# Simulation of Rock Failure Cone Development Using a Modified Load-Transferring Anchor Design
## 2 Materials and Methods
### Model Geometry, Finite Element Mesh, and Boundary Conditions
This type of connector element includes two nodes (A and B, see Figure 10) whose relative distance can be prescribed and controlled during the simulation. This configuration allows for relative displacement between the two selected nodes of the model exclusively along a predefined axis--in this case, the Y-axis (as shown in Figure 10b)--while rotational degrees of freedom are restricted. By associating at least two points from each of the relevant components of the anchor model (i.e., the tip of the drive screw and the conical anchor head) with the respective nodes of the connector, it becomes possible to simulate the progressive change in distance between the front face of the anchor head and the end of the screw along the screw axis (the axis of symmetry of the model), as illustrated in Figure 10b. Figure 9: Geometry of the rock mass model with an undercut borehole for anchor installation. This procedure effectively enables the implementation of kinematic loading in the finite element model through the use of the defined axial connector. A total connector elongation of \(\Delta\)Y = 10 mm was assumed, in accordance with Figure 8. The elongation was applied iteratively, beginning with an initial incremental step of 0.01 mm, which was subsequently increased until the maximum value was reached while maintaining the numerical convergence of the solution. In the region where the tip of the drive screw contacts the borehole bottom, as well as in the interaction zone between the conical head and the rock, frictional contact was defined using the \"Penalty contact\" formulation available in ABAQUS. The coefficient of friction (\(\mu\)) for the steel-rock interface was set to 0.2, representing an average value typically adopted in this type of simulation. The boundary conditions applied to the model's external nodes are illustrated in Figure 10a, where U denotes translational degrees of freedom and UR denotes rotational degrees of freedom. The constraints were defined as follows:  
Right edge: U1 = 0, allowing displacement only along the Y-axis (vertical direction);  
Bottom edge: U2 = 0, allowing displacement only along the X-axis (horizontal direction);  
Left edge of the rock domain, left edge of the screw, and connector nodes: U1 = U3 = UR2 = 0, permitting linear displacement only along the Y-axis, enforcing axisymmetry with respect to the model's central axis. The model was discretized using 4-node axisymmetric finite elements of type CAX4R (continuum, axisymmetric, 4-node, reduced integration), generating the finite element mesh shown in Figure 11. This meshing strategy ensured an efficient balance between computational cost and the accuracy required for stress concentration and fracture prediction in the critical zones. In critical regions of the model, a non-uniform mesh density was applied by using the automatic mesh generator available in ABAQUS, with manually assigned element seed sizes in selected zones. As a result, the global element size (edge length) was set to 25 mm, while local mesh refinement was implemented in regions of expected high stress gradients and contact interactions as follows:  
* In the contact area between the conical anchor head and the rock, the element size was reduced to 2 mm;  
Figure 10: Boundary constraints of the model (**a**); modeling of the connection between the anchor head and the drive screw using an axial connector (**b**). Representation of the movable linkage between anchor components in ABAQUS: A and B—nodes of the linear connector. * In the contact zone between the screw tip and the borehole bottom, a finer mesh was used with element sizes ranging from 0.4 mm to 1 mm;
* Along the predicted crack propagation path, the element size was refined to 5 mm to enhance the resolution of fracture development;
* Along the upper edge of the rock mass, the element size varied between 3 mm and 10 mm, depending on the specific subregion of the rock domain.