| Command | Explanation |
| Input Module Configuration | |
Input.modules = [ "input", "nodeInput" ]; | define the input modules: "input" for geometry reading and "nodeInput" for node group creation |
| Geometry Input Settings | |
Input.input.type = "GMSHInput"; | specify that the input module is a GMSHInputModule |
Input.input.verbose = false; | suppress some outputs |
Input.input.store_tangents = true; | additionally store the tangent direction of each rod segment at the nodes, needed to construct the initial (curved) rod kinematics |
Input.input.onelab.Rotation = "180"; | set the GMSH onelab parameter Rotation (rotates the whole structure by 180°) |
Input.input.onelab.BaseWidth="0.0083"; | set the honeycomb's base bar width \(b=.3\)mm |
Input.input.onelab.LengthRatio="0.5883253012048192"; | set the ratio between the two bar lengths of the re-entrant unit cell |
Input.input.onelab.Angle="55"; | set the re-entrant angle between the two bars to 55° |
Input.input.onelab.Thickness="0.00075"; | set the (unused by the .geo file directly, but referenced for context) wall thickness to 0.75mm |
Input.input.onelab.RepX="3"; | tile the unit cell 6 times in the horizontal (x) direction |
Input.input.onelab.RepY="2"; | tile the unit cell 4 times in the vertical (y) direction |
Input.input.onelab.Scale="4.0"; | apply a scaling factor of 4 to recover the original size from the paper |
Input.input.file="tests/docs/re-entrant.geo"; | set the geometry file path |
| Node Group Definition | |
Input.nodeInput.type = "PBCGroupInput"; | use PBCGroupInputModule instead of the plain GroupInputModule from Properties for Example 1, which additionally derives the boundary node groups (xmin, xmax, ymin, ymax, and the corner nodes) needed to apply periodic boundary conditions |
Input.nodeInput.groupSettings.restrictToGroup = "points"; | only consider the original GMSH geometry points (not intermediate/duplicated nodes) when constructing these boundary groups |
Input.nodeInput.ymax.xbounds=["ORIGIN.X+SIZE.X/2-SIZE.X/6","ORIGIN.X+SIZE.X/2+SIZE.X/6"]; | narrow the default "ymax" (top edge) group down to its central third, matching the finite width of the physical impactor |
Input.nodeInput.ymax.restrictToGroup = "beams"; | loosen the restriction for the narrowed "ymax" group to all nodes that belong to the lattice ("beams") |
| Command | Explanation |
| Model Structure | |
model.type = "Matrix"; | define the top-level model type as MatrixModel |
model.model.type = "Multi"; | specify that the model contains multiple sub-models (MultiModel) |
model.model.models = [ "lattice", "load", "fixed" ]; | define three sub-models: the lattice itself, the loading/support conditions, and additional (planar) constraints |
| Lattice / Material Configuration | |
model.model.lattice.type = "Lattice"; | as in Properties for Example 1, use a LatticeModel to assemble many individual rods into one model |
model.model.lattice.prefix = "beam_"; | prefix used for the individual rod element names |
model.model.lattice.child.type = 'specialCosseratRod"; | each rod in the lattice is again a SpecialCosseratRodModel |
model.model.lattice.child.dofNamesTrans = ["dx", "dy", "dz"]; | translational degrees of freedom |
model.model.lattice.child.dofNamesRot = ["rx", "ry", "rz"]; | rotational degrees of freedom |
model.model.lattice.child.material_ey = [ 0., 0., 1. ]; | set the rod's local cross-section "up" direction, needed to orient the (non-circular) rectangular cross-section |
model.model.lattice.child.material.type="ElastoPlasticRod"; | unlike Test 1's purely elastic rod, use the elasto-plastic rod material to capture plastic hinge formation |
model.model.lattice.child.material.cross_section = "rectangle"; | rectangular cross-section |
model.model.lattice.child.material.side_length=[0.00075, 0.00075]; | 0.75mm × 0.75mm cross-section |
model.model.lattice.child.material.young = 210e9; | steel Young's modulus, \(210\)GPa |
model.model.lattice.child.material.poisson_ratio=0.265; | steel Poisson's ratio |
model.model.lattice.child.material.density=8000.; | steel density, \(8000\) kg/m³ |
model.model.lattice.child.material.yieldCond = "..."; | define the (multi-axial) yield surface, fitted so its yield strength matches a macroscopic 280 MPa yield strength scaled from a microscopic J2 value of 450 MPa and the rod's cross-section |
model.model.lattice.child.material.kinematicTensor = [...]; | define the 6×6 kinematic-hardening modulus tensor, scaled from a reference hardening modulus of 20 GPa down to the 1.75 GPa hardening modulus fitted to the Johnson-Cook material model used experimentally |
model.model.lattice.child.material.edge_factor = 1.25; | increase the rod's effective bending stiffness by 25% to account for the stiffening effect of the physical joints connecting the rods |
| Self-Contact | |
model.model.lattice.contact.type = "RodContact"; | enable rod-on-rod self-contact, since the re-entrant cells touch each other once sufficiently compacted |
model.model.lattice.contact.radius=0.000375; | contact radius, matching the rod's half cross-section side length |
model.model.lattice.contact.penaltySTS=56250.0; | segment-to-segment contact penalty stiffness |
model.model.lattice.contact.penaltyNTS=562500.0; | node-to-segment contact penalty stiffness |
model.model.lattice.jointContact.type = "JointContact"; | additionally enable contact between the rod joints themselves |
model.model.lattice.jointContact.radius=0.0005; | joint contact radius |
model.model.lattice.jointContact.penalty=5625000.0; | joint contact penalty stiffness |
| Loading and Support | |
model.model.load.type = "Multi"; | bundle the impact and support related sub-models together |
model.model.load.models=["fix_dynamic","impact","init","top_bottom_mass"]; | define the four loading sub-models |
model.model.load.fix_dynamic.type = "Dirichlet"; | guide the top and bottom edges so they can only move vertically |
model.model.load.fix_dynamic.nodeGroups = [ "ymin", "ymax", "ymax" ]; | apply this to the "ymin" and "ymax" edges |
model.model.load.fix_dynamic.dofs = [ "rz", "dx", "rz" ]; | constrain the bottom edge's rotation and the top edge's horizontal displacement and rotation |
model.model.load.fix_dynamic.factors = [ 0., 0., 0. ]; | all three constraints are homogeneous (zero) |
model.model.load.init.type = "InitLoad"; | InitLoadModel, used to set the impactor's initial velocity |
model.model.load.init.veloGroups = "ymax"; | apply the initial velocity to the top ("ymax", impactor) group |
model.model.load.init.veloDofs = "dy"; | in the vertical direction |
model.model.load.init.veloVals="-1*70.0"; | initial impact velocity of \(70\)m/s, directed downward |
model.model.load.impact.type = "ImpactBC"; | ImpactModel, used to give the impactor a finite effective mass so it decelerates realistically under the lattice's resistance |
model.model.load.impact.nodeGroups = "ymax"; | applies to the impactor group |
model.model.load.impact.dofs = "dy"; | in the vertical direction |
model.model.load.impact.weights = "1.2 / 25 * 0.75"; | (fraction of the) impactor mass |
model.model.load.top_bottom_mass.type = "Mass"; | add an additional lumped mass representing the striker plate's inertia |
model.model.load.top_bottom_mass.nodeGroups = ["ymax"]; | attached to the impactor group |
model.model.load.top_bottom_mass.totalMass = ["0.1308/25*0.75"]; | total mass distributed over that group |
model.model.load.top_bottom_mass.dofs = ["dx", "dy", "dz"]; | mass acts equally in all three translational directions |
| Additional Planar Constraints | |
model.model.fixed.type = "Dirichlet"; | keep the whole lattice planar |
model.model.fixed.nodeGroups = [ "all", "all", "all" ]; | applies to every node |
model.model.fixed.dofs = ["dz", "rx", "ry"]; | constrain out-of-plane translation and the two in-plane bending rotations |
model.model.fixed.dispIncr = 0.; | homogeneous (zero) constraint |
| Compliant Support Plate | |
model.model.models += "plate_springs"; | add a further sub-model representing the support plate |
model.model.plate_springs.type = 'springMass"; | SpringMassModel, used to model the compliant support as a small elastic rod rather than a rigid boundary |
model.model.plate_springs.boundary = "ymin"; | attach the spring to the bottom ("ymin") edge |
model.model.plate_springs.springs = [ "plate1"]; | define a single named spring, "plate1" |
model.model.plate_springs.plate1.extentVector = [ 0., -0.01, 0.]; | the spring rod extends 10mm further downward from the lattice's base |
model.model.plate_springs.plate1.nElem = 4; | discretize the spring rod into 4 elements |
model.model.plate_springs.plate1.pElem = 1; | use linear (order 1) elements for the spring rod |
model.model.plate_springs.plate1.type = 'specialCosseratRod"; | the spring itself is again a SpecialCosseratRodModel |
model.model.plate_springs.plate1.dofNamesTrans = [ "dx", "dy", "dz" ]; | translational degrees of freedom |
model.model.plate_springs.plate1.dofNamesRot = [ "rx", "ry", "rz" ]; | rotational degrees of freedom |
model.model.plate_springs.plate1.material_ey = [0., 0., 1.]; | cross-section orientation |
model.model.plate_springs.plate1.material = "ElasticRod" { ... }; | a purely elastic rod representing a steel plate, \(0.18\)m wide and 0.75mm thick, used to give the support a realistic, finite stiffness rather than being perfectly rigid |
| Command | Explanation |
| Logging Configuration | |
log.pattern = "*.info"; | only log "info"-level messages |
log.file="$(CASE_NAME)/run.log"; | write the log to a file next to the case's other outputs |
| Output Module Configuration | |
Output.modules = ["groupOut", 'sampling", "paraview"]; | define three output modules: group averaging, CSV sampling, and ParaView visualization |
Output.groupOut.type = "GroupOutput"; | GroupOutputModule, used to compute averaged group quantities used below |
Output.groupOut.nodeGroups = ["ymax", "ymin", "plate1_bot"]; | track the impactor, the base of the lattice, and the bottom of the support spring |
Output.groupOut.dofs = "dy"; | in the vertical direction |
| CSV Output Configuration | |
Output.sampling.type = 'sample"; | SampleModule, used to write a CSV time history |
Output.sampling.file = "$(CASE_NAME)/data.csv"; | output file path |
Output.sampling.header="..."; | descriptive column header for the CSV file: time, impactor velocity/displacement/force, base force, nominal strain, top/bottom pressure, potential/dissipated/kinetic energy, mass, support-plate force |
Output.sampling.dataSets=[...]; | the corresponding data expressions: t, ymax.velo.dy, ymax.disp.dy, ymax.resp.dy, ymin.resp.dy, the nominal compaction ymax.disp.dy/SIZE.Y, the top/bottom pressures (force divided by the lattice's cross-sectional area), potentialEnergy, dissipatedEnergy, kineticEnergy, mass, and the support-plate force plate1_bot.resp.dy |
Output.sampling.separator = ","; | comma-separated output |
| ParaView Visualization Output | |
Output.paraview.type = "ParaView"; | ParaViewModule visualization output, as in Properties for Example 1 |
Output.paraview.groups = [ "beams","plate1" ]; | output both the lattice ("beams") and the support spring ("plate1") |
Output.paraview.beams.disps = ["dx", "dy", "dz"]; | translational displacement fields |
Output.paraview.beams.otherDofs = ["rx", "ry", "rz"]; | rotational degree of freedom fields |
Output.paraview.beams.el_data = [ "mat_strain", "mat_stress", "plast_strain" ]; | element data: material strain, stress, and (unlike Test 1) accumulated plastic strain |
Output.paraview.beams.node_data = ["fres", "F_contact", "kineticEnergy", "mass"]; | node data: residual force, contact force, kinetic energy and mass |
Output.paraview.beams.shape = "Line2"; | visualize the (linear) rod elements as 2-node line segments |
Output.paraview.plate1 = Output.paraview.beams; | re-use the same settings for the support spring group ... |
Output.paraview.plate1.el_data = [ "mat_strain", "mat_stress" ]; | ... except for element data, since the spring is purely elastic (no plastic strain) |
Output.paraview.plate1.node_data = ["fres"]; | ... and node data, since it carries no contact or lumped mass |
Output.paraview.output_format = "$(CASE_NAME)/vis%i"; | output file naming pattern |
Output.paraview.sampleWhen = "(Output.paraview.sampleInfo-Output.paraview.oldSampleInfo > 0.002) OR (i<=1)"; | write a ParaView frame every 1% strain |
Output.paraview.sampleInfo="abs(ymax.disp.dy/SIZE.Y)"; | define strain measure for Output |
