A Computational Model for the Thermal Spallation of Crystalline Rocks

Abstract

Thermal spallation is the erosion of brittle materials subjected to high heat fluxes, such as a hot fire in a concrete structure. While experimental investigations provide valuable data on the spallation process, they lack generality to be extrapolated to other materials or loading conditions. This paper presents a numerical method for predicting bulk quantities of the spallation process, such as the average recession rate, for crystalline materials. The method is based on direct numerical simulations of the microstructure. The crystal grains and their boundaries are modeled with finite elements and cohesive zones. These elements have anisotropic and temperature-dependent physical properties, a novel level of fidelity and one that accurately captures known crystal phenomena including the $\alpha$–$\beta$ quartz transition. These models of the crystalline material and the thermal spallation process are validated against experiment results for Barre granite, and then applied to predict the thermal spallation of Martian basalt.

Highlights

• This paper presents a high-fidelity model of a process called thermal spallation.

• Each individual grain within a rock is simulated directly, with material properties that are both temperature- and direction-dependent.

• This computational model reproduces experimental results for Barre granite.

• The model is then used to predict thermal spallation of Martian basalt, which is relevant to landing large robot and human missions on Mars.

Appendix A: Numerical Solution Process

1.1 A.1: 2D Plane Strain Solution

The model presented above is fully 3D; however, modern computers are limited such that a statistically representative volume element would be computationally intractable. The model is instead simplified to 2D plane strain, which is common practice in crack propagation models (Bouchard et al. 2003). The entire process described in this section is extensible to 3D, when computing power becomes available to model an RVE with a statistically significant number of grains.

1.2 A.2: Staggered One-Way Coupling

General solutions to the system of equations defined in Sect. 2.2 cannot be found analytically, so instead they are computed using direct numerical simulation (DNS). The material is discretized into finite elements, with unstructured triangular elements inside the grains and cohesive elements at the grain boundaries.

The equations presented in Sect. 2.2 show that the mechanical PDE is strongly influenced by temperature, but the thermal PDE is weakly influenced by displacement. In addition, mechanical wave propagation in igneous rocks is orders of magnitude higher than temperature propagation, so changes in stress occur nearly instantaneously compared to changes in temperature. Staggering the solution of these two equations avoids using an unnecessary quasi-static approach to solving the mechanical equations. Time is advanced through the thermal simulation, then a static mechanical analysis is performed at the end of each thermal step. A Crank–Nicolson scheme advances time in the thermal simulation, while the mechanical analysis is solving $Ku=F$, as in standard FEM (Pletcher et al. 2012).

The simulations are performed by Abaqus, with a Python manager that prepares input files and processes output files from each time step. The flowchart for the manager is shown in Fig. 19. The two “step” blocks are calls to Abaqus, with the other blocks performed by the manager.

Fig. 19

Staggered thermomechanical simulation of thermal spallation

1.3 A.3: Initialization

At the beginning of the simulation, mesh and job files are created from defined parameters for the run. These parameters include the magnitude of the heat flux, size of the domain, and the properties of the constituent materials. The first step is to run MicroStructPy (Hart and Rimoli 2020a, b), to create a domain with the same composition and grain size distributions as the material being simulated. Cohesive elements are inserted between elements at grain interfaces. A material section is created for each grain, and the material orientations of these sections are sampled from a uniform random distribution:

$$\begin{aligned}{} & {} q' \sim Z + Z i + Z j + Z k \end{aligned}$$

(24)

$$\begin{aligned}{} & {} q = \frac{q'}{||q'||} \end{aligned}$$

(25)

To uniformly sample orientations, the components of a quaternion are sampled from the standard normal distribution, Eq. 24, then the quaternion is normalized to have unit magnitude, Eq. 25 (Marsaglia 1972). An undirected graph of the elements is also generated, which is used in the mechanical post-processing step.

1.4 A.4: Time Advancement in Thermal Analysis

1.4.1 A.4.1: Pre-processor

The thermal pre-processor updates the thermal mesh and heat flux boundary condition. If it is the first step, $i=0$, then there are no updates from the initial mesh and boundary conditions. The nodes, elements, and contact pairs in the thermal mesh are updated with the outputs from the $i-1$ mechanical step. Nodal coordinates are updated with the displacements computed by the mechanical step. Elements are removed from the thermal mesh based on the mechanical post-processor output. When an entire grain is removed, then the contact pairs associated with it are also removed. The thermal job is also updated to reflect changes to the initial and boundary conditions. The initial temperature field of step i is set to the final temperature field of step $i-1$.

1.4.2 A.4.2: Thermal Step

The thermal step takes the job file created by the thermal pre-processor and runs it in Abaqus. The temperature jump conditions in Eq. 6 are implemented with a gap conductance interaction between contact pairs. Since the nodal coordinates were updated by the pre-processor, gaps that are associated with failed cohesive elements do not conduct heat ($\kappa =0$).

The boundary conditions of the thermal model are adiabatic on all sides except the side with an applied heat flux. For example if heat is applied to the $+z$ face of the domain, then the $\pm x$, $\pm y$, and $-z$ faces are all adiabatic. Since many applications are nearly infinite in the $-z$ direction, additional grains must be included in the simulation to avoid numerical artifacts in the simulation results. For the granite simulations below, this ghost layer is four times the average grain size.

The Crank–Nicolson algorithm is used to advance the temperature states in time. It is an unconditionally stable, implicit scheme. The temperature at each node is advanced from timestep i to $i+1$ using central differences at timestep $i+1$ to approximate the gradient in Eq. 1. For grid points on the ends of the mesh, a one-sided finite difference is used instead.

1.4.3 A.4.3: Post-processor

The thermal step results are post-processed after the step completes. The final temperature of each node is used as the initial condition in thermal step $i+1$ and in the thermal strain for mechanical step i, which follows immediately after thermal step i.

1.5 A.5: Static Mechanical Analysis with Temperature Change

1.5.1 A.5.1: Mechanical Pre-processor

Similar to the thermal pre-processor, the mechanical pre-processor updates the mechanical mesh and job file. If $i=0$, no updates are needed and the initial mesh and job are used in the mechanical step. The job file is updating by creating a *RESTART from the $i-1$ mechanical step. Displacement, stress, and damage fields calculated for step $i-1$ are loaded as initial conditions for step i. The initial temperature field for the mechanical job is taken from the end of step $i-1$ and the final temperature field is from the end of step i. These temperatures set the material properties of the grains and their difference results in a thermal strain, $\alpha _{kl} (T-T_0)$. This strain is applied in addition to the strains from the end of step $i-1$.

Since the mechanical steps use the *RESTART option, a new mesh does not need to be created for each step. When spalls are removed from the mesh, *MODEL CHANGE steps are included to remove the elements and contact pairs associated with those spalls.

1.5.2 A.5.2: Mechanical Step

The mechanical step is a static finite element analysis that takes place instantaneously, at the end of step i. The domain is traction-free on the surface where heat is applied, and fixed displacement on the other boundaries. For example, the $\pm x$ faces are fixed in x, $\pm y$ faces are fixed in y, and $-z$ face is fixed in z. The only load applied is the $\Delta T$ at each node in the mesh, representing the change in temperature from the beginning of step i to the end.

The static finite element procedure solves the linear system of equations $Ku=F$. Cohesive elements create additional degrees of freedom and force balancing equations compared to a model with only continuum elements. In this case, additional rows would be inserted into K, with stiffness defined in Eq. 8. Iteration on the static analysis is required, since the displacement field determines the damage state of the cohesive elements, the damage changes the stiffnesses in matrix K, and that matrix is used to solve for the displacements.

As in the thermal step, the $-z$ boundary condition is artificial, imposed to limit the domain to a tractable size. To avoid numerical artifacts in the simulation results, a ghost layer of grains is added to the $-z$ side of the domain. This ghost layer can be multiple grains wide, with the exact number of grains depending on their thermal diffusivity. The grain interfaces in this model are represented by cohesive elements and contact pairs. Abaqus cohesive elements do not enforce contact on their own, so contact is enforced separately with a pressure–overclosure relationship and no softening.

If there are spalls to be removed, *MODEL CHANGE steps are performed before the static finite element analysis. These steps remove the spalls identified at the end of job $i-1$ before performing the job i static step.

1.6 A.6: Spall Identification and Removal

The results from the mechanical step are used to determine if a spall has formed and should be removed from the material. First, the cohesive elements with damage $D\ge 0.8$ are removed from an undirected graph of the mesh elements. This value was chosen as a compromise between accuracy on the dissipated cohesive energy and the ability of DNS models containing damaged cohesive elements to converge. Allowing the damage to reach the value of 1 results in singular stiffness matrices that halt the simulation process. In our experience, the remaining energy under the curve in the TSL is vanishingly small after $D=0.8$ , having minimal effect on the energetics of the problem while allowing the models to converge. It may be the case that not all of the cohesive elements surrounding a spall have failed, for example a single element with $D < 0.8$. This is a numerical feature of DNS, rather than a realistic one, so an additional step is taken to identify and remove these cohesive elements.

Fig. 20

Identification of under-damaged cohesive elements using shortest paths

As shown in Fig. 20, under-damaged cohesive elements are identified by finding the shortest paths between the continuum elements on each side of the fully damaged elements. These shortest paths are computed using the undirected graph, where the vertices of the graph are the elements and the edges are weighted by the distances between element centroids. Inspecting Fig. 20 visually, it is clear which cohesive elements should be removed. The shortest paths approach gives the job manager the ability to algorithmically identify these elements. If the under-damaged cohesive elements represent less than one-third of the total area of cohesive elements removed, then the spall is considered to be topologically separated from the main body. This threshold balances fidelity of the spall formation model with reliability of the DNS to converge to a solution. If the spall fully topologically separates from the main body, those elements become unconstrained and can prevent the solver from finding a converged displacement field.

Topological separation is a necessary, but not sufficient, condition for a spall to be removed from the material. If a grain in the middle of the material were to become topologically separated, it should not be removed, because it has no path away from the main body. To be removable, a spall must also satisfy a geometric condition. As shown in Fig. 21a, the surface attached to the removed cohesive elements has a set of normal vectors, $n_{1-4}$. The mathematical condition that must be true to remove a spall with a given set of normal vectors, N, is that

$$\begin{aligned} \exists \,u \quad n_i\cdot u \ge 0 \quad \forall \,n_i \in N \end{aligned}$$

(26)

The linear system of inequalities $n_i \cdot u \ge 0$ ensures that the pull direction, u, would not cause the spall to collide with the remaining material at any of its boundaries. From the expressions in Eq. 26, it is not immediately clear how to test for the existence of a pull direction, u. An equivalent condition to Eq. 26 is that u exists if N can be contained by a hemisphere. For a given u, the set of points on that sphere that have a positive dot product with u is a hemisphere. In Fig. 21b, the normal vectors are all contained in the $+y$ hemisphere, so this spall can be removed. If, however, there were an $n_5$ that was mostly in the $+x$ direction with a small $-y$ component, the set would still fall within a hemisphere, with a pull direction in the $(+x,+y)$ quadrant. To systematically test for the existence of a pull direction, the convex hull of the set N is taken.

Fig. 21

Spall normal vectors and their convex hull

If the origin is contained within this convex hull, then N spans more than a hemisphere and a pull direction does not exist. On the other hand, if the convex hull does not contain the origin, then the set N spans less than a hemisphere, a pull direction u exists, and the spall is geometrically removable. This approach to testing if a spall can be removed is general for any number of dimensions and does not need to be modified for 3D simulations.

For time steps where multiple potential spalls have formed, the geometric conditions are modified if the spalls shared a grain boundary. If the spall in Fig. 20, for example, had a jagged grain boundary between the two halves, then each half would not have a pull direction. The union of the two halves is removable, but not each half individually. To catch for these cases, the algorithm first tests the unions of neighboring spalls, then tests them individually. If an individual spall is removable, the algorithm iterates to check if other spalls can be removed after that individual has been removed. For example, if the $n_2$ grain boundary extended to divide the spall in Fig. 20 into two individuals, initially the spall on the left would be considered removable and the spall on the right would not. After removing the spall on the left, the spall on the right no longer has that confining surface, so it would be considered removable in the second iteration.

1.7 A.7: Reapplication of the Heat Flux

The heat flux applied to the top of the domain is updated to reflect the changes in nodal coordinates and element removal. The total heat applied to the domain during each thermal step is held constant, so if a surface element stretches or rotates then the heat applied to it must change. To compute the heat flux on each surface element, it is projected onto the plane perpendicular to the direction of the applied heat flux. For example, if heat is applied in the z-direction, each surface element is projected onto the xy plane. Once projected, the job manager checks for overlapping surface elements, then determines which elements to apply the heat flux to using ray-tracing. This ensures that the total heat flux remains constant, and that heat is only applied to those surfaces that are visible to the heat flux. For flame-jet spallation, heat would be applied, wherever the hot gas flows; however, an estimate for that flux value would be inaccurate without CFD.

1.8 A.8: Termination Conditions

After material has been removed from the domain, there is a check to determine if the model should terminate. If the top surface of the domain penetrates the ghost layer, then the model should terminate. This check prevents the domain from becoming small enough that numerical artifacts are introduced into the simulation results.