In this article Stress Linearization Procedure based on Annex 5-A of ASME Sec VIII Div 2 code will be illustrated using an example.

**Example Problem**: A carbon steel vessel (ID 500 mm x 20 thk x 1000 mm long) has a nozzle connection (ID 250 mm x 20 thk x 130 mm projection) of the same material. The ends of the vessel are fixed and a shear load of 1000 kN is applied at the nozzle to shell junction along the vessel axis. Using FEA the linearized Von-Mises Membrane and Membrane + Bending Stresses in the vessel needs to be evaluated near the location of maximum stress.

The problem analysis is conducted using ANSYS.

**ANSYS Analysis Plots**

The Finite Element Model

Boundary Conditions and Loads (Note: Both ends including the end not visible in the plot are fixed)

Von-Mises Stress in the vessel

Coordinate system to define the path for the Stress Classification Line (SCL). A local coordinate system is created (using create coordinate system aligned with hit point normal method in ANSYS) near the max Von-Mises Stress location, so that its X-Y-Z axes represent tangential (radial), hoop and normal (meridional) directions respectively.

SCL Path (Near the Location of Max Von-Mises Stress)

**Stress Linearization Procedure:**

The hoop, normal (meridional) and tangential (radial), direct along with corresponding shear stress components were recorded across 5 equidistant points along the SCL path.

Subscript Meanings: h – hoop, n – normal, t – tangential, hn – hoop normal, nt – normal tangential, th – tangential hoop

Thickness across SCL Path, t = 20 mm

Distance between points, Δx = t/4 = 5 mm

**Calculation of Membrane Stress Tensor**

The membrane stress tensor is the tensor comprised of the average of each stress component along the stress classification line.

Membrane Hoop Stress

Subscripts: hm – hoop membrane, hnm – hoop normal membrane etc

**Calculation of Bending Stress Tensor**

(a) Bending stresses are calculated only for the local hoop and meridional (normal) component stresses, and not for the local component stress parallel to the SCL or in-plane shear stress.

(b) The linear portion of shear stress needs to be considered only for shear stress distributions that result in torsion of the SCL (out-of-plane shear stress in the normal-hoop plane).

(c) The bending stress tensor is comprised of the linear varying portion of each stress component along the stress classification line

Bending Hoop Stress

Subscripts: hb – hoop bending, hnb – hoop normal bending etc

Note that bending for other components are not calculated (see points (a) and (b)) as required by ASME Sec VIII Div 2, Annex 5-A para 5-A.4.1.2.

**Calculation of Membrane + Bending Stress Tensor**

x = 0 represents 1st point on the SCL

x = t represents the other end point on the SCL

Subscripts: hmb0 – hoop membrane + bending at x = 0, hnmbt – hoop normal membrane + bending at x = t etc

**Calculation of Linearized Von-Mises Membrane and Membrane + Bending Stress**

Subscripts: eqvm – Equivalent Membrane Stress or Von-Mises Membrane Stress, eqvmb0 – Equivalent Membrane + Bending Stress at x=0, eqvmbt – Equivalent Membrane + Bending Stress at x=t

Reference: Composite Simpson’s Rule

Hello Mr. Sandip,

The article is nicely illustrated with examples.

You have mentioned stress integration method to linearize stress results from solid elements. It is good.

But could you explain how structural stress method based on nodal forces works with some examples?

Have to understand the concepts of nodal forces methods and how later methods are way off with stress integration method

Hi Krishna,

I illustrated the stress integration method as this is the method used by most commercial softwares (eg ANSYS, ABAQUS) for carrying out stress linearization. However conceptually the method based on nodal forces also does the same thing. Basically membrane stress is the average stress across the section being evaluated and is computed as f/t (total force experienced by the SCL line per unit width divided by length of the SCL)

Bending stress here is simply 6m/t^2, where m is the moment per unit width experienced by the SCL line. Consider a rectangle of unit width and t height subjected to moment m to understand this formula. The computation of f is done using nodal forces and width of the elements under consideration using code formulas. For computation of moments in addition to finding forces the location of forces w.r.t mid thickness is required to calculate moments. I’ll see if I can illustrate this through an example in my upcoming articles.

This is one of the best explanations I have seen for stress linearisation. You have describe it very clearly much better than the commercial software manuals.

Thank you for sharing your nice work!

Nice to hear that, James.

Yes, at one point of time Ansys Stress linearization procedure wasn’t compliant with this ASME requirements. But in recent versions ( though i am not sure from which version on wards),Ansys has a option to Include or Exclude Zero Through-Thickness Bending Stress, by setting this to YES, now Ansys Stress linearization procedure can produce results compliant with ASME requirements.

Thanks Santosh. Yes ANSYS has included this in some iteration of 19 th version. I have updated the article accordingly.