Theory & verification

What the analysis represents

The program models a planar frame as straight, prismatic, line elements joined at nodes. Each node has three global degrees of freedom:

Members use linear-elastic material behavior and small-displacement kinematics. Each member can have its own Young’s modulus E, shear modulus G, area A, second moment of area I, and effective shear area A_v. The steel section database supplies the in-plane area and inertia for its profiles; concrete input is currently a rectangular gross section for elastic analysis.

Frame element stiffness

The backend builds a two-node, six-degree-of-freedom local stiffness matrix. Its axial block is the standard bar stiffness; bending couples the two transverse translations and end rotations.

Local stiffness matrix in matrix form

Using local degree-of-freedom order \(\mathbf d_l=[u_1,v_1,\theta_1,u_2,v_2,\theta_2]^T\), the assembled element matrix is:

The bending coefficients include shear flexibility when enabled:

Coordinate transformation

For member angle \(\alpha\), with \(c=\cos\alpha\), \(s=\sin\alpha\), transform the local matrix using \(\mathbf{k}_g=\mathbf{T}^T\mathbf{k}_l\mathbf{T}\):

Euler–Bernoulli option: shear deformation off

When shear deformation is disabled, φ is set to zero. The standard bending stiffness coefficients are recovered:

Timoshenko option: shear deformation on

When it is enabled, the bending coefficients are modified using the shear-flexibility parameter:

This is a shear-flexible two-node frame element. For a slender member φ tends to zero and the response approaches the Euler–Bernoulli result. Rolled I/H sections use an effective web shear area derived from section dimensions; manual and rectangular concrete sections default to 5A/6 and can use the member-table value.

Coordinates, releases, and global solve

1. Local axes. For each member, its end coordinates define length L and direction cosines c and s. A transformation matrix converts nodal displacements and actions between global and local axes.
2. Global stiffness. Each member matrix is transformed as K_e = T^T k_e T and added into the global rows and columns corresponding to its two nodes.
3. End releases. A released member-end rotation is eliminated by static condensation. For active and released coordinates, the reduced stiffness is K_aa − K_arK_rr⁻¹K_ra. The compatible member load is condensed as well.
4. Supports. Prescribed degrees of freedom are removed from the free solve. A rotated support first transforms its translational coordinates into the support’s local axes; the selected local restraints are then enforced.
5. Sparse linear solve. The assembled system is stored as a sparse matrix and solved for free displacements using SciPy’s sparse direct solver:

After solving, the nodal displacement vector is transformed back to global coordinates. Reactions are recovered from the residual R = Kd − P at restrained degrees of freedom.

Loads, combinations, and response recovery

Nodal forces and moments are entered directly. Member loads support uniform loads and internal point loads, each in global X or global Y. Both types can be applied to the same member at once, and multiple point loads can be placed at different distances from the member’s i-end. Member loads are converted to consistent equivalent nodal loads so they act through the same assembled equilibrium system as nodal loads.

For each solved case, the backend recovers local axial force N, shear V, bending moment M, and longitudinal/transverse displacement along each member. Distributed-load equilibrium contributes continuously along the member; point-load jumps are treated on the appropriate side of each load position. Station points also include candidate locations for interior response extrema so plotted peak values do not depend only on coarse sampling.

Load combinations are computed by linear superposition of the solved load cases. This is consistent with the model’s linear-elastic stiffness assumption. The program does not re-solve a nonlinear structural state for a combination.

Modal analysis and mass source

Choose Modal analysis in the Results overview, click Run analysis, then select a load case or combination as a mass source. The eigenvalue solver uses the same elastic frame stiffness, support rotations, member releases, and shear-deformation setting as static analysis.

Member self-mass follows the consistent two-node frame mass matrix, based on each member’s density ρ and area A. In local coordinates, the matrix is (ρAL/420) times a dimensioned 6×6 coefficient matrix; it includes axial translation, transverse translation, and rotational coupling. It is transformed into global coordinates and assembled over all members. The sparse symmetric generalized eigenproblem returns the lowest requested positive modes.

Convert selected loads into translational mass

Mass conversion is optional in global X and global Y independently. For a selected case, or each nonzero case in a selected combination, the app converts the absolute factored force magnitude by:

• A nodal force becomes mass at that node’s matching global translation degree of freedom.
• A uniform member load contributes |w|L/g, split equally between the two end nodes in the chosen global direction.
• An internal member point load contributes |P|/g, apportioned between end nodes according to its relative position along the member.
• Moments do not become translational mass; unchecked directions are ignored. For a combination, absolute factored load contributions accumulate, so opposing signs do not cancel mass.

Modal response spectrum

The X-direction spectrum analysis uses natural periods and mode shapes from modal analysis. For influence vector \(\mathbf r_x\), each mode has participation factor \(\Gamma_n\) and effective modal mass \(M_n^*\):

The modal displacement contribution is \(\mathbf u_n=\boldsymbol{\phi}_n\Gamma_nS_a(T_n)/\omega_n^2\). Modal results are combined using SRSS or CQC. Since a response-spectrum result is an envelope magnitude, plotted signs follow the dominant modal contribution.

EN 1998-1:2004/2005 design spectrum

For the EN 1998-1 design spectrum, \(a_g=\gamma_Ia_{gR}\). The ground type and spectrum type define \(S,T_B,T_C,T_D\):

The lower bound \(\beta a_g\) applies on the descending branches. Modal force response uses \(S_d(T)\); modal displacement includes the behaviour-factor scaling defined by the analysis procedure.

EN 1998-1-1:2024 elastic response spectrum

The 2024 formulation uses mapped reference spectral accelerations (S_{\alpha,RP}) and (S_{\beta,RP}), site factors (F_\alpha) and (F_\beta), and the topographic factor (F_T). The zero-period ratio (F_A) is a separate parameter:

The damping factor changes across the initial ramp, then is held at its plateau value; the minimum is 0.55:

Here \(\xi\) is the damping ratio in percent. The standard NDP defaults shown in the tool are \(T_A=0.02\,\mathrm{s}\), \(F_A=2.5\), and \(\chi=4\). The default \(T_D\) depends on \(S_{\beta,RP}\). Supply project-specific mapped hazard, site, and National Annex parameters. If \(T_C\ge1\,\mathrm{s}\), the NDP calls for a spectrum-specific study.

EN 1998-1-1:2024 reduced spectrum for force analysis

The force-based approach reduces the elastic spectrum using \(q=q_Rq_Sq_D\). The reduction is period dependent below \(T_B\):

The 2024 elastic displacement spectrum transforms acceleration for shorter periods and extends the curve at long periods:

When \(v_{s,H}\) is available, \(F_L=(v_{s,H}/800)^{-0.4}\). Otherwise the site-category default for \(F_L\) is used. For reduced-spectrum design, the tool scales modal displacement with \(q_{disp}\), while the force spectrum lower bound does not enter the displacement calculation.

Modal combination

For CQC, \(\rho_{ij}\) depends on modal frequency ratio and viscous damping. The 2024 edition uses a distinct single-spectrum hazard parameterization and reduced spectrum; Type 1 and Type 2 apply to the earlier edition. Use project-specific hazard and National Annex parameters. See the BSI EN 1998-1-1:2024 publication page.

Shells combined with beams, and stiffness modifiers

The 3D workspace is a 3D Structure: beams and four-node shell elements (walls, slabs, plates) share the same nodes, with six degrees of freedom at every node (u_x, u_y, u_z, θ_x, θ_y, θ_z). One global stiffness matrix is assembled from the beam matrices and the shell matrices and solved once for all load cases.

Shell element

• Local frame. The shell normal is e_z = d₁ × d₂ (cross product of the two diagonals); e_x follows the mid-sides. Nodes are ordered round the shell, and the normal gives the positive sign of the pressure and of m_x, m_y.
• Membrane. Four-node isoparametric quadrilateral with Wilson–Taylor incompatible modes (QM6, condensed out with the Taylor correction), which removes shear locking in in-plane bending.
• Plate bending and shear. Reissner–Mindlin plate with the MITC4 assumed transverse shear strain (tying points at the mid-sides) and a shear correction factor of 5/6, so thin and thick plates are both handled without shear locking.
• Drilling rotation. A small penalty term γGt(θ_z − ½(∂v/∂x − ∂u/∂y))² (penalty form of the Hughes–Brezzi drilling formulation [14, 30–32]; γ = 10⁻⁴ is FaxinaX's own choice, not a value taken from those papers) gives the θ_z degree of freedom a stiffness, so shells connect rigidly to beams and to other shells in any plane.

Results are the membrane forces n_x, n_y, n_xy (kN/m), the bending and twisting moments m_x, m_y, m_xy (kNm/m) and the transverse shears q_x, q_y (kN/m), at the centre and the four corners, plus the von Mises stress on the top and bottom surfaces. The contour on the canvas averages the corner values at shared nodes. Pressure loads and self-weight are lumped consistently to the nodes; gravity, wind and user pressures are all area loads.

Checks run: six rigid-body modes and no spurious zero-energy mode; membrane and bending patch tests; simply supported and clamped square plates; Scordelis–Lo roof (vertical displacement of the free edge 0.301 against the reference 0.3024); beam and shell cantilevers; coupling of a beam into a shell edge; self-weight and combinations; free vibration of a simply supported plate (first frequency within 1 % of the closed form). They are automated in tests/test_shell_solver.py.

Stiffness modifiers for cracked reinforced concrete

Cracking lowers the stiffness of reinforced concrete members, so a linear analysis of a concrete structure multiplies the gross-section stiffness by modifiers. In FaxinaX each modifier belongs to one stiffness term, that is, to one degree of freedom of the element, and is entered between 0.001 and 10 (default 1.0).

The coupling term uses √(f₁₁f₂₂), so the modified matrix stays positive definite. Member forces and shell resultants are recovered with the modified stiffness, which keeps equilibrium exact.

The presets are starting values taken from the published tables; they are editable and are not a design recommendation. Use values appropriate to the load level (service or ultimate), to your national annex, and to the reinforcement. A modifier of 0.35 on I increases a flexural deflection by 1/0.35 = 2.86 at the same load. The test suite checks that A, I_y and J change only their own degree of freedom in the beam, for the shell bending (ratio 3.96 for m = 0.25, just under 4 because shear deformation is not reduced) and for the membrane (f₁₁ = 0.5 doubles the in-plane extension).

Triangular shell, regions and discs

• Three-node shell. A shell may have three nodes. Membrane and drilling stiffness come from three QM6 quadrilateral sub-elements (corners, side mid-points, centroid) whose mid-side dofs follow the corners linearly, with the centroid condensed out, so neighbouring shells stay conforming. Plate bending is a Reissner–Mindlin triangle with linear w, θ_x, θ_y and MITC3-type assumed shear strains tied to the tangential shear strain at the three side mid-points, which is free of shear locking and passes the constant-curvature patch test. Results (n, m, q) are in the triangle's local axes (e_x along side 1–2).
• Region mesher. Mesh region creates shells for a convex polygon from its corner nodes (a triangle gives three quadrilateral blocks or a regular triangle grid), a circular slab (square core with four curved blocks) or a ring/circular opening. Quadrilaterals or triangles can be chosen; nodes that coincide with existing nodes are reused. A clamped circular plate under uniform pressure meshed this way reproduces the closed-form centre deflection q a⁴/(64 D) within a few per cent.
• Speed and saved results. Shell recovery is linear in the element displacements, so a recovery matrix is built once per element shape and every load case is a matrix product; the server sends compact flat arrays and combinations are rebuilt in the browser from the load cases (including the von Mises values from n and m). Results are stored with the saved model and shown again until the model changes.

Combined beam and shell formulation

This section writes out how the beam and shell elements of the 3D workspace are formulated, how they are joined into one structure, and how forces are recovered. The formulations are the standard ones of the finite element literature listed under References; the numbers in square brackets point to that list.

1 · Degrees of freedom and assembly

Every node has six degrees of freedom, \(\mathbf d_i=[u,v,w,\theta_x,\theta_y,\theta_z]^T\) in global axes. Beams and shells use the same six, so they are joined simply by sharing a node: translations and all three rotations are continuous there. Each element matrix is built in its own local axes, rotated to global axes, and added at the positions of its nodes:

\(\mathbf A_e\) is the Boolean connectivity matrix of the element. \(\mathbf T_e\) is block diagonal with the 3×3 rotation \(\mathbf R=[\mathbf e_x\ \mathbf e_y\ \mathbf e_z]^T\) of the element local axes, repeated for the translation and rotation parts of every node (12×12 for a beam, 24×24 for a four-node shell, 18×18 for a triangle). Restrained degrees of freedom are removed, the free system is solved with a sparse direct solver, and the reactions are \(\mathbf R_s=\mathbf K_{sf}\mathbf d_f-\mathbf F_s\) [1,2,3].

2 · Beam element (Timoshenko, 12 degrees of freedom)

Axial and torsional behaviour are linear bars; bending in each principal plane is a Timoshenko beam, which keeps the shear deformation that the Euler–Bernoulli element neglects [4,5,6]. With the shear parameter \(\Phi=\dfrac{12EI}{GA_v L^2}\) the bending block of one plane, for deflection \(v\) and rotation \(\theta\), is

It is used once with \((I_z,A_{vy})\) for bending in the x–y plane and once with \((I_y,A_{vz})\) for the x–z plane, and \(\Phi=0\) gives the Euler–Bernoulli matrix. The local axes are \(\mathbf e_x\) along the member, \(\mathbf e_z\) upward (or global X for vertical members) and \(\mathbf e_y=\mathbf e_z\times\mathbf e_x\), then rotated by the roll angle. A release (hinge) at an end is applied by static condensation of that degree of freedom, \(\mathbf k'=\mathbf k_{aa}-\mathbf k_{ab}\mathbf k_{bb}^{-1}\mathbf k_{ba}\), so the member end carries no force in it [3,6]. Stiffness modifiers multiply the individual terms \(EA,\ GA_v,\ GJ,\ EI_y,\ EI_z\).

Complete element stiffness matrix. Joining the axial bar, the torsion bar and the two bending blocks gives the 12×12 local stiffness matrix of the Timoshenko beam element. The degrees of freedom of the two ends are ordered \(\mathbf d^{\ell}=[u_1,v_1,w_1,\theta_{x1},\theta_{y1},\theta_{z1},\;u_2,v_2,w_2,\theta_{x2},\theta_{y2},\theta_{z2}]^T\) in the local axes, with \(\mathbf f^{\ell}=\mathbf k^{\ell}\mathbf d^{\ell}\).

The matrix is symmetric and has exactly six zero eigenvalues, the six rigid-body motions. Bending in the x–z plane uses the same block as the x–y plane with the signs of the \(w\)–\(\theta_y\) coupling terms reversed, because the rotation about the local y axis is \(\theta_y=-\mathrm dw/\mathrm dx\). The entries above are the ones the solver assembles: they were compared numerically with the matrix produced by the program for a test member and agree to rounding error. Setting \(\Phi_y=\Phi_z=0\) gives the Euler–Bernoulli matrix, and the stiffness modifiers scale \(EA\), \(GJ\), \(EI_y\), \(EI_z\) and the shear areas before the matrix is formed.

Member loads become consistent nodal loads, for example a uniform load \(q\) gives \(\mathbf f=[\tfrac{qL}{2},\ \tfrac{qL^2}{12},\ \tfrac{qL}{2},\ -\tfrac{qL^2}{12}]^T\) per bending plane, and a point load \(P\) at \(a\) gives the usual fixed-end forces. Warping torsion of open sections is not part of the 12-degree-of-freedom element; it is recovered afterwards from the torque (see the warping post-processing in the steel check) with Vlasov's theory [7].

3 · Four-node shell element (membrane + plate + drilling)

The shell is flat. In the local frame \(\mathbf e_x,\mathbf e_y,\mathbf e_z\) (normal \(\mathbf e_z=\mathbf d_1\times\mathbf d_2\), the cross product of the diagonals) its 24 degrees of freedom split into membrane \((u,v)\), plate \((w,\theta_x,\theta_y)\) and drilling \((\theta_z)\) parts, with the isoparametric map \(\mathbf x=\sum_i N_i(\xi,\eta)\mathbf x_i\), \(N_i=\tfrac14(1+\xi_i\xi)(1+\eta_i\eta)\) and Jacobian \(\mathbf J=\partial\mathbf x/\partial(\xi,\eta)\) [1,2,3]. The element matrix is

Membrane. The displacement field is enriched with incompatible modes, \(\mathbf u=\sum N_i\mathbf u_i+\sum_{k=1}^{2}M_k\boldsymbol\alpha_k\) with \(M_1=1-\xi^2\) and \(M_2=1-\eta^2\) (four extra parameters, two per direction) [8,9]. The enhanced strain–displacement matrix is evaluated with the Taylor correction \(\mathbf B_\alpha=\dfrac{\det\mathbf J_0}{\det\mathbf J}\mathbf J_0^{-T}\nabla_{\xi\eta}M\), where \(\mathbf J_0\) is the Jacobian at the element centre, which makes the element pass the patch test on distorted meshes [9]. The parameters \(\boldsymbol\alpha\) are condensed out at element level:

Plate bending and shear. With the Reissner–Mindlin kinematics [10,11] the curvatures are \(\boldsymbol\kappa=[\partial\theta_y/\partial x,\ -\partial\theta_x/\partial y,\ \partial\theta_y/\partial y-\partial\theta_x/\partial x]^T\) and the transverse shear strains \(\boldsymbol\gamma=\nabla w-\boldsymbol\theta\). Evaluated directly at the Gauss points, the shear strains lock when the plate is thin. The MITC4 element [12,13] replaces them by an interpolation of the covariant strains sampled at four tying points at the mid-sides:

which are then transformed to the local Cartesian components with \(\mathbf J^{-1}\). The shear correction factor is \(\kappa=5/6\). Integration is 2×2 Gauss for all terms. The constitutive matrices are \(\mathbf D_m=\dfrac{Et}{1-\nu^2}\begin{bmatrix}1&\nu&0\\\nu&1&0\\0&0&\frac{1-\nu}{2}\end{bmatrix}\) and \(\mathbf D_b=\dfrac{t^2}{12}\mathbf D_m\).

Drilling rotation. A flat shell has no stiffness for \(\theta_z\), so a beam or another shell meeting it in a different plane would give a singular matrix. The rotation is tied to the in-plane rotation of the continuum by a penalty on \(\theta_z-\omega\), \(\omega=\tfrac12(\partial v/\partial x-\partial u/\partial y)\), with a small coefficient \(\gamma\); \(\mathbf b_d\) is the row that evaluates it. This is the penalty form of the variational formulation of Hughes and Brezzi [14], whose behaviour in membrane elements was assessed by Hughes, Masud and Harari [31] and which Ibrahimbegović, Taylor and Wilson [32] used for a quadrilateral; the older alternative is Allman's special displacement interpolation with vertex rotations [30]. In that literature the penalty parameter is a free parameter, reported of the order of the shear modulus or a fraction of it. FaxinaX uses the much smaller \(\gamma=10^{-4}\) (times \(Gt\)) because \(\theta_z\) mainly has to be non-singular where a beam or a second shell is attached, not to reproduce an accurate in-plane rotation field. The value is the program's own choice and is not taken from the references; it is small enough not to stiffen the membrane and large enough to keep the system well conditioned.

4 · Three-node shell

The triangle keeps the same split. The membrane and drilling parts are built from three QM6 sub-quadrilaterals formed with the corners, the side mid-points and the centroid; the mid-side degrees of freedom follow the corners linearly and the centroid is condensed out, so neighbouring shells remain conforming. The plate part is a Reissner–Mindlin triangle with linear \(w,\theta_x,\theta_y\) and MITC3-type shear strains tied to the tangential shear strain at the three side mid-points [15], which is free of shear locking and passes the constant-curvature patch test.

5 · Loads on shells

A pressure \(p\) (gravity, wind, user pressure) is converted to consistent nodal forces \(\mathbf f=\int_A\mathbf N^Tp\,\mathbf n\,dA\) on the translations, and the self-weight is \(\rho g t\) over the area. The wind loads of EN 1991-1-4 act on the shells through the same area-load vector, so they appear in the combinations exactly like any other pressure.

6 · How beams and shells interact

• Compatibility. A beam end and the shell corner at the same node have identical translations and rotations, so a beam on a slab or wall edge is rigidly connected there. Between nodes the two elements are independent; refining the mesh along the edge makes the connection closer to the true line contact.
• Force transfer. The beam's axial force and shear are carried by the shell's membrane and plate degrees of freedom through the shared translations, the beam bending and torsion by the shell's \(\theta_x,\theta_y\) rotations, and any moment about the shell normal by the drilling stiffness. The drilling stiffness is deliberately small, so a beam lying in the plane of a wall mainly transfers its in-plane bending through the wall's membrane action, which is physical.
• Axes and eccentricity. The beam centroid and the shell mid-surface coincide at the node. The offset of a downstand beam below a slab is not modelled automatically; it can be represented with a rigid or short member at the correct level, or by modifying the beam stiffness for the T-beam flange.
• Stiffness modifiers. Cracking factors act term by term on both element types (see the table above), and the recovered forces use the modified stiffness, so equilibrium stays exact.

7 · Solution, reactions and recovery

• Beams. The end forces are \(\mathbf f^{\ell}=\mathbf k^{\ell}\mathbf T\mathbf d-\mathbf f_{\text{fixed}}\); values at stations along the member follow from equilibrium of the free body between the start and the station, including the member loads, which gives \(N,V_y,V_z,T,M_y,M_z\).
• Shells. The resultants \(\mathbf s=[n_x,n_y,n_{xy},m_x,m_y,m_{xy},q_x,q_y]^T=\mathbf D\mathbf B\,\mathbf d^{\ell}\) are linear in the element displacements, so a recovery matrix \(\mathbf R_s\) (rows for the centre and the corners) is built once per element shape and \(\mathbf s=\mathbf R_s\mathbf d^{\ell}\) for every load case. Combinations are linear sums of the case results.
• Check. The sum of applied loads and reactions in each direction and about the origin is reported as the equilibrium check.
• Dynamics. The mass matrix is lumped from the member and shell masses plus the added mass, and the modes follow from \(\mathbf K\boldsymbol\phi=\omega^2\mathbf M\boldsymbol\phi\) [1].

8 · Verification of the combined formulation

The tests are automated in tests/test_shell_solver.py. They validate the formulation on the standard benchmarks; a project model still needs its own review of supports, mesh density and the position of the beam relative to the shell mid-surface.

Wind on frames, cladding and shells

• Zones and coefficients. Tables 7.1 to 7.5 and the Figure 7.4 wall strips (zones A, B, C by height), flat, duopitch, monopitch, hipped, multispan, vaulted and domed roofs; net pressure with the internal pressure c_pi.
• Parapets (7.4.1, Table 7.9), friction (7.5, Table 7.10) and structural elements: rectangular, sharp-edged, polygonal and circular sections (7.6 to 7.9, Figure 7.28 for c_f,0, Table 7.13 for roughness, Table 7.14 end effects for cylinders in a row).
• Lack of correlation. The reduction of the windward and leeward pressures applies only when the structure is designed for the overall force. The generator and the 3D wind dialog have a Design for switch: frame (overall force, reduction applied) or cladding (full local pressures). The overall-force card is the same in both.
• 2D frame. The Wind load dialog takes the frame spacing s, multiplies each surface pressure by s to obtain a line load in N/m, and creates a wind load case (ψ₀ = 0.6).
• 3D cladding panels. One-way and two-way panels pass their pressure to the supporting members as trapezoidal or triangular loads (tributary areas), which the solver integrates exactly. The supporting edges of a panel are chosen by the user.
• Shells. A shell that is marked as receiving wind is given the zone pressure at its centre, as a surface pressure on the shell; the finite element solution distributes it to the supports and to the connected beams. The outward side is taken away from the model centre, or set by the user.
• Pressure map. The canvas can colour cladding panels and shells by the net pressure of the active wind case (blue suction, red pressure), with a colour bar.

Verification: tests/test_wind_engine.py, tests/test_wind_fig74.py and tests/test_cladding_engine.py check the zone tables, q_p by hand, force equilibrium of the generated cases and the resultant of the shell pressures. The generated wind loads should still be reviewed against the building and the national annex.

Does the answer make sense?

A solver always returns numbers. Whether they are believable is an engineering judgement, and it is best made before looking at the values: sketch the load path, the deflected shape and the bending moment diagram you expect, then compare. Most serious errors are visible at that level.

1. Load path and deflected shape

• Loads travel to the supports along the stiffest route. A stiffer member attracts a larger share of the force. A pinned end or release passes no moment, a rigid joint passes moment and keeps the angle between the connected members.
• Supports fix the shape. A fixed support has zero translation and zero rotation, a pin has zero translation and zero moment, and a roller has zero moment and moves freely along its free direction.
• The deflected shape is continuous and smooth except at releases, where the rotation may jump. Its curvature has the sign of the bending moment: it is concave upward where the member sags and concave downward where it hogs, with inflection points where the moment is zero.
• Symmetry is inherited. A symmetric structure under a symmetric load gives symmetric deflections and moments, and zero shear on the axis of symmetry.

2. Relations between the diagrams

Use these relations to read a diagram quickly. Uniform load gives linear shear and parabolic moment, a point load gives constant shear segments and linear moment, and a member with no load between its ends has linear moment. If a diagram shows a curve where there is no load, or a jump where nothing is applied, the model is not what you meant.

3. Hand checks with standard formulas

Compare the order of magnitude with the closed-form values below (prismatic member, length L, flexural rigidity EI, uniform load q, point load P). The first benchmark cases on this page use the same formulas.

For a frame, isolate one member and check it with these formulas using the end moments the solver reports. Static equilibrium of that member must hold: the shears at the two ends must balance the load on it, and the end moments plus the moment of the shears must balance as well.

4. Count the redundancy

• n < 0: the structure is a mechanism. No static solution exists, and the Result check will report it with the likely cause.
• n = 0: statically determinate. Forces follow from equilibrium alone, so changing a section size changes the deflections but not the forces.
• n > 0: indeterminate. Forces depend on the relative stiffness of the members, so every member property matters, including the ones you assumed.

The count is a necessary condition only. A structure can pass it and still contain a local mechanism, for example a bay with a missing diagonal, so also look at the deflected shape.

5. Typical mistakes and what they look like

6. A short checklist before you rely on a result

1. Read the Result check message. Resolve every error and understand every warning.
2. Confirm that reactions equal the applied loads and that gravity reactions point upward.
3. Compare the deflected shape and the moment diagram with your sketch.
4. Check one or two values by hand using the formulas above or a simplified model.
5. Change an input a little (a section, a support, a release) and make sure the result moves in the direction and by the amount you expect.
6. Compare the deflection with the limit in the applicable code and National Annex. A deflection above span/50 is rarely a real serviceable structure and usually points to an input error.

Model limits and independent review

Idealized supports, section axes, restraints, load signs, effective lengths, and member properties can materially change results. The steel check is a separate resistance assessment and does not add nonlinear behavior to the frame solver. Results must be checked independently by a qualified structural engineer before they are used in design or construction.

References

The formulations in this page follow the standard literature below. The program implements them; it does not reproduce any commercial code. Equation numbers and page numbers are not given because the cited works should be read in full when the details matter.

Finite element and matrix structural analysis

1. Bathe, K.J. (1996). Finite Element Procedures. Prentice Hall, Englewood Cliffs.
2. Zienkiewicz, O.C., Taylor, R.L., Zhu, J.Z. (2013). The Finite Element Method: Its Basis and Fundamentals, 7th ed. Butterworth-Heinemann, Oxford.
3. Cook, R.D., Malkus, D.S., Plesha, M.E., Witt, R.J. (2002). Concepts and Applications of Finite Element Analysis, 4th ed. Wiley, New York.
4. McGuire, W., Gallagher, R.H., Ziemian, R.D. (2000). Matrix Structural Analysis, 2nd ed. Wiley, New York.
5. Przemieniecki, J.S. (1968). Theory of Matrix Structural Analysis. McGraw-Hill, New York (Dover reprint 1985).
6. Timoshenko, S.P. (1921). On the correction for shear of the differential equation for transverse vibrations of prismatic bars. Philosophical Magazine 41, 744–746.
7. Vlasov, V.Z. (1961). Thin-Walled Elastic Beams, 2nd ed. Israel Program for Scientific Translations, Jerusalem.

Shell and plate elements

8. Wilson, E.L., Taylor, R.L., Doherty, W.P., Ghaboussi, J. (1973). Incompatible displacement models. In: Fenves, S.J. et al. (eds), Numerical and Computer Methods in Structural Mechanics. Academic Press, New York, 43–57.
9. Taylor, R.L., Beresford, P.J., Wilson, E.L. (1976). A non-conforming element for stress analysis. International Journal for Numerical Methods in Engineering 10(6), 1211–1219.
10. Reissner, E. (1945). The effect of transverse shear deformation on the bending of elastic plates. Journal of Applied Mechanics 12, A69–A77.
11. Mindlin, R.D. (1951). Influence of rotatory inertia and shear on flexural motions of isotropic, elastic plates. Journal of Applied Mechanics 18, 31–38.
12. Dvorkin, E.N., Bathe, K.J. (1984). A continuum mechanics based four-node shell element for general non-linear analysis. Engineering Computations 1(1), 77–88.
13. Bathe, K.J., Dvorkin, E.N. (1985). A four-node plate bending element based on Mindlin/Reissner plate theory and a mixed interpolation. International Journal for Numerical Methods in Engineering 21(2), 367–383.
14. Hughes, T.J.R., Brezzi, F. (1989). On drilling degrees of freedom. Computer Methods in Applied Mechanics and Engineering 72(1), 105–121.
15. Lee, P.S., Bathe, K.J. (2004). Development of MITC isotropic triangular shell finite elements. Computers & Structures 82(11–12), 945–962.
16. MacNeal, R.H., Harder, R.L. (1985). A proposed standard set of problems to test finite element accuracy. Finite Elements in Analysis and Design 1(1), 3–20.
17. Timoshenko, S.P., Woinowsky-Krieger, S. (1959). Theory of Plates and Shells, 2nd ed. McGraw-Hill, New York.
18. Scordelis, A.C., Lo, K.S. (1969). Computer analysis of cylindrical shells. Journal of the American Concrete Institute 61(5), 539–561.
19. Chapelle, D., Bathe, K.J. (2011). The Finite Element Analysis of Shells – Fundamentals, 2nd ed. Springer, Berlin.

Reinforced-concrete design of beams, columns, slabs and walls

20. Wood, R.H. (1968). The reinforcement of slabs in accordance with a pre-determined field of moments. Concrete 2(2), 69–76; and Armer, G.S.T. (1968), discussion, Concrete 2(8), 319–320.
21. Marti, P. (1990). Design of concrete slabs for transverse shear. ACI Structural Journal 87(2), 180–190.
22. Nielsen, M.P., Hoang, L.C. (2011). Limit Analysis and Concrete Plasticity, 3rd ed. CRC Press, Boca Raton.
23. fib (2013). fib Model Code for Concrete Structures 2010. Ernst & Sohn, Berlin (punching shear and shear provisions).

Standards

24. EN 1992-1-1:2023, Eurocode 2: Design of concrete structures – Part 1-1: General rules and rules for buildings, bridges and civil engineering structures, including Annex G (design of membrane, shell and slab elements) and 8.4 (punching).
25. EN 1992-2:2005, Eurocode 2 – Part 2: Concrete bridges, Annex LL (sandwich model for shell elements).
26. EN 1993-1-1:2005 and EN 1993-1-1:2022, Eurocode 3: Design of steel structures – Part 1-1.
27. EN 1991-1-4:2005, Eurocode 1: Actions on structures – Part 1-4: Wind actions.
28. EN 1998-1:2004 and EN 1998-1-1:2024, Eurocode 8: Design of structures for earthquake resistance.
29. ACI 318-19, Building Code Requirements for Structural Concrete (effective stiffness modifiers, Table 6.6.3.1.1(a)).

Drilling rotation (rotation about the shell normal)

30. Allman, D.J. (1984). A compatible triangular element including vertex rotations for plane elasticity analysis. Computers & Structures 19(1–2), 1–8.
31. Hughes, T.J.R., Masud, A., Harari, I. (1995). Numerical assessment of some membrane elements with drilling degrees of freedom. Computers & Structures 55(2), 297–314.
32. Ibrahimbegović, A., Taylor, R.L., Wilson, E.L. (1990). A robust quadrilateral membrane finite element with drilling degrees of freedom. International Journal for Numerical Methods in Engineering 30(3), 445–457.

The drilling-rotation sources were looked up online; the original formulation is Hughes and Brezzi [14] (DOI 10.1016/0045-7825(89)90124-2). Check issue and page numbers against the journal.

The reference list names the sources the methods are based on. Where a clause of a current standard is paraphrased (EN 1992-1-1:2023 in particular), check the wording and the National Annex values against the published standard before relying on the result.