FULLY COUPLED THERMAL STRESS - convergence problem

[mvp23]

Hi,
I’m performing a fully coupled thermal stress analysis of a foil sandwiched between 2 cylindrical tubes.
Kindly look at the attached file to see how the foil is oriented between the cylinders.
Also , I have the message filed and cae file attached.

The 2 ends of the cylindrical tubes are welded together once the foil is placed between them . However in Abaqus , since there should be a fixed constraint , I applied a tied constraint to one end of the inner and outer cylinder and an ENCASTRE BC to the other end of the cylinders.
Of interest to me is the Contact pressure and the temperatures

Following are the settings used in the STEADY STATE analysis
1. Using Abaqus standard
2. Mesh – Linear , C3D8T Hex elements
3. STEPS – coupled temp disp ,NLGEOM ON
4. Solution Technique – Full Newton
5. Interaction property – Penalty friction formulation and hard contact
6. Interactions – I used the ‘Find contact Pair’ option to find all possible interactions

Problems encountered :
Basically I have been unable to obtain convergence!
- inner tube and outer tube are distorting excessively
- displacement increment for contact is too big

I’ve been reading through posts in this forum hoping to overcome these issues , but I have been unsuccessful until now.

I would be grateful to anyone who could help me out .

Thanks

 

[mvp23]

here is the message file

 

[mvp23]

the assembly pic

 

[corus]

In the load module you define heat generation for a steady state step, but with no other thermal boundary conditions. When you have heat generation and no cooling, then temperatures will be infinite in steady state. Either define other boundary conditions or input an initial temperature distribution and run the job as a transient over a fixed time period.

Tara

 

[mvp23]

corus ,

I specified a sink temperature ( coolant temp ) and a heat transfer coefficient in thermal interactions , but I still get the same errors as before. I have attached the updated cae file , along with the msg file. what else could be wrong ?

 

[mvp23]

here is the message file corresponding to the cae file in the above post

 

[corus]

You've defined heat transfer for the inner and outer cylinder surfaces but none for the foil inbetween. When contact is made then heat loss from the foil will be via conduction, but initially there is no contact, and so no heat loss from a foil which has heat generation in steady state. I think you need to specify heat loss using gap conduction/radiation so that you have heat flow via conduction in contact (zero gap) and radiation otherwise.

I'd also refine the mesh so that the aspect ration is closer to 1. Also check the adjustment made for contact as some nodes are being moved a significant amount to close initial gaps, hence you get element distortion even before the job starts. Look in the odb file (even if the job has failed) to see these distorted elements.

Tara

 

[mvp23]

Corus ,
the problem im looking at is after assembly , so the foil is in contact with the tubes. moreover , the thermal contact resistance ( reciprocal of thermal conductance) is taken into account here.
so the energy from the foil goes through the tubes , with which it is in contact ( there is a contact resistance here) and there is coolant flowing on outer surface of the outer tube and inner surface of the inner tube that takes away the heat. thats why i specified the coolant temp and 'h' for the inner and outer tubes.
however , when i specified my interaction properties (thermal) , I gave in a value for the air gap conductanc (h air).

as per your suggestion , i ll look into mesh refinement and the odb file to view the distorted elements.

 

[mvp23]

if I may add to my previous post

so the idea is to to determine the thermal contact resistance , along with the contact pressure and nodal temperatures.
the contact pressure includes the assembly pressure and the pressure due to thermal expansion.

 

[mvp23]

Thanks for the help corus . I re-did the assembly and contact definitions which helped to resolve the excessive element distortion issue. I still do have convergence problems due to SDIs . One of the errors from the attached message file is as below :

3742 SEVERE DISCONTINUITIES OCCURRED DURING THIS ITERATION.
58 POINTS CHANGED FROM CLOSED TO OPEN
3640 POINTS CHANGED FROM SLIPPING TO STICKING
44 POINTS CHANGED FROM STICKING TO SLIPPING

I have the automatic overclosure tolerances and auto stabilization turned on. I'm doing a node-surface discretization and a Full-Newton technique with NLGEOM turned off. Are these problems related to contact chattering or slip reversal ?

I have the message file for this particular job attached.

 

[corus]

It would help to halve the model and use symmetry on the cut planes. You can then use a finer mesh and get better results. I'd try a mesh size of 0.001 rather than the value you use now.

I'd also prevent any initial overclousre in your contact definition and use small sliding. You can switch back to finite sliding later if the relative distorion is signficant.

The 'chattering' in contact may be due to the thermal conditions across the gap. I'd use radiation for a non-zero gap instead of having zero conductivity which may be causing sudden changes in temperature if in contact or not. Radiation would be the correct condition to apply across a gap anyway.

Tara

 

[mvp23]

Hello Corus ,
I got my model to converge. It had to do with the very low value of gap conductance being used .
I would like to know how exactly the conductance vs clearance relationship is to be defined ? I read through the manual , but all that it says is a conductance needs to be defined at zero clearance and another value as the clearance increases.

I use Abaqus 6.10 and it expects an input of
conductance - clearance as opposed to earlier versions where the user is expected to input conductivity-clearance. I know abaqus defines the gap conductance based on newton's law of cooling as hgap=q''/deltaT .
I am confused about defining a 'gap conductance 'value for 'zero clearance'. My understanding of this is - when there is zero clearance , both the materials are in contact. In that case why would you need a 'gap conductance' value ?.

Hope you could shed some light on this issue.

 

[corus]

Looking at the manual it seems the gap conductance is in units of W/m^2 C, ie. is the same as a heat transfer coefficient or k/x where x is the gap and k is conductivity. I would guess that with a zero gap then the gap conductance would be infinite, ie. the temperatures on either side of the 'gap', or at the point of contact, are equal. Obviously you can't input 'infinity' as a value so you'd have to just input a large value. Similarly it assumes that the gap conductance is immediately zero after the last value defined in the data lines, ie. the gap is infinite and k/x is zero. Mathematically it's not very tidy and I can only assume that part of the software was written by an engineer.

You probably need to input a value of gap conductance for zero gap so that it can interpolate between zero and the 2nd data point you've input. My guess is that for this inverse function of x they use linear interpolation. Sigh.

Tara