Spurious oscillation in heat transfer analysis 1

[tianle]

I've met a problem with ABAQUS.
In fully coupled thermal-stress analysis (or just simple heat transfer analysis), there's a phenomenon called
"Spurious oscillation", which is stated in ABAQUS/Doc as below:

Spurious oscillations due to small time increments
In transient analysis with second-order elements there is a relationship between the minimum usable time increment and the element size. If time increments smaller than this value are used in a mesh of second-order elements, spurious oscillations can appear in the solution, in particular in the vicinity of boundaries with rapid temperature changes. These oscillations are nonphysical and may cause problems if temperature-dependent material properties are present. In transient analyses using first-order elements the heat capacity terms are lumped, which eliminates such oscillations but can lead to locally inaccurate solutions for small time increments. If smaller time increments are required, a finer mesh should be used in regions where the temperature changes rapidly.

I frequently encountered this problem and because my model is for 3D-fully coupled thermal-stress analysis, the mesh size can't be too small in consideration of computation cost.
Anyone can help me?
Thanks a lot!

 

[xerf]

I think the oscillations are common to the explicit schemes.
(also the restrictions on the time increment)

If you're using ABAQUS/Explicit, then you might be interested in changing to ABAQUS/Standard ...

 

[tianle]

xerf,

Acutally I'm using Standard.

Tianle

 

[rstupplebeen]

Tianle,

You might want to try first-order elements and with the time savings of the simpler elements use a tighter mesh to get the accuracy you need. Hope this helps.

Robert Stupplebeen

 

[tianle]

Hi, Robert
What I used is S4T in Abaqus which is fully coupled
thermal-stress shell elements(with 4 nodes). "with time savings of simpler elements"? Would you please make me clearer?
ABAQUS/Doc suggests me to user finer mesh, but my problem
is, I think it already very fine. Because it's a fully coupled thermal-stress analysis with contact, the computation is quite complicated and time-consuming, if I refine the mesh, the computation time might be unbearable...

 

[corus]

You see this problem in both Standard and Explicit and is akin to stability of finite difference methods. What I've found is that although you see these variations at the beginning of the transient, where there are sudden changes intemperature, they soon disappear and the solution you get later in the transient isn't affected to any significant amount. If you're concerned about the initial behaviour then try doing a smaller model (say using 2D elements) in that area where you can make reasonable assumptions about the boundary conditions away from that region. You can then judge whetehr it's of any signifciance or not to your results later in the the transient.

corus

 

[rstupplebeen]

Tianle,

Your first message made me think that you were using second order elements but apparently you are using first order. I think corus is getting you down the right path.

Rob

 

[tianle]

corus,
Did you mean you meet the same problem by finite difference method? I'm not sure if what I met is akin to
the instability to FDM. However, my model is fully coupled thermal-stress analysis with contact and geometrically nonlinearity, the considerable spurious oscillation may be not very significant at the beginning but it may cause significant difference at the end due to the high nonlinearity.
Actually the oscillation is caused by forced convection on a surface (modeled by shell elements S4T). Someone told me that I could find the theoretical description on this topic in some advanced finite element books while I've not got it so far. Maybe I would follow your suggestion, to setup a smaller model and then to examine the effects on the oscillation.

 

[corus]

A smaller model is a better way of seeing if there is a general problem with convergence, and faster too! With finite difference methods the theory is easier to understand and I remember that there was some problems with time steps and mesh as to convergence. There is a simple formula to get an estimate of the initial time step you need, which I forget now. It was something like 4(mesh size)^2/diffusion but that's from memory. I've always found though that the more non-linearity you have in a problem then the less likely you'll succeed in getting a solution, and you may be better by simplifying it a little, say by using linear properties, or removing large displacements, rather then trying to include every possible behaviour you can think of. Reintroduce these non-linearities one at a time to see what effect it has and to see if you have convergence problems with each new property.

corus

 

[marine59]

Your problem has nothing to do with any particular implementation/FEA/FDM. It is telling you that the time increment cannot be shorter than is dictated by the material properties and the discretization size, or your transient solution will be oscillatory.

I am surprised that ABAQUS says it is a function of of the order of the element. A transient solution should show the same problems element-element if you violate the rules. If the solver can't relax a solution in the time intervals demanded, it won't.

Sinda G manual or TAK manuals have good explanations.
or see Carslaw and Jaeger
or the Handbook of Heat Transfer.

Sorry I can't provide detail but my HT books are elsewhere and I've been working stress/structure for the last 3 years. It's like cleaning your desk between jobs.

Gerry Starkeson
Principal Mechanical Engineer
Aerospace - Stress/Thermal

 

[tianle]

It is recounted in ABAQUS/Doc that for 2nd order element,
time increment 'Delta t' should be
Delta t > (Density*Specific heat)*(Delta L)^2/6k
where k is the thermal conductivity. ^2 means power law of 2
Delta L stands for the typical element size.

Also, it's stated that for 1st order element, this formula
might not fit, and the only thing is that the time increment can't be too small or the result will be inaccurate.

I know my problem is. I just face to how to solve it. It's said the upwinding scheme might be effective but I'm not sure, either do I know how to implement it in ABAQUS.