Effect of Residual Stresses on Design Assessment of Partial Penetration Laser Welds in a Pressure Valve Component

     The construction of the valve component includes joining the cap, the outlet and the inlet fittings to the valve body using the laser welding process. This valve component is made of 316L stainless steel and designed for 500 lb/in.² (3.4 MPa) maximum operating pressure. Autogenous CO₂ welds are made along the circumference of the fitting edges. During the proof tests, this valve component must sustain 750 lb/in.² (5.2 MPa) proof pressure and 1250 lb/in.² (8.6 MPa) burst pressure. Sufficient weld penetration is required to resist these pressures. The weld penetration ranging from 0.02 to 0.04 in. (0.50 to 1.0 mm) is recommended by the current design specifications. The allowable clearance between the fitting surfaces is 0.001 in. (0.025 mm) 

Material Properties  

     Material properties of the 316L used in this design analysis are summarized as follows:  
     Mechanical Properties (Ref. 4). Minimum yield strength, 25 ksi (173.4 MPa); minimum ultimate tensile strength, 70 ksi (482.6 MPa); elongation for cold rolled, 40%; and 45% for hot rolled; and 50% minimum reduction in cross-sectional area. For the flow stress-strain relationship, a linear strain hardening exponent of 0.165 is assumed. The flow stress-strain relationship terminates at fracture strain (0.4 strain).  
     Fracture Properties (Ref. 5). Charpy V-notch impact: 25 ft-lb (33.9 J), weld; 69 ft-lb (93.6 J), heat-affected zone; and 109 ft-lb (147.8 J), base metal, at -440°F (-262° C) and the translated critical stress intensity factor, using Barsom's two-stage and other methods described by Barsom and Rolfe (Ref. 3), would be 69 ksi (in.)^1/2 at the same temperature. In a real situation, the stress intensity factor will be a lot higher than 69 ksi (in.)^1/2 because the room or operating temperatures are much higher than -440°F.  
     Fatigue Properties (Ref. 3). Fatigue propagation threshold of steel is 5.5 ksi (in.)^1/2 for pulsating pressure variations and the fatigue crack propagation equation in room temperature and air environment is  

(1)

Design Evaluation Criteria   

     The design variables analyzed in this project include 1) weld penetration varying from 0.02 to 0.04 in. and 2) pressure loading varying from 500 lb/in.² to actual rupture pressure for each weld penetration in the cap fitting. The ANSYS finite element program (Ref. 6) was used for the stress analysis of each design condition. The design evaluation criteria consist of the following:  
     1) The minimum required weld penetration for all valve fittings is 0.02 in. This serves as a baseline for design evaluation.

Finite Element Model  

     Figure 1 shows the valve system from a 45-deg view angle and a plane view of the valve system. Three axisymmetric fitting components, cap, outlet and inlet are connected to the valve body. As mentioned previously, only the joint between the cap and valve body will be discussed. Figure 2 shows the finite element meshes and the boundary conditions of the fitting component isolated from the valve system for analysis. Refined meshes were used in the weld area and singular elements were used around the tip of the root opening - Fig. 3. A root opening of 0.001 in. was used in the models. The boundary conditions include pressure loading at the internal surfaces, axisymmetry along the central axis, restraint in the axial (parallel to the axis of symmetry) displacement at the threaded contact points, and simple supports along the cut-off sections of the finite element analysis (FEA) model. The ANSYS code was used for the analysis.  
     The sux-node triangular solid elements (ANSYS plane 2 element type) were used in the models. This type of element has quadratic displacement shapes, which fit well with the irregular boundary geometry. These types of elements can be assigned as either plane stress, plane strain, or axisymmetric elements with or without thickness input. The axisymmetric condition was assigned to the element in this design analysis. The singular point at the crack tip was treated by the concept of quarter point element (Ref. 8). This is a conventional finite element in which the mid-side node is shifted to reflect the singular behavior in elastic crack problems. The stress in the crack tip is calculated by extrapolating the stresses at the nodes around the crack tip.

Fig. 2 - Finite element model for cap to body weld.  
  
  

Fig. 3 - Refined crack tip model.  
  
 

 (2) 

where G is shear modules, r is the radius from the crack tip and k = 3-4v for plane strain and plane stress. For symmetry at the crack plane, Equation 2 can be reorganized to give  
  

 (3) 

For nonsymmetry, Equation 2 will be  
  

 (4) 

 (5) 

and calculating A and B by the displacements of point J and K, then the stress intensity factor at the crack tip can be represented as  
  

(6) 

     For elastic-plastic analysis, instead of the stress intensity factors K, the J-integral around the tip is the criterion to determine fracture. Assuming that the crack lies in the globe Cartesian X-Y planes, with X parallel to the crack, the J-integral can be expressed as Equation 7  
  

 (7) 

where  = any path around the crack tip,  W = strain energy density, t_x = traction vector along x axis =  = traction vector along y axis =  * = component stress, n = unit outer normal vector to path , s = distance along the path .  
  

Fig. 4 - The Von Mises equivalent stress at the crack tip. (weld pentration, 0.02 in.; stress unit, psi.)  
  

Fig. 5 - The Von Mises equivalent stress at crack tip. (weld pentration, 0.04 in.; stress unit, psi.)

 (8) 

where E'= E for plane stress and E'= E/(1-v²) for plane strain and axis symmetry.  
      The inherent shrinkage strain method (Ref. 7) was applied to calculate the residual stresses. A thermal analysis was performed first by assuming that the initial temperature at the weld was 1500°F (816°C) and the base metal and surrounding air had initial temperature 70°F (21.1°C). The temperature dependent material properties, such as conductivity, specific heat and thermal expansion coefficient were considered in the analysis. The temperature at the weld gradually cooled down to the room temperature (70°F) because of the effects of conduction and convection. The temperature distributions during the cooling period were considered as the thermal loads in stress analysis. An elastic-plastic analysis procedure was performed to determine the equilibrium between the weld shrinkage and the structural rigidity of the valve fitting.  

Results and Discussion  

     Two FEA procedures, linear-elastic and elastic-plastic, were conducted in this study. The linear-elastic analysis was to determine the stress intensity factors of opening mode (K_I) and sliding mode (K_II), as well as their combined effect on weld fracture using the effective stress intensity factor (K_eff). The elastic-plastic analysis was used to determine the yield load, the ultimate load, and the rupture load of the weld joints. It was also used to determine the residual stresses and their effects on the J-integral and the effective stress intensity factor.  
 The discussions below consist of results without the consideration of residual stresses and results with the consideration of residual stresses.  

Results without the Consideration of Residual Stresses  

Von Mises Equivalent Stress Map  

     Figures 4 and 5 show the equivalent stress maps in the weld section of the cap valve fitting at the design load (maximum operating load at 500 lb/in.²). Only the results from analysis of two weld penetration depths, 0.020 and 0.040 in., are shown. Equivalent stress distributions for other penetration depths have a similar pattern but the size of the constant stress zones falls between these two extreme penetration cases.  
     The average equivalent stress in the weld section is between 5 and 10 ksi. Higher stress areas are at the root of the weld and at the top surface. The maximum stress for 0.040-in. weld penetration is between 20 and 24 ksi at the weld root and is less than 15 ksi at the top surface. For 0.020-in. weld penetration, the maximum stress is approximately yield stress (25 ksi) at the weld root where a small amount of plastic deformation is present. Stress at the top surface is between 15 and 20 ksi. The high-stress zones are small in both penetration cases.  
     From the stress pattern at the root of weld penetration, the tensile stress is significant in opening up the root. This root opening is also subject to a strong influence of shear stresses. This is referred to as Mixing Mode fracture characteristics.  

Load Parameters for Design Evaluation by Elastic-Plastic Stress Analysis  

     Figure 6 shows three load parameters for design evaluation of various weld penetrations. The rupture loads and ultimate loads are almost at the same value of 2500 lb/in.². This is because the large strain will occur when the plastic hinge is formed. The yield load is below 500 lb/in.² when the penetration is less than 0.030 in. When the penetration is larger than 0.030 in., there is no yielding under the operating pressure (500 lb/in.²). It is the common engineering practice to consider the ultimate load as the limiting capacity of the valve components to sustain the pressure. The rupture load is typically used for a safeguard to prevent rupture of the components from unexpected overloading. It is also used to relax the quality control requirement during manufacturing of the valve system. Yield load is used to determine when the weld section will begin the plastic deformation process. Local plastic deformation stabilizes the root opening due to blunting the opening tip. Excessive yielding conditions in the weld section is guarded by checking the ultimate load. Therefore, no alarm is necessary if local plastic deformation is shown at the root of the weld penetration, as the general yielding failure is the only concern. For fracture and fatigue analysis, attention should be given to the local high stress zone because stress concentration will affect the fatigue and fracture characters.  
     To determine the factor of safety of various weld penetrations in the valve component, the ultimate loads are divided by the design load, which is the maximum operating pressure at 500 lb/in.². Table 1 summarizes the factor of safety values. The factor of safety varies from 4.76 (0.020-in. penetration) to 5.00 (0.035-in. penetration). The factor of safety commonly used in engineering design is between 1.5 and 2 depending on the confidence level with respect to the reliability issues. Therefore, any weld penetrations not less than 0.02 in. are acceptable  

Fracture Stability of Partial Penetration Welds  

     Figure 7 shows the stress intensity factors at the root opening tip of the weld at the burst pressure of 1250 lb/in.². The stress intensity factors were plotted vs. the weld penetration.  
     All the predicted stress intensity factors are less than 11% of the critical stress intensity factor of 316L stainless steel, which is 69 ksi (in.)^1/2 at -440°F and is expected to be greater than the value at room or higher temperatures. Therefore, it is concluded that any weld penetrations not less than 0.020 in. are free of sudden fracture under the burst load at 1250 lb/in.².  
     To determine any penetration reduction due to cyclic pressure variations during service life of the valve system, the effective stress intensity factor range, K_eff, is compared with the fatigue propagation threshold, which is 5.5 ksi (in.)^1/2 for 316L stainless steel. Weld penetration in the cap welds may be reduced by growth of the root opening towards the top surface under the repeated pressure variations.  
     Paris's crack propagation law for austenitic stainless steel was used to determine the root opening growth. The effective stress intensity factor ranges for the propagating root openings were determined numerically from Fig. 7. An integration procedure using Paris's crack propagation law was then conducted over the penetration depth range from 0.04 to 0.02 in. with a decrement of 0.005 in. (0.127 mm) Figure 8 shows the cumulative pressure load cycles needed for any of the intermediate penetration depths, propagating to the final 0.02 in. in the cap welds. Under normal operating conditions (not exceed 500 lb/in.² maximum operating pressure) it would take approximately 3 million cycles for the cap weld to reduce the penetration from 0.04 to 0.02 in.  

Fig. 8 - cumulative load cycles needed for weld pentration, decreasing to 0.02 in.  

Results with the Consideration of Residual Stresses   

     Residual stress comes from shrinkage of the weld. To show typical stress distributions, the residual stresses along the weld centerline in the cap fittings were plotted against the normalized weld penetration in Fig. 9. The zero distance represents the weld surface and the unit distance represents the root of the welds. Three stress components, longitudinal, radial and circumferential, were plotted for the 0.02 and 0.04-in. penetration cases. 

Residual Stress Effects  

     Figure 9 shows high compressive stresses at the weld root in a radial direction. It implies that the residual stress could close the root opening, improving the fracture stability at the root. Table 2 shows the J-integral and effective stress intensity factors at different loads. It can be observed that when the load is less than 750 lb/in.², the J-integral is negative, which means that the compressive radial residual stress keeps the root opening closed and no fracture is expected. When the applied load is large enough (e.g. 1250 lb/in.²), the compressive residual stress will be overcome by the load, which tends to open the root. The outward load will interact with the tensile residual stress at the midsection of weld, so the effective stress intensity factors will be larger than the factors that do not consider residual stress. Although the effective stress intensity factor becomes larger, it still is less than the critical stress intensity factor. Therefore, the valve is stable at burst pressure.  

Fig. 9 - Distribution of radial, circumferential and longitudinal residual stresses along the cross section of the cap weld fitting.  

Fig. 10 - Residual stress's effect on rupture load and ultimate load (cap fitting).  

Experiment Verification  

     The joined cap and valve body was tested under 500 lb/in.² design load, 750 lb/in.² proof load and 1250 lb/in.² burst load. Hydraulic oil was used to pressurize the component. After reaching the expected pressure, the pressure was held more than one minute to observe and record any visible rupture. Figure 11 shows the pressure change during these tests. It can be observed that the variation is very small after pressure reached the expected values and that also implies the current design for weld penetration can resist the applied loads. These results verify the FEM analysis.  
     A fatigue test was also perform under the design load (500 lb/in.²). The pressure was gradually increased from 0 to 500 lb/in.² and backed to 0 lb/in.² for one thousand cycles with hydraulic oil. Any visible outside damage was recorded. The fatigue test shows the component can operate more than one thousand cycles under the design load. This result also matches the FEM's life perdition.  
    The maximum load that the component can resist was obtained by pressurizing the component with hydraulic oil until it ruptured. Figure 11 shows the maximum load is about 4450 lb/in.². The rupture pressure is higher than the predicted pressures from FEM analysis, which were about 2500 lb/in.² when residual stress was not considered and 1500 lb/in.² when residual stress was considered. The predicted rupture pressure was decided as the lowest load that has the stress higher than the tensile strength of the material. This is a conservative prediction because more load is needed for total rupture after the incipience of plastic fracture. Another reason of the difference maybe comes from the change of material properties during processing and assembling. Although there is some difference, the results from FEM analysis can provide the lower band of rupture load.  
 

Fig. 11 - Experiment results of cap and value body joint under different load.  

Conclusions  

     Several conclusions can be obtained from the FEM analysis results.  
     1) No welds within the specified penetration range of 0.02 to 0.04 in. will fracture at the burst pressure (1250 lb/in.²).  
     2) The minimum factor of safety of welds in the valve body at the maximum operating pressure is three.  
     3) Any weld penetration equal to or greater than 0.030 in. will not result in plastic deformation under the maximum operating pressure (500 lb/in.²). At this pressure level, yielding just begins to occur at the root of the weld if the penetration depths are smaller than 0.030 in.  
     4) Under repeated loading and unloading pressure variations between zero and 500 lb/in.², it would take 3 million cycles for the cap weld to reduce its weld penetration from 0.040 to 0.020 in.  
     5) No failure is anticipated to occur in any of the weld penetrations not less than 0.020 in. during proof testing.  
     6) Welding-induced compressive residual stresses will stabilize the crack at the root of the weld when the pressure is low. When the applied pressure places the weld root in tension, the outward load will interact with the tensile residual stress at the midsection of the weld to make the component more fracture sensitive.  
     7) Residual stress will change the plastic zone's size and pattern. Due to the expansion of the plastic zone, the ultimate load and rupture load of the welding component will decrease.  
     8) It is concluded that weld penetration of 0.02 in. in the valve fittings investigated in this project is adequate for normal service use. However, for a more conservative design to relax the postweld inspection requirement or to protect the valve system from unexpected overloading, a minimum of 0.030-in. weld penetration is recommended. 

1. The American Society of Mechanical Engineers. 1992. ASME Boiler & Pressure Vessel Code, Sections VIII and IX, New York, N.Y.  

2. Lipson, C. 1969. Basic Course for Failure Analysis, Penton Education Division, Cleveland, Ohio.  

3. Barsom and Rolfe. 1987. Fracture & Fatigue Control in Structures, 2nd Edition, Prentice-Hall, Englewood Cliffs, N.J.  

4. QQ-S-763E: Federal Specification on Steel Bars, Wire, Shape, Forgings, and Corrosion Resistance.  

5. Peckner and Bernstein. 1977. Handbook of Stainless Steels, McGraw-Hill, pp. 19-2 to 19-26, 21-5 to 21-6.  

6. ANSYS 5.0. 1992. User's Manual, Analysis Systems, Inc., Houston, Pa.  

7. Ueda, Y., et al. 1986. Simple prediction methods for welding deflection and residual stress of stiffened panels. Trans. JWRI 15(2): 197-204.  

8. Henshell, R. D., and Shaw, K. G. 1975. Crack-tip finite elements are unnecessary. International Journal for Numerical Methods in Engineering, 9, pp. 495-507.  

9. Kanninen, M. F., and Popelar C. H. 1985. Advance Fracture Mechanics, Oxford University Press, New York, N.Y.