're right Corus, conductivity is defined as a function of the distance apart, I defined it as a the value for my material for a 0.0 distance and defined it as 0.0 for a distance of 0.00001. I believe abaqus interpolates for the values in between.
Isn't surface to surface contact a suficient condition for the two parts to be at a "zero distance" at those surfaces?
Thanks again for replying. Any further help will be higly appreciated.

 

[corus]

I'd try a bigger value for your second term in the gap conductance. You can get rounding erroros in CAE due to the translation of the instance, for example, that can put your co-ordinates out. For your case it would make no difference if you put in a larger value for the second term. See section 22.2.1 of the manual for a full description of gap conductance. As I said before though, it'd be much easier just to tie the nodes together at the interface.

corus

 

[mrgoldthorpe]

AntCrespo,

As Corus says, tying the temperature dof is best if you have nodes on the mating surface that correspond:

** Tie temperature degrees of freedom:
*EQUATION
2
NSURF_UP , 11 , -1.0 , NSURF_LO , 11 , 1.0

where NSURF_UP is the unsorted nodes set on the upper mating surface and NSURF_LO the corrsponding node set
on the lower.

MRG

 

[corus]

mrgoldthorpe,
I'm not sure that is correct as the *equation will use the node numbers in the order that they appear in the set which may give errors if the nodes in the corresponding set aren't in the same order. I believe that you can simply tie the two surfaces together as in a surface to surface contact.

corus

 

[mrgoldthorpe]

Corus,

*NSET, NSET=NSURF_UP, UNSORTED
1,2,3, ....
*NSET, NSET=NSURF_LO, UNSORTED
1001, 1002, 1003 ....

putting the nodes in the same order is OK, provided of course there are an equal number of matching nodes on each surface.
MRG

 

[AntCrespo]

Thanks for helping.
Corus, I think your suggestion solved my problem. It took me a while to do it because the contacting surfaces I was trying to tie were not the same size, and I was getting an error message saying the assembly was not consistent. I then tried with two similar surfaces and I think it worked. I'm still checking a couple of things because sometimes there seems to be a gradient of temperatures at the interface and I was not expecting that, so I'm analyzing the thing. Still I am not able to do it when I have a smaller part resting on top of a larger one. Can it be done in a similar way? I'll be looking on the manual for that. Thanks for putting me in the right track, anyway.
I have one question: why wasn't it working when I had a surface to surface thermal interaction? What in fact is that? It didn't look like anything was happening, the simulation ran as if the two parts were completely unrelated, so I'm doubtfull any interaction was estabilished at all...
Mrgoldthorpe, thanks as well, I think your suggestion will be helpfull when trying to tie a smaller surface to a specific region of a larger one. I think I will have to define a node set of the larger surface that corresponds to the contact zone with the smaller one, and then, do as you say. Is that it?
Thanks again for your valuable help

Antonio

 

[corus]

You can check your results by looking at the contours. If the nodes are tied correctly then the contours should be continuous across the two surfaces. The gradients may differ if you have different materials. There may be a slight error in the contours at the interface as surface to surface tied nodes are made approximately, so that if one node is tied to another surface in which there is no directly oppposite node, then an interpolation is made.

Gap conductance should have worked between the two surfaces regardless of surface sizes. Remember that the gap conductivity is k/x ie has units of W/m^2 K and not W/m K as you'd expect. An infinitely high conductivity in the gap would have ensured that the temperatures across the gap were the same.

corus

 

[AntCrespo]

Hi,

I was looking at the contours, but I was applying a homogeneous thermal load at the bottom surface, so the isothermals were straight lines paralel to the contacting interface and I could only have a suspicion that something was not right.
Then I applied a concentrated heat flux (thermal load at one point) so that the isothermals are curved, and there's an evident discontinuity at the interface...
Summarizing: I created a part (a slab) and assigned it thermal properties. Then I created 2 instances of that part (to make sure they have the same thermal properties) and placed one on top of the other. Tied the contacting surfaces and applied a thermal load. I expected it to behave as single piece of material but there's a descontinuity at the interface. The upper part is aproximately one element "out of phase" with the bottom one.
Does anyone have any idea of what might be wrong? Is my assumption that it should behave as a single piece incorrect?
Sorry to keep pushing on this...
Thanks for any help you can spare,

Antonio

 

[AntCrespo]

The situation I'm trying to model must seem a little trivial, instead of using two instances I could use a single part twice as big.
Actually, I hope to arrive at a model that allows me to simulate the deposition of molten particles on top of a substrate of the same material. After depositing the particles, they will be part of a continuum of material, composed of the original substrate plus the deposited material on top.
I'm new to abaqus, so I started with something simpler and I'll try to work from there. The particular situation I've put to discussion is the basis of the process I want to build.
Just to clarify that this is not a total waste of your time.

Antonio

 

[corus]

If the contours are passing between the two then at least it shows that heat is being transferred across the boundary. As I said before, you can get an error in the temperatures that are tied. This error can increase the larger the discrepancy between nodal positions. Try and have your meshes line up with each other if possible.

corus

 

[AntCrespo]

Thanks Corus, you've really helped me a lot.
I'm running a heat transfer analysis, and in fact, the temperature is smoothly continuous across the interface, BUT the heat flux is not, which still strikes me as strange. I guess the *TIE is imposing an equal temperature at the contacting nodes but there must be some problem with the heat flux, probably some discontinuity in the value of the conductivity at the interface.
Thanks again

Antonio

 

[corus]

The heat flux across the contact region will be the same if the temperatrure gradient is the same. You can simply check this by looking at the shape of the contours at the interface. If it's not and you've used an infinite conductivity across the gap then you must have different materials assigned to each part.

corus

 

[AntCrespo]

Corus,

I was using abaqus 6.3-1, but now I'm using abaqus 6.5-4 and in this version it is possible to merge parts in the assembly module. Basically it allows you to mesh two different parts as if they were only one and avoid having to estabilish tie constraints between the interfacing surfaces.
I'm still getting to know this feature but it seems really helpful.
Just wanted to share this because it seemed an important piece of information regarding the subject being discussed.

Antonio