Abaqus migration
================

If your starting point is an Abaqus ``.inp`` deck (Standard
or Explicit), this page is the bridge into femorph-solver.
The mapping is mostly mechanical — the keyword vocabulary is
distinctive but every concept has a direct counterpart.

For the one-table cheat-sheet, see :doc:`terminology`.  For
the full keyword-by-keyword coverage, keep going.

Loading an INP deck
-------------------

Single call (``from_inp``) reads the keyword-style deck and
returns a :class:`~femorph_solver.Model` ready to assemble::

    from femorph_solver.interop.abaqus import from_inp

    model = from_inp("rotor.inp")
    model.fix(nodes=clamped_nodes, dof="ALL")
    result = model.solve_static()

The reader handles Abaqus 6.14+ standard / explicit decks
written through ``*HEADING`` / ``*NODE`` / ``*ELEMENT`` /
``*MATERIAL`` / ``*BOUNDARY`` / ``*CLOAD`` / ``*STEP`` blocks.
Decks generated through Abaqus/CAE export, abaqus2matlab, and
the ``abaqus`` Python scripting API all parse cleanly.

What's read
-----------

The reader covers the linear-elastic structural-mechanics
slice femorph-solver supports today.  Element types — the
core mapping table:

==========================  ============================================
Abaqus element type          Maps to femorph-solver
==========================  ============================================
``C3D8``                     ``ELEMENTS.HEX8`` (plain Gauss)
``C3D8R``                    ``ELEMENTS.HEX8`` (reduced — same kernel today)
``C3D8H``                    ``ELEMENTS.HEX8`` (hybrid → plain HEX8)
``C3D8I``                    ``ELEMENTS.HEX8(integration="enhanced_strain")`` — Simo-Rifai EAS
``C3D20`` / ``C3D20R``       ``ELEMENTS.HEX20``
``C3D10`` / ``C3D10M``       ``ELEMENTS.TET10``
``C3D15``                    ``ELEMENTS.WEDGE15`` (degenerate HEX20)
``S4`` / ``S4R``             ``ELEMENTS.QUAD4_SHELL`` (Mindlin-Reissner)
``B31``                      ``ELEMENTS.BEAM2`` (Bernoulli)
``T3D2``                     ``ELEMENTS.TRUSS2`` (axial bar)
``CPS4`` / ``CPS4R``         ``ELEMENTS.QUAD4_PLANE`` plane-stress
``CPE4`` / ``CPE4R``         ``ELEMENTS.QUAD4_PLANE`` plane-strain (BC sets the regime)
``MASS``                     ``ELEMENTS.POINT_MASS``
``SPRING2`` / ``SPRINGA``    ``ELEMENTS.SPRING``
==========================  ============================================

Keyword blocks the reader processes:

========================================  ============================================
Abaqus keyword                              Effect on the Model
========================================  ============================================
``*NODE``                                   Grid points + global coordinates
``*ELEMENT, TYPE=...``                      Element connectivity (cell type chosen via the table above)
``*ELSET`` / ``*NSET``                      Named sets used for BC / load assignment
``*MATERIAL`` + ``*ELASTIC``                Isotropic material (E + nu, plus optional rho)
``*DENSITY``                                Material density on the in-progress material
``*ELASTIC, type=ENGINEERING_CONSTANTS``    Orthotropic material (full 9-constant form)
``*SOLID SECTION``                          Property → element-set binding for solids
``*SHELL SECTION``                          Shell thickness + property binding
``*BEAM SECTION``                           Beam cross-section + property binding
``*BOUNDARY``                               :meth:`Model.fix` per pinned DOF
``*BOUNDARY, ENCASTRE``                     Equivalent to ``Model.fix(dof="ALL")``
``*BOUNDARY, XSYMM``                        Symmetry plane normal to x (and Y / Z analogues)
``*CLOAD``                                  :meth:`Model.apply_force` (translational + rotational components)
``*DLOAD, P``                               Distributed surface pressure
``*DLOAD, GRAV``                            Gravity body force
``*DSLOAD``                                 Distributed surface load (vector form)
``*MPC``                                    Multi-point constraint (cyclic-symmetry only at present)
``*STEP`` / ``*END STEP``                   Step boundary — first step processed; multi-step decks warn on the rest
========================================  ============================================

What's flagged but not read
---------------------------

The reader emits a warning and skips:

- ``C3D8R, ELEMENT_TECHNIQUE=ENHANCED`` — Abaqus's
  enhanced-hourglass-control flavour.  Closest equivalent is
  ``C3D8I`` which we map to HEX8-EAS already.
- ``C3D6`` (linear wedge), ``C3D4`` (linear tet), and
  composite ``S8R`` — not yet shipped.
- ``CONN3D2`` connector elements — connector library is on
  the planned roadmap.
- ``*PLASTIC``, ``*HYPERELASTIC``, ``*VISCOELASTIC`` —
  non-linear material cards.  Linear elastic only at present.
- ``*INITIAL CONDITIONS`` — pre-stress / temperature initial
  state needs the planned thermal-stress workflow.
- ``*RESTART`` / ``*OUTPUT`` — output-control directives.
  We always emit the canonical ``.pv`` file via
  ``StaticResult.save``.
- Multi-step ``*STEP`` blocks beyond the first — handle as
  separate ``Model`` instances.

Procedure / step types
----------------------

Abaqus declares the analysis type via the ``*STEP`` block's
procedure keyword.  The reader is geometry + BC + load
focused — it ignores the procedure keyword and lets you pick
the analysis type via the ``Model`` API:

==============================  ============================================
Abaqus procedure                 femorph-solver call
==============================  ============================================
``*STATIC``                      :meth:`Model.solve_static`
``*FREQUENCY``                   :meth:`Model.solve_modal`
``*BUCKLE``                      not yet shipped (planned)
``*STEADY STATE DYNAMICS``       :meth:`Model.solve_harmonic`
``*DYNAMIC, IMPLICIT``           :meth:`Model.solve_transient`
``*DYNAMIC, EXPLICIT``           not shipped (explicit dynamics planned)
``*MODAL DYNAMIC``               :meth:`Model.solve_transient` (mode-superposition mode)
==============================  ============================================

This separation lets the same geometry serve multiple
analysis types without re-parsing the deck.

Result-format readback
----------------------

The reader is INP-only.  Reading Abaqus ``.odb`` output isn't
currently supported — the binary format is proprietary and
the documented Python API requires a paid Abaqus license to
import the libraries it depends on.  An NPZ-format converter
``odb_npz`` is shipped in
:mod:`femorph_solver.interop.abaqus._odb_npz` for users who
exported their ODB through the Abaqus Python API to NPZ; the
recommended workflow is to solve through femorph-solver and
export to ``.pv``::

    from femorph_solver.interop.abaqus import from_inp

    model = from_inp("model.inp")
    result = model.solve_static()
    result.save("model.pv", model)

Edge cases worth flagging
-------------------------

**DOF ordering.**  Abaqus orders DOFs as ``(U1, U2, U3, R1,
R2, R3)`` — same content as femorph-solver's ``(UX, UY, UZ,
ROTX, ROTY, ROTZ)``, just renamed.  No re-mapping needed.

**Free-form vs fixed.**  Abaqus INP is comma-separated
free-form throughout; the reader handles arbitrary whitespace.

**Comment cards** (``**``).  Stripped silently.

**Continuation lines** (lines ending in trailing comma).
Joined transparently.

**Set references by name** (``ELSET=mybolts`` /
``NSET=clamp``).  Resolved against the deck's named-set
definitions — out-of-order references work because the
reader does two passes.

**Local coordinate systems** (``*ORIENTATION``).  Read but
currently warned-and-skipped — every field is interpreted in
the global Cartesian frame.  Local-coordinate support is on
the planned roadmap.

**Step amplitude curves** (``*AMPLITUDE``).  Static decks
parse them but the amplitude is currently applied as the
deck's reference value; time-varying load tables need the
transient solver's amplitude binding (planned).

Concrete migration recipe
-------------------------

For a typical static-analysis deck:

.. code-block:: python

    from femorph_solver.interop.abaqus import from_inp

    # 1. Load the deck.  All the *NODE / *ELEMENT /
    #    *MATERIAL / *BOUNDARY / *CLOAD blocks above
    #    populate the Model.
    model = from_inp("aircraft_panel.inp")

    # 2. Optionally inspect or modify:
    print(f"{model.grid.n_points} nodes, {model.grid.n_cells} cells")

    # 3. Solve.
    result = model.solve_static()

    # 4. Export to canonical ``.pv`` for downstream
    #    post-processing in the femorph-solver gallery
    #    recipes (:doc:`/gallery/post-processing/index`).
    result.save("aircraft_panel.pv", model)

    # 5. Stress recovery + design check follow the
    #    standard recipes — same code regardless of which
    #    deck you started from:
    from femorph_solver.recover import compute_nodal_stress, stress_invariants
    sigma = compute_nodal_stress(model, result.displacement.ravel())
    inv = stress_invariants(sigma)
    print(f"Peak σ_VM = {inv['von_mises'].max() / 1e6:.2f} MPa")

Cross-references
----------------

- :doc:`terminology` — the one-table Rosetta covering every
  concept across femorph-solver / MAPDL / NASTRAN / Abaqus /
  LS-DYNA.
- :doc:`nastran` — the NASTRAN equivalent of this page.
- :doc:`/getting-started/mapdl-interop` — the MAPDL
  equivalent.
- :doc:`/reference/elements/index` — per-element technical
  sheets, each carrying a cross-vendor mapping table that
  starts from the femorph-solver name and lists the Abaqus
  element type.