# Seam Weld Fatigue Analysis

Seam Weld Fatigue analysis is available to facilitate Fatigue analysis for seam welded structures. It allows you to simulate the Fatigue failure at the seam weld joints to assess the corresponding fatigue failure characteristics like Damage and Life.

Two methods are currently available to run Seam Weld Fatigue Analysis in OptiStruct:
• Volvo Method (METHOD=VOLVO on FATPARM entry)
• Joint Line Method (METHOD=JNTLINE on FATPARM entry)

The Volvo method implemented in OptiStruct is based on a research paper Fatigue Life Prediction of MAG-Welded Thin-Sheet Structures published by M. Fermér, M Andréasson, and B Frodin. The method is a hot spot stress approach applicable to thin metal sheets. Hot spot stress is calculated from grid point forces at weld line. The method showed a good agreement with laboratory test results for sheet thickness between 1.0 mm and 3.0 mm. The method typically requires two SN curves. One is a bending SN curve which is dominated by bending stress, and the other is a membrane SN curve which dominated by membrane stress.

The Joint Line method is based on directly calculating the stresses within a certain evaluation distance from the joint or weld line. Additionally, unlike the Volvo method, the weld elements are not modeled in the Joint line method. The damage evaluation is only conducted at the root locations for Joint line method.

## Implementation

### Modeling Requirements: Volvo Method

With the Volvo method, the Seam Weld Fatigue Analysis implementation in OptiStruct consists of the following modeling requirements.
1. Weld sections to be analyzed for seam weld fatigue should be meshed with CQUAD4 elements whenever possible. CTRIA3 elements may be used for corner weld if inevitable and for closing the end of weld line, if necessary. Other element types are currently not supported for seam weld fatigue.
2. The weld should be modeled by a single or double row of CQUAD4 elements. If a 2 sided fillet is to be modeled, a third row of CQUAD4 may be used.
3. The thickness of the weld element is the same as the effective throat.
4. The mesh size around the weld should be as regular as possible. Although this method is less sensitive to mesh size, a mesh size of about 10 mm would be a good choice according to Fermér, Andréasson, Frodin. This paper showed that large hot spot stress differences did not exist between mesh size 12 mm and mesh size 5 mm in case of a regular mesh.
5. The weld element should have a dedicated property ID that is referenced by the PIDi fields of the FATSEAM Bulk Data Entry. For more information, refer to Input/Output. The property should be stiff enough to be a force transducer.
6. The weld element normal direction should point outwards such that the normal direction is toward the weld toe, not toward the weld root. The normal direction of weld element plays a critical role in determining the weld toe and the surface to be examined on the base of the weld.

### Modeling Requirements: Joint Line Method

With the Joint Line method, the seam weld Fatigue Analysis implementation in OptiStruct consists of the following modeling requirements.
1. Unlike the Volvo method, the weld itself is not modeled in the Joint line method.
2. The weld line or joint line should be represented using PLOTEL elements.
3. These elements should be referenced as SETs on the ELSET continuation line of the FATSEAM Bulk Data Entry.
4. Mismatch in mesh density is allowed on either side of the joint line.
5. The normal direction of the shell elements part of the two or more plates welded at the joint line can be visualized in HyperMesh. The weld side (which side the Fatigue damage is evaluated) is determined based on the WLDSIDE field on the FATSEAM entry.
6. All elements sharing the same weld line and REFEID should have consistent element normals, which match with the element normal identified by the corresponding REFEID element.

### Weld Basics

A weld can be used to join two parts together. Welds vary in shapes and sizes depending on the type of joint that is required. For example, welds for fillets and overlap joints are different. Typically, a weld consists of the following parts:
• Face
• Toes
• Throat
• Root
• Legs
The face of a weld is the outer surface of the weld that is visible to you. The toes are the points where the base material of the connected plates intersects with the weld material along the weld face. The weld throat is the distance between the root and the center of the face. The weld root is point of deepest weld penetration and it is opposite to the weld face. The weld legs extend from the root of the weld to the toes.

### Good Weld Design Practice

This section provides a basic overview of stress concentrations in welded structures and a few recommendations for good weld design. This section should not be considered as a complete weld design guide and does not cover an exhaustive list of weld design recommendations.

All welds contain stress concentrations which will reduce the fatigue life. A local stress concentration occurs at the toe of the weld and is controlled by the welding process conditions. This stress concentration is embedded in a macroscopic stress concentration that is a result of the design of the weld joint.
• Weld shape-based stress concentration:
Figure 2 shows the stress concentration at the toe of a weld. Its magnitude depends on the flank angle, $\theta$, local weld toe radius, r, and plate thickness, t. The concept of a weld reinforcement is a misnomer as you can see that the stress concentration actually increases with increasing weld metal, that is, an increase in flank angle, $\theta$.
• Weld design-based stress concentration:

The second stress concentration comes from the joint design. Stress concentrations arise whenever there is a change in stiffness in the structure. It can result from either an increase of decrease in stiffness. For example, a hole in a plate will have about the same stress concentration as a rigid boss added to the plate. Here are some examples of weld joints contrasting good and poor design practice.

First you need to consider a cover plate welded to a bending beam. A large stress concentration exists at the end of the cover plate because of the large change in stiffness. A better design is shown on the right side where there is a more gradual change in stiffness.
A second source of stress concentration is unintentional bending stresses caused by asymmetric geometries. The design on the left will have larger bending stresses than the double lap joint on the right side.
Welding plates of differing thicknesses or widths is always problematic. Just as above, the easiest geometry to weld has the largest stress concentration. You should always consider moving the welds to lower stress areas in the structure and have a gradual transition in stiffness such as the joint shown Figure 5(b).

## Volvo Method

### Supported Weld Types

OptiStruct supports certain types of welds for Seam Weld Fatigue Analysis.

The type can be selected using the WTYPE field on the FATSEAM Bulk Data Entry.
• Only one row of elements can be defined for the weld face elements or either of the weld legs.
• The damage calculation locations are automatically chosen based on the weld type (as explained in Fillet). With the exception of the throat damage location, both the root and toe damage locations are evaluated based on the grid point forces and subsequent stresses induced in the corresponding elements adjacent to the weld elements. For throat damage, the weld element grid point forces, and subsequent stresses are directly considered.
• OptiStruct currently supports the following weld types.

#### Fillet

A fillet weld is a weld joining two sheets at an angle. Typical failure locations are marked in Figure 6(a). A fillet weld may be modeled by inclined CQUAD4 as in Figure 6(b). Depending on how much the weld penetrates, the weld may be modeled by a single or double row of CQUAD4. If a Two-sided fillet is to be modeled, three rows of CQUAD4 may be used.

OptiStruct evaluates failures at root and toe when a weld element is CQUAD4. If CTRIA3 is used for a weld element, only toe is evaluated.

#### T-joint

• One-sided One Row
For a One-sided One Row T-joint, the weld element normal direction should point towards the weld toe. The nodes of the weld element are in line with the weld toes. The length should be determined by the actual dimensions of the weld element (typically L=T1+T2).

The thickness of the weld element is the effective weld throat (typically it is equal to L/1.414).

• One-sided Two Row
Multiple rows are recommended for welds where the weld penetration is high and the weld typically forms the basis for contact between the two plates. Such welds are more rigid compared to welds where the penetration is lower, thereby additional rows of weld shell elements are required to capture the behavior. In Figure 8, the weld has penetrated more than the weld in Figure 7. For a One-sided Two Row T-joint, the two weld element normal directions should point towards the weld toe. The length should be determined by the actual dimensions of the weld element (typically L=T1+T2).

The thickness of the weld element is recommended to be set equal to 0.35*L.

• Two-sided Two Row
For a Two-sided Two Row T-joint, the weld element normal directions should point towards the corresponding weld toe. The nodes of the weld elements are in line with the corresponding weld toes. The length should be determined by the actual dimensions of the weld element (typically L=T1+T2).

The thickness of the weld element is the effective individual weld throat (typically it is equal to 1.414*L).

• Two-sided Three Row
Multiple rows are recommended for welds where the weld penetration is high and the weld typically forms the basis for contact between the two plates. Such welds are more rigid compared to welds where the penetration is lower, thereby additional rows of weld shell elements are required to capture the behavior. In Figure 10, the welds have penetrated more than the welds in Figure 9. For a Two-sided Three Row T-joint, the two weld element normal directions should point towards the corresponding weld toe. The weld element normal for the central vertical element can point to either weld toe.

#### Cross-joint

For a cross-joint, all weld elements associated with one cross joint weld should be specified in a single FATSEAM entry, otherwise OptiStruct will treat the cross-joint fillet weld as separate multiple welds and may output unexpected results. Additional requirement for a cross-joint is that the joint should be symmetric.
• One-sided One Row
For a One-sided One Row Cross-joint, the weld element normal direction should point towards the corresponding weld toe.
• One-sided Two Row

Multiple rows are recommended for welds where the weld penetration is high and the weld typically forms the basis for contact between the two plates. Such welds are more rigid compared to welds where the penetration is lower, thereby additional rows of weld shell elements are required to capture the behavior. In Figure 12, the welds have penetrated more than the welds in Figure 11. For a One-sided Two Row Cross-joint, the weld element normal direction should point towards the corresponding weld toe. The vertical weld element normals should also point towards the corresponding weld toe.

• Two-sided Two Row
For a Two-sided Two Row Cross-Joint, the weld element normal direction should point towards the corresponding weld toe.
• Two-sided Three Row

Multiple rows are recommended for welds where the weld penetration is high and the weld typically forms the basis for contact between the two plates. Such welds are more rigid compared to welds where the penetration is lower, thereby additional rows of weld shell elements are required to capture the behavior. In Figure 14, the welds have penetrated more than the welds in Figure 12.

For a Two-sided Three Row Cross-Joint, the weld element normal direction should point towards the corresponding weld toe. The normals of the vertical weld elements can point towards either weld toe on each side.

### Overlap or Laser Edge Overlap

An overlap weld is a weld joining two overlapped sheets in parallel. Figure 15 shows possible failure locations. OptiStruct evaluates these locations. Typical failure locations are marked in Figure 15. An overlap weld may be modeled by inclined and vertical CQUAD4. Depending on how much the weld penetrates, the weld may be modeled by a single or double row of CQUAD4.

Meshing rules are the same as that for fillet weld. Normal direction of weld element should be toward weld toe. Weld nodes should be along the line of the weld toe. Weld element thickness should be effective weld throat. In laser weld, failure at weld throat is evaluated as well as weld toe and weld root.

#### Two Row Overlap

Multiple rows are recommended for welds where the weld penetration is high and the weld typically forms the basis for contact between the two plates. Such welds are more rigid compared to welds where the penetration is lower, thereby additional rows of weld shell elements are required to capture the behavior. The typical length of the weld element is L=T1+T2.

Typical weld element thickness is about 0.27*L.

#### One Row Overlap or One Row Laser Edge Overlap

For overlap, weld element thickness should be 2 times the thickness of the thinner sheet. Its minimum thickness is 3mm. For laser edge overlap, weld element thickness should be effective weld throat. It is about 0.7* the upper sheet thickness.

#### One Row Overlap or One Row Laser Edge Overlap (Alternative)

The previous weld can also be modeled as shown in Figure 18.

#### Laser Overlap

The thickness of the weld element should be the weld width. The weld width should be 90% of the thickness of the thinner sheet. Its minimum thickness is 1 mm. The laser overlap welds are intended for very thin sheets (> 1 mm).

### Failure Evaluation

Failure evaluation points differ from one weld type to another.

The following sections provide information about which locations of the weld elements are used for failure evaluation in Seam Weld Fatigue Analysis. Figure 20 shows how the identification points are illustrated in subsequent images.

#### Fillet

The weld toe and root locations are evaluated. Throat location is not evaluated.
Note: The arrows in Figure 21 and Figure 22 indicate surfaces for evaluation (surface of the shell elements adjacent to the weld element).

#### Overlap

The weld toe and root elements are marked in Figure 23, Figure 24, and Figure 25. The weld throat is not evaluated.

#### Laser Overlap

The weld throat and root elements are marked in Figure 26. Both sides of the throat element are evaluated because either side of the throat can have a crack.

#### Laser Edge Overlap

Throat location has to be evaluated. Thus weld should be modeled with a single row in order to get a realistic result.

Note the surface where weld throat is evaluated. This surface is determined by normal direction of the weld element.

### Hot Spot Stress

OptiStruct calculates hot spot stress based on grid point force of a toe/root element.

In the original approach suggested by Fermér, Andréasson, Frodin, grid point forces contributed to the element of interest were directly used without any "adjustment". Later research [P. Fransson and G. Pettersson, 2000] showed that averaging grid point forces made grid point forces less mesh sensitive.

The calculation method implemented in OptiStruct includes weighted averaging of grid point forces, as:
1. OptiStruct identifies potential damage locations at weld toe, weld root, weld throat and their evaluation surface from weld elements location and its normal direction (as shown in previous sections).
2. For the corresponding root and toe damage locations (in adjacent elements), and in the throat (in the weld element), local coordinate systems are constructed. The local X axis is constructed in the direction perpendicular to and away from the corresponding weld element face at the center of the adjacent element on the weld line (the X axis is in located in the plane of the adjacent element). The local Y axis is constructed perpendicular to this X axis in the plane of the adjacent element.
3. Grid point forces are calculated at grids (Q and R) of the adjacent element (2) along the weld line. Grid point force contributions are sourced from elements attached (1 and 3) to the adjacent element.
Grid point forces are calculated as:(1) ${f}_{Q}={f}_{Q1}+{f}_{Q2}$ (2) ${f}_{R}={f}_{R2}+{f}_{R3}$
Moments are written as:(3) ${m}_{Q}={m}_{Q1}+{m}_{Q2}$ (4) ${m}_{R}={m}_{R2}+{m}_{R3}$
4. At each node ($Q$ and $R$) of the adjacent element that lies on the weld line, averaged grid point forces/moments weighted by length of the adjacent element and the attached element on the weld toe line are calculated.
Weighted forces are written as:(5) ${f}_{Q}^{RIGHT}=\frac{{L}_{2}}{{L}_{1}+{L}_{2}}{f}_{Q}$ (6) ${f}_{R}^{LEFT}=\frac{{L}_{2}}{{L}_{2}+{L}_{3}}{f}_{R}$
Weighted moments are written as:(7) ${m}_{Q}^{RIGHT}=\frac{{L}_{2}}{{L}_{1}+{L}_{2}}{m}_{Q}$ (8) ${m}_{R}^{LEFT}=\frac{{L}_{2}}{{L}_{2}+{L}_{3}}{m}_{R}$
5. Line Forces and Moments are calculated based on the weighted grid point forces and moments. These line forces and moments from both ends of the adjacent element on the weld line are averaged to generate the line force and moment at the midpoint ($L$).
Line Forces are calculated as:(9) ${f}_{LQ}^{RIGHT}=\frac{2}{{L}_{2}}\left(2{f}_{Q}^{RIGHT}-{f}_{R}^{LEFT}\right)$ (10) ${f}_{LR}^{LEFT}=\frac{2}{{L}_{2}}\left(2{f}_{R}^{LEFT}-{f}_{Q}^{RIGHT}\right)$
Line Moments are calculated as:(11) ${m}_{LQ}^{RIGHT}=\frac{2}{{L}_{2}}\left(2{m}_{Q}^{RIGHT}-{m}_{R}^{LEFT}\right)$ (12) ${m}_{LR}^{LEFT}=\frac{2}{{L}_{2}}\left(2{m}_{R}^{LEFT}-{m}_{Q}^{RIGHT}\right)$
The averaged line forces and moments at the midpoint, $L$, for element 2 are:(13) ${f}_{2}=\frac{{f}_{LQ}^{RIGHT}+{f}_{LR}^{LEFT}}{2}$ (14) ${m}_{2}=\frac{{m}_{LQ}^{RIGHT}+{m}_{LR}^{LEFT}}{2}$
6. The line force and moment at the midpoint are then resolved in the local coordinate system constructed in step 2 to generate ${f}_{2X}$ and ${m}_{2Y}$ respectively. This force and moment pair leads to tensile and bending stresses in the adjacent element with respect to the weld line. These are the forces that are used to calculate stresses.
7. Stresses are then calculated normal to the weld line for the adjacent element from this force moment pair. Stresses are calculated for both top and bottom of the shell element, and depending on the type of weld, either one or both are used for fatigue calculations. This is the final hot spot stress used in further S-N Fatigue Damage Evaluation. For addition information, refer to Stress-Life (S-N) Approach.(15) ${\sigma }_{TOP}=\frac{{f}_{2X}}{T}+6\frac{{m}_{2Y}}{{T}^{2}}$ (16) ${\sigma }_{BOTTOM}=\frac{{f}_{2X}}{T}-6\frac{{m}_{2Y}}{{T}^{2}}$

### Fatigue Properties

There are a few fatigue properties relevant to Seam Weld Fatigue Analysis that allow you to control the fatigue behavior.

#### Bending Ratio

Experiments show that two types of SN curves are required to perform Seam Weld Fatigue Analysis based on a method suggested by M. Fermér, M Andréasson, and B Frodin. Based on lab tests, two SN curves were plotted (Figure 29). The upper curve is obtained in tests where the maximum stress is dominated by Bending Moment (${m}_{2Y}$) and the lower curve is obtained from tests where membrane force (${f}_{2X}$) dominates the maximum stress.

The upper and lower curves are referred to as Bending SN curve and Membrane SN curve, respectively. It is recommended that membrane SN curve should be used when membrane stress dominates in an element, and bending SN curve should be used when bending stress dominates. Interpolation between the two curves may be carried out depending on the degree of bending dominance.

Degree of bending dominance can be determined by the average bending ratio (${r}_{B}^{AVG}$). First, the bending ratio ($r$) is defined as:(17) $r=\frac{|{\sigma }_{B}|}{|{\sigma }_{B}|+|{\sigma }_{M}|}$
Where,
${\sigma }_{B}$
Maximum bending stress equal to $6\frac{{m}_{2Y}}{{T}^{2}}$
${\sigma }_{M}$
Maximum membrane stress equal to $\frac{{f}_{2X}}{T}$
The average bending ratio (${r}_{B}^{AVG}$) for an element is defined as:(18) ${r}_{B}^{AVG}=\frac{\sum _{i=1}^{n}\left({r}_{i}{\left[{\sigma }_{TOP}^{2}\right]}_{i}\right)}{\sum _{i=1}^{n}{\left[{\sigma }_{TOP}^{2}\right]}_{i}}$
Where,
${\left[{\sigma }_{TOP}^{2}\right]}_{i}$
Square of the maximum stress at the top surface of shell element $i$ at which the damage is calculated (that is, root, toe, or throat shell elements)
${r}_{i}$
Bending ratio of shell element $i$.

is the

An interpolation factor ($IF$) is now defined as:

$IF=0.0$ when $0.0\le {r}_{B}^{AVG}\le {r}_{B}^{CRIT}$

$IF=\frac{{r}_{B}^{AVG}-{r}_{B}^{CRIT}}{1-{r}_{B}^{CRIT}}$ when ${r}_{B}^{CRIT}<{r}_{B}^{AVG}\le 1.0$

The ${r}_{B}^{CRIT}$ value is defined by the BRATIO field on the PFATSMW Bulk Data Entry. It is set to 0.5 by default. If average bending ratio (${r}_{B}^{AVG}$) is less than or equal to the critical bending ratio (${r}_{B}^{CRIT}$), then the Membrane SN curve is used to assess damage. If average bending ratio is greater than the critical bending ratio, then an SN curve that is interpolated between membrane SN curve and the bending SN curve is used. The value of the interpolation factor ($IF$) is used in the linear interpolation method as illustrated in Figure 30. For example, if you consider the Fatigue Strength coefficient value (SR1_i) for the interpolated curve, the calculation is performed as:(19) $SR1_i=\left[SR1_m+\left(SR1_b-SR1_m\right)IF\right]$

#### Thickness Correction

The thickness correction process is for size effect correction. SN curves are based on test results from a particular size of the specimen. In reality, the stress versus life curve may vary depending on specimen size. Therefore, thickness correction parameters can be used to correct for this effect. It may be applied based on the thickness $T$ of each shell element under consideration for Fatigue calculation (that is, toe, root, or throat element). The calculations are:

If $T\le TREF$, then there is no Thickness Correction.

If $T>TREF$, OptiStruct increases stress based on OptiStruct:(20) ${\sigma }_{TOP/BOTTOM}={\sigma }_{TOP/BOTTOM}{\left(\frac{T}{TREF}\right)}^{TREF_N}$

This results in fatigue life reduction, making the design more conservative. TREF and TREF_N can be defined via the corresponding fields on the PFATSMW Bulk Data Entry. The default values are 1.0 and 0.2 respectively. The defaults are in inches (English units). If the metric system is used, then the values should be modified accordingly.

Thickness Correction can be turned on or off using the corresponding THCKCORR field on the FATPARM Bulk Data Entry for Seam Weld Fatigue Analysis.

#### Mean Stress Correction

FKM mean stress correction is supported for Seam Weld Fatigue. Stress sensitivity can be defined on the MATFAT Bulk Data Entry via the FKMMSS_SM field. Mean stress correction for Seam Weld fatigue is disabled by default and can be enabled via the corresponding CORRECT field on the FATPARM Bulk Data Entry.

### Input/Output

To activate Seam Weld Fatigue Analysis, FATDEF has to have a FATSEAM and PFATSMW identifier.

#### Fatigue Element Identification

1. The FATDEF Bulk Data and Subcase Information Entries can be used to identify the elements for which fatigue analysis should be performed. For seam weld fatigue, the FATSEAM and PFATSMW entries should be referenced on the FATDEF entry. The FATSEAM entry identifies the corresponding shell elements (CQUAD4 and CTRIA3) for which fatigue analysis is to be performed.
2. The FATDEF Bulk Data Entry also provides the corresponding PFATSMW Bulk Data Entry references for each FATSEAM entry set to define the seam weld fatigue properties.

#### Fatigue Parameters

1. The FATPARM Bulk Data and Subcase Information entries can be used to specify fatigue parameters for the seam weld fatigue analysis.
2. The SMWLD continuation line on the FATPARM entry allows you to input the seam weld fatigue method and identify various parameters.
3. The PFATSMW Bulk Data Entry allows the definition of some properties for seam weld fatigue analysis.

#### Fatigue Material

1. The MATFAT Bulk Data Entry can be used to specify the material properties for seam weld fatigue analysis.
2. The SMWLD continuation line allows you to specify mean stress sensitivity value, and separate SN curve attributes for bending and membrane SN curves. Bending SN curve and membrane SN curve may be defined in MATFAT after a flag SMWLD. If only one SN curve is defined for seam weld, it is used as both bending SN curve and membrane SN curve.

1. Similar to regular fatigue analysis, the FATLOAD, FATSEQ, and FATEVNT entries can be used to define loading sequences.

#### Optimization

1. The PTYPE field on the DRESP1 entry can be set to FATSEAM and the ATTi fields should be FATSEAM identification numbers for seam weld fatigue optimization.

## Joint Line Method

### Supported Weld Types

OptiStruct supports certain types of welds for Seam Weld Fatigue Analysis using the Joint Line method.

The type can be selected using the WTYPE field on the FATSEAM Bulk Data Entry.
• The Weld elements should not be modeled when using the Joint Line method
• All elements sharing the same weld line and REFEID should have consistent element normals which match with the element normal identified by the corresponding REFEID element
• The damage calculation locations only consist of the toes of the welds and they are based on the evaluation distance (EVALDIS field on PFATSMW entry) as explained below.