FEM Solver Handoff

Tensyl computes an equivalent ABD stiffness. A finite-element solver consumes that stiffness through whatever shell-section machinery it provides. Sometimes that machinery is a reduced orthotropic material. Sometimes it is a preintegrated shell stiffness. Sometimes it is a solver-specific section option that benefits from a quick patch check before it joins the serious model.

This page describes practical handoff routes for NX Nastran, ANSYS, and Abaqus. A YAML or JSON artifact from External Workflows is still a useful traceability record: it keeps the stiffness, units, validity warnings, and assumptions together while the solver input gets the particular syntax it needs.

Before Solver Input

Tensyl's canonical generalized strain and resultant order is defined in Equivalent-Stiffness Mechanics. Treat that ordering as part of the data contract, not as a formatting preference.

For solvers that take a six-by-six shell section stiffness, the part to hand off is:

\[ \mathbf K_{ABD} = \begin{bmatrix} \mathbf A & \mathbf B \\ \mathbf B & \mathbf D \end{bmatrix} \]

with row and column order:

\[ (11,\ 22,\ 12,\ k11,\ k22,\ k12). \]

The transverse-shear block is separate:

\[ \mathbf A_s = \begin{bmatrix} A_{s11} & A_{s12} \\ A_{s12} & A_{s22} \end{bmatrix}. \]

Keep these checks explicit:

  • Use one unit system. A and As have force/length units, B has force units, and D has force-length units.
  • Align local solver material axes with Tensyl's e1 and e2. For the built-in Cylinder, e1 is axial and e2 is circumferential.
  • Match the reference surface. Moving the solver section offset without shifting the ABD stiffness changes B.
  • Preserve the engineering shear and engineering twist convention.
  • Review result.validity.warnings before export. The solver sees stiffness numbers; the validity context has to travel with the model.

When a solver card, spreadsheet, or hand equation wants scalar terms, use the named coefficient view instead of indexing matrices throughout the export code:

coefficients = result.coefficients

print(coefficients.A11, coefficients.B12, coefficients.D66, coefficients.As22)

Reduced Orthotropic Properties

The simplest route is to convert the membrane block to equivalent orthotropic plane-stress constants and let the solver build a conventional shell section. This is useful for preliminary modal, static, or sizing models when the ABD stiffness is nearly uncoupled.

Choose an effective shell thickness t_eff. In this context, t_eff is the thickness that the downstream shell property will use with the reduced material constants. It is the bookkeeping thickness for the solver handoff, not something Tensyl can discover from the ABD matrix alone.

The reduction forms:

\[ \mathbf Q_\mathrm{eff} = \frac{\mathbf A}{t_\mathrm{eff}}, \qquad \mathbf S_\mathrm{eff} = \mathbf Q_\mathrm{eff}^{-1}. \]

For local axes aligned with the orthotropic axes:

\[ E_1 = \frac{1}{S_{11}}, \quad E_2 = \frac{1}{S_{22}}, \quad G_{12} = \frac{1}{S_{66}}, \quad \nu_{12} = -\frac{S_{12}}{S_{11}}, \quad \nu_{21} = -\frac{S_{12}}{S_{22}}. \]

What the reduced route keeps

This preserves the chosen membrane compliance. It does not generally preserve the bending block, eccentric stiffener coupling, or transverse-shear stiffness. If those are carrying the physics, use a richer workflow.

Use the reduced route when the terms it discards are intentionally negligible:

  • membrane-bending coupling B;
  • off-axis membrane coupling A16 and A26;
  • off-axis bending coupling D16 and D26;
  • transverse shear details if the chosen shell element computes them from the material and thickness.
props = result.reduced_orthotropic_properties(t_eff=0.080)

print(props.E1, props.E2, props.G12, props.nu12)
print(props.warnings)

Common t_eff choices are:

  • the physical skin or laminate thickness when the model is skin-dominated;
  • the total smeared structural depth for a coarse stiffened-shell study;
  • a project-defined shell property thickness chosen to match mass, stress-output, or legacy model conventions.

Changing t_eff changes the reported E1, E2, and G12, but the membrane reduction stays consistent because A = Q_eff * t_eff. Just keep a record of which thickness the reduction used.

NX Nastran

For NX Nastran, the most common handoff is through ordinary Bulk Data shell properties and materials. The examples below use NX Nastran-style MAT8, PSHELL, and laminate-property workflows. Check the installed Siemens NX Nastran Quick Reference Guide for the exact field definitions used by your solver release.

Simple Route: MAT8 and PSHELL

For an uncoupled equivalent orthotropic stiffness:

  1. Use result.reduced_orthotropic_properties(t_eff=...) to obtain E1, E2, G12, and nu12.
  2. Define a MAT8 with those in-plane constants.
  3. Define a PSHELL with thickness t_eff, using the MAT8 as the membrane and bending material.
  4. Use element material-angle fields or coordinate systems so material direction 1 matches Tensyl e1.

This route is easy to inspect and works well when the equivalent stiffness is close to a conventional orthotropic shell.

$ Illustrative NX Nastran-style Bulk Data fragment.
MAT8, 101, E1, E2, NU12, G12, G1Z, G2Z, RHO
PSHELL, 201, 101, T_EFF, 101

Use PCOMP or PCOMPG instead when the equivalent stiffness is better represented as a laminate stack and you want the solver to integrate ply stiffnesses. An unsymmetric laminate can produce membrane-bending coupling, but it is still a laminate model, not an arbitrary ABD matrix fit.

Good first model

MAT8 plus PSHELL is a useful first model when membrane behavior is the main target. It is not meant to preserve every term of a general stiffened ABD matrix.

Higher Fidelity: PSHELL Material References

The PSHELL card has separate material references for membrane, bending, transverse shear, and membrane-bending coupling through MID1, MID2, MID3, and MID4. That lines up nicely with the way Tensyl reports A, D, As, and B, but the card fields still carry NX Nastran's shell-property scaling rules.

Use this path when you have verified the mapping for the NX Nastran solution sequence and element family you plan to use:

  1. Decide whether MAT2 or MAT8 is the right material card for each block.
  2. Account for PSHELL thickness and bending-inertia factors, including 12I/T**3, and any transverse-shear factors.
  3. Print or recover the element section stiffness from NX Nastran when that output is available.
  4. Run a one-element patch model with imposed membrane strains and curvatures, then compare recovered resultants with K_ABD @ eta.

Verify the section stiffness

MID1 through MID4 can be a useful high-fidelity path, but it is not a universal "paste the ABD matrix here" slot. If the recovered section stiffness does not match the Tensyl matrix within the tolerance needed for the analysis, keep the NX Nastran model reduced and document the approximation.

ANSYS

ANSYS Mechanical APDL has a direct preintegrated shell-section path. The current command reference lists SECTYPE,,GENS as a preintegrated general shell section and identifies SSPA, SSPB, SSPD, and SSPE as the follow-on commands for membrane, coupling, bending, and transverse shear. The command field layouts are:

Tensyl block ANSYS command Field order
A SSPA A11, A12, A16, A22, A26, A66, T
B SSPB B11, B12, B16, B22, B26, B66, T
D SSPD D11, D12, D16, D22, D26, D66, T
As SSPE As11, As12, As22, T

The first six stiffness fields are the lower symmetric half of each three-by-three block, taken column by column: (1,1), (2,1), (6,1), (2,2), (6,2), (6,6), written here with Tensyl's engineering index 6 for the in-plane shear/twist component. SSPB also accepts three optional off-diagonal fields for a non-symmetric coupling block; Tensyl's B is symmetric, so those repeat the lower terms and can be omitted unless the solver workflow specifically asks for them.

! Illustrative APDL fragment.
SECTYPE, 10, GENS, , TENSYL_WALL
SSPA, A11, A12, A16, A22, A26, A66, T_REF
SSPB, B11, B12, B16, B22, B26, B66, T_REF
SSPD, D11, D12, D16, D22, D26, D66, T_REF
SSPE, AS11, AS12, AS22, T_REF
SECNUM, 10

Use T_REF as the nominal section thickness required by the solver command syntax and stress-output workflow. The preintegrated stiffness terms still need to be entered with their actual integrated units.

For a reduced workflow, define an orthotropic material with MP/TB data and a normal shell section thickness. That route is easier to inspect in Mechanical, but it inherits the same limitations as the reduced-property method above.

Abaqus

Abaqus has two relevant routes:

  • material-based shell sections for reduced orthotropic workflows;
  • direct general shell sections for full linear section stiffness.

For the direct route, omit MATERIAL, COMPOSITE, and USER on *SHELL GENERAL SECTION. Abaqus then reads the symmetric half of the six-by-six section stiffness matrix, 21 entries total, eight entries on each of the first two lines and five on the third line. Abaqus also accepts an ORIENTATION parameter, which should align section direction 1 with Tensyl e1.

Pack:

\[ \mathbf K = \begin{bmatrix} A_{11} & A_{12} & A_{16} & B_{11} & B_{12} & B_{16} \\ A_{12} & A_{22} & A_{26} & B_{12} & B_{22} & B_{26} \\ A_{16} & A_{26} & A_{66} & B_{16} & B_{26} & B_{66} \\ B_{11} & B_{12} & B_{16} & D_{11} & D_{12} & D_{16} \\ B_{12} & B_{22} & B_{26} & D_{12} & D_{22} & D_{26} \\ B_{16} & B_{26} & B_{66} & D_{16} & D_{26} & D_{66} \end{bmatrix}. \]

The data order is:

K11, K12, K22, K13, K23, K33, K14, K24,
K34, K44, K15, K25, K35, K45, K55, K16,
K26, K36, K46, K56, K66

An illustrative input fragment:

*SHELL GENERAL SECTION, ELSET=panel, ORIENTATION=tensyl_axes, DENSITY=rho_area
A11, A12, A22, A16, A26, A66, B11, B12
B16, D11, B12, B22, B26, D12, D22, B16
B26, B66, D16, D26, D66
*TRANSVERSE SHEAR STIFFNESS
AS11, AS22, AS12

The transverse shear line is separate. Abaqus documents *TRANSVERSE SHEAR STIFFNESS as a shell-compatible option with first-direction stiffness, second-direction stiffness, and coupling term fields.

For a reduced workflow, define an engineering-constants material and use *SHELL SECTION or a material-based *SHELL GENERAL SECTION. That is convenient when B = 0 and the ABD stiffness behaves like a conventional orthotropic shell. It is not a substitute for the direct 21-entry stiffness when stiffener eccentricity coupling matters.

Patch Check

Before using a translated stiffness in a production model, run a one-element check in the target solver:

  1. Use one shell element with the intended section, orientation, offset, and units.
  2. Impose a pure epsilon11, epsilon22, gamma12, kappa11, kappa22, and kappa12 case, one at a time if the solver setup allows it.
  3. Compare solver-reported section forces and moments with:

$\(\mathbf r_{ABD} = \mathbf K_{ABD}\boldsymbol\eta_{ABD}.\)$

  1. For transverse shear flexible elements, apply independent shear checks against As.

Small model, large leverage

The patch check catches axis swaps, offset mistakes, solver-specific scaling, and the occasional perfectly formatted wrong number. A single element is cheap; a bad coordinate system can get expensive.

Next: SP-8007 Data Handoff.

References