FEM logo

What is shear locking?

Shear locking is an error that occurs in finite element analysis due to the linear nature of quadrilateral (first order) elements. The linear elements do not accurately model the curvature present in the actual material under bending, and a shear stress is introduced. The additional shear stress in the element (which does not occur in the actual beam) causes the element to reach equilibrium with smaller displacements, i.e., it makes the element appear to be stiffer than it actually is and gives bending displacements smaller than they should be.

Shear locking occurs when the element is unable to capture the kinematics of deformation. Let's consider pure bending of a beam. The linear elastic solution is given for an Euler Bernoulli beam at the left side and linear equation of the element at the right side.

In the linear element the corner nodes at horizontally shifted, resulting in a shear strain in horizontal plane. The shear stress contributes to the equilibrium of forces and thereby disturbs the deformation of the bending beam.

Exact solution Linear element
equation equation
Strains in the beam:
Strains in element:
Shear strain is zero Shear strain is non-zero

Note that:
L= length of the element;
Y= half the element thickness;

How to prevent shear locking?

In areas where linear elements are loaded by in plane bending, shear locking in first order elements is prevented by using preferably 3 elements over the height. This is illustrated in the example below. In the area of interest ensure that the elements are as rectangular as possible (preferably square), to give the most accurate results.

The results shown below are calculated with NX Nastran (CQUAD4 elements), but calculations with ANSYS 14 show similar results (SHELL63, SHELL181, BEAM44 and BEAM188 elements).
The following example shows an I-beam (h=200mm, tweb=9mm, w=200mm, tflange=15mm) with length L=8m. The end load is W=21.36kN. The web is modelled by linear shell elements and the flange by beam elements. The beam is clamped at the other side. The theoretical maximum deflection is (according to Euler Bernoulli):


(with E=205000 MPa and I=6611.25·104 mm4)

Five models were run containing five different ways of meshing as illustrated in the figure below.

FEA or FEM Shear locking example

The result of deflection and maximum stresses due to the different element shapes is given in the table below:

Element shape Deflection δ
Max stress
Error in deflection
Trapezoidal elements 83.1 144.4 69.1
Parallelogram 185.1 209.4 31.2
Rectangle 268.3 259.7 0.26
Square 270.2 279.2 -0.44
Square 3 elements in height 270.2 277.4 -0.44

*Note that these stresses include bending of the flange element.  Therefore this value may be calculated with the theoretical equation σ=W·L·½h/I.  The average value (average max and min of the combined stresses is 259MPa for the square element, which is correct).

To get accurate results with the buckling code checker, when in plane bending occurs, only the last model gives reliable results. The reason is that due to bending the stress differs from the neutral axis to the flange of the beam.  With only 1 element in height, this element stress is not accurately calculated with linear elements in the model.

Another way to avoid shear locking is to use 2nd order (quadratic) elements with full integration scheme. The mid-side nodes wil follow the bending curve, avoiding the shear strain in horizontal plane.

What else is important besides preventing shear locking?

When modeling a model using linear shell (plate) elements, the model should comply with the following guidelines to increase the reliability of your results:

The code checker works with the element stresses. Try to reduce the use of triangular elements as much as possible. In The NX Nastran manual the following direction is given:

“You should use the CQUAD4 element when the surfaces you are meshing are reasonably flat and the geometry is nearly rectangular. For these conditions, the quadrilateral elements eliminate the modeling bias associated with the use of triangular elements, and the quadrilaterals give more accurate results for the same mesh size. If the surfaces are highly warped, curved or swept, you should use triangular elements.”

For ANSYS users the same rule applies in case of using linear plate elements.

Read the other tips for a healthy and realistic FEA model:

Customer area

Sign in

Forgot your password?
Hand calculations

Latest software release

Sign up for a free trial <