How often have you been faced with the task of performing Finite Element Analysis (FEA) on a welded component? Have you wondered how to properly model welds in that analysis? This article is meant to explain the method we use at Apollo Engineering Design Group to model and predict stress in a weld using the Hot Spot method. We will then explore a few different options that one might choose to model welds and compare to the results obtained using the Hot Spot Method.

**A Quick Review of Fillet Weld Terminology**

**Terms:**

**Toe**– the outer edge of the weld where the parent material and the weld material meet.**Root**– the point opposite the weld face where the weld material and the parent material meet.**Leg**– The distance from one face of the parent material to the opposite Toe**Material Thickness**– an important parameter for the Hot-Spot Method (discussed later).

Labeled in the image above are specific terms related to a fillet weld and relevant in an FEA model. For complete fillet weld terminology, refer to a previous blog post **Right Down the Weld’s Throat**.

**The Near IMPOSSIBILITY of Predicting Weld Stress**

Before delving into FEA of a fillet weld joint, it’s important to understand a few things about weld stress. First and foremost, stresses in welds are nearly impossible to predict with a high degree of accuracy. The theoretical weld size specified in drawings, FE models, and other analyses will rarely be a reality. Welding is a mostly manual process subject to error at many levels, including the chemical makeup of the parent material, weld size and shape, and the unique method and setup of each individual welder. No two welds are exactly alike, and rarely will a physical weld match exactly an engineer or designer’s theoretical model. For this reason, welded joints compliant with common industry standards, such as AWS and AISC, generally have a lower allowable stress for fatigue scenarios.

**Deviations from Theoretical Model:**

**Base Material**– This includes variation in chemical makeup, surface imperfections, local corrosion, etc.**Heat-affected Zone**– The weld and base material heat and cool at different levels and rates causing variations in hardness and strength along the length of the joint.**Microcracking**– Small cracks may form as part of the welding process.**Warping**– Heating and then cooling through the affected area near the welded joint causes the base material to distort.**Residual Stress**– Due to the cooling rate, thermally induced stresses may remain in and around the joint.

**The Problem with Singularities**

Aside from recognizing the pitfalls associated with predicting weld stress using an FEA model, it is just as important to understand the complexities of interpreting that same stress. Generally speaking, weld representation in FEA models produces sharp corners which leads to discontinuities and/or non-converging geometry. These discontinuities often cause singularities on nearby nodes.

A singularity is a point in the mesh where the stress does not converge towards a specific value. As the mesh is refined, the stress at this point increases with no apparent limit. Theoretically, the stress at the singularity is infinite. An FEA analyst must recognize these singularities in the model and interpret them correctly.

The contour plots below demonstrate singularities in a welded T-joint model:

**Plate thickness –**1/4 in**Weld Representation**– Chamfer**Boundary Conditions**– Fixed at base plate edges**Loading**– [50,50,50] lbf applied to the top edge

**Initial Simulation:**

An initial simulation reveals a max stress of **4474.6 ps**i.

**1st Refinement:**

Refining the mesh and rerunning the simulation shows a max stress of **5515 psi**.

**2nd Refinement:**

A second refinement increases the max stress to **7313.7 psi**.

**3rd Refinement:**

The final refinement shows yet another increase in max stress to **8783.1** psi.

A convergence plot shows how each simulation increases the stress by roughly 20%. This is a classic example of singularities in a finite element model. The high stresses along the edge of the weld cannot be considered accurate.

**The Hot Spot Method**

As mentioned previously, because of singularities existing in FEA weld models, a method known as the hotspot method is used as a reliable means of predicting the stresses at the toe of the modeled welds. The theory of the hotspot method is well documented and tested. *See Fatigue Design of Plated Structures Using Finite Element Analysis: Lotsberg*.

In short, the stresses derived from the Hot Spot Method are linear interpolations of the stresses present at the toe of the weld. Typically the weld is included in the FEA model as a chamfer. In the following example, we will use a chamfered fillet to represent the weld and to identify the weld toe.

Two stress measurements are taken, each offset from the weld toe (as shown). Lotsberg suggests that the two measurements be taken at a distance of T/2 and 3T/2 from the nearest weld toe (T = plate thickness).

Taking the two measurements from the FEA model above, we use the following calculation to solve for an interpolated Hot Spot Stress. As seen below, the calculated hotspot stress of **4881.7 psi** will be used as the “baseline stress” to which the following FEA model results will be compared.

**Other Ways to Model Welds WITHOUT Using the Hot Spot Method**

We conducted a test using 5 different FEA models, each refined using the same mesh size and type (0.05 in hex elements), and each under the same loading condition performed in the Hotspot FEA model described above. We took stress measurements from each model at the location where the toe of the weld would be if modeled and then compared the results to our baseline established using the Hot Spot Method (shown above).

**Simulation 1**

(Single-body. No weld.)

**Simulation 2**

(Two bodies. No modeled welds. Single bonded contact.)

**Simulation 3**

(Single-body. Welds modeled as chamfers.)

**Simulation 4**

(Single-body. Welds modeled as fillets.)

**Simulation 5**

(Multi-body. Welds modeled as triangle extrusions. Bonded contact between welds and plates. Frictionless contact between plates.)

**Conclusion**

Comparing the results from this idealized test, we see that the most accurate reading was from Simulation 5 with a stress reading deviation of 3.7% . The next closest reading was Simulation 4 followed by Simulation 3. Simulations 1 & 2 had the highest deviations and incidentally, were the only models that did not represent the weld with a solid body. It is difficult to say which method yields the best results and how the above results may be applied to more complex FEA models. Mesh type, element size, and the presence of singularities all play a part in the final result. However, in the above study, Simulation 5 produced the best results.

One thing does stand out: If the analyst decides against using the Hot Spot Method to analyze FEA weld stress results, it would be more accurate to include model welds rather than no welds at all. In complex weldments, this often proves impractical. Therefore, understanding the potential error in simplifying the FEA model is key.