you are here:   / News & Insights / Engineering Advantage Blog / Tips & Tricks for Modeling Thermal Stress Analysis of Assemblies

# Tips & Tricks for Modeling Thermal Stress Analysis of Assemblies

December 18, 2015 By: Peter Barrett

Predicting accurate thermal stresses in mixed material assemblies can be a challenging analytical problem. Thermally induced stresses are created by temperature gradients, supports, and when the connecting materials have different coefficients of thermal expansion (CTE). For the CTE mismatch case, even a uniform temperature will result in differences in thermal strain, which will induce mechanical strains and stresses. Modeling assumptions for these connections can have a major impact on the local stresses. The first question the analyst must answer before modeling these types of assemblies is: What keeps the parts together? Is there an actual bond via an adhesive, weld etc., or is it a mechanical support from a bolt or spring? Can the connection be assumed to be bonded or is this an assembly of components where the individual parts are free to slide and/or separate?

From an FEA prospective, the modeling setup can be a flow-through mesh, bonded, no separation or frictional contact. Each of these different modeling procedures introduce numerical challenges in regards to accuracy of stress reporting and numerical convergence. Modeling of the adhesive or weld material may or may not be included in the simulation. When these connectors are ignored, simplifying assumptions can produce numerically induced singular stresses.

In order to better understand these assumptions, this post provides results of a series of comparative connection simulations to help quantify their relative impact on interface material stresses. Figure 1 (above) illustrates a 1/2 symmetric section of a bolted flange connection composed of  multiple materials with varying CTE's. The geometry includes both a thin layer of soft material and a layer of thermal mismatch material with 2.5 times the CTE compared to the Aluminum cover it mates with. Loading conditions include a uniform temperature of 500 degrees F and a Bolt Pre-tension of 500 lbs. for those specified cases where mechanical resistance to separation is needed.

A flow through mesh is used to define both top and bottom interfaces with the soft layer. This soft interface layer thermal mismatch induces mechanical strains, but not significant stresses due to the low stiffness of this material. The bolt head and nut are bonded to the two Aluminum parts, which also induces a local stress concentration that is ignored in this study. The area of investigation in these simulations is the interface between the thermal mismatch material and the lower Aluminum cover plate as illustrated in Figure 1.

Table 1 summarizes nine different simulations comparing nominal and peak stresses as a function of this interface modeling. The bonded and MPC (Cases 1 and 2) do not allow any relative normal or sliding interface displacement.  This would be a quick way to join the components without modeling the bolt, but will likely produce unrealistic stress results at the interface. No separation (Cases 3 through 5) allows relative sliding but no normal separation.  Friction (Cases 6 through 8) allows normal separation when tensile forces overcome the bolt pretension loading and resistance to sliding is governed by the friction coefficient.  Lastly, a rough interface (Case 9) assumes an infinite coefficient of friction but allows  normal separation similar to the friction cases.

Three different stress results are tabulated for the mismatch material: the peak stress including singular stresses that occur with the bonded methods, the nominal stress where the local peak singular stress at the edge of the bond is excluded when applicable, and the peak membrane (average stress through the cross section) stress.  Figures 2 and 3 below illustrate examples of the deformed shape and stress contour results.  Similar patterns are seen in all models.

Table 1 - Demonstration of Connection Modeling Impact on Thermal Stress Analysis of Assemblies

## thermal stress table.png

Figure 2 - Total Displacement Contour Plot (in) - .2 Frictional Interface Representative Case

## thermal stress2.png

Figure 3 - Von Mises Stress Contour Plot (psi) - .2 Frictional Interface Representative Case

## thermal stress3.png

Physical testing is the ideal way to determine the type of connection support, where the interface FEA model could be adjusted to match displacement measurements.  For cases where little or no lateral bond exists, the no separation assumption can develop a similar stress state to the low frictional contact cases, without the added expense of the nonlinear simulation. For the bonded materials of similar stiffness where no relative lateral motion is allowed, local simulations such as the one presented herein and engineering judgment are often needed to develop the best modeling approach based on individuals results requirements, materials, connections and computational resources to determine what stress value to extract from the simulation and apply against the design criterion.

How do you model connections with different CTE's?  I would love to hear how others solve this challenging engineering problem.