Numerical Simulation Study on Welding Process of Upper Frame of Hydropower Unit

Abstract

To optimize the welding process of the upper frame of the hydropower unit, a thermal elastic–plastic (TEP) finite element model of the typical T-joint of the upper frame was established, and the effectiveness and accuracy of the model were verified by welding tests. The effect of welding speed and interlayer cooling time on welding residual stress and deformation was analyzed, and a welding process in line with the requirements was obtained. Based on the results of the TEP calculation, the inherent strain was obtained, and the inherent strain method (ISM) was used to predict the overall deformation of the upper frame under three welding sequence schemes, and the optimal welding sequence was obtained.

1. Introduction

The hydropower unit is the core mechanical device for hydropower energy development and utilization, and its manufacturing quality is directly related to the efficiency of hydropower energy extraction and conversion. The upper frame is the key structural component of the hydropower unit, which plays the role of supporting and guiding the shafting of the hydropower unit. The upper frame is mainly formed by welding, and welding residual stress and deformation will inevitably occur after welding, and large residual stress and deformation will reduce its structural strength and stability, thus affecting the overall performance of the unit [1]. The upper frame structure is shown in Figure 1.

Therefore, it is necessary to study the welding process of the upper frame in order to reduce the residual stress and deformation and improve the service life and operation safety of the unit. With the development of computer technology and finite element theory, numerical simulation can accurately simulate the welding process, thus reducing the test cost and improving the welding quality [2]. Therefore, this paper adopts numerical simulation methods to study the welding process of the upper frame of a hydropower unit and predict its welding deformation.

Currently, the thermal elastic–plastic method (TEPM) and inherent strain method are the two main methods in the field of welding numerical simulation. Professor Ueda [3] of Osaka University in Japan was the first to propose the TEP finite element method (FEM) and applied it to two-dimensional and three-dimensional finite element models to simulate the stress–strain field during the welding process. Since then, with the improvement of computer performance and the emergence of professional simulation software, researchers have conducted more in-depth research based on the TEP-FEM and have achieved abundant research results. Deng et al. [4] simulated the welding deformation of fillet welds using the TEPM and verified its effectiveness through experiments. Capriccioli et al. [5] used the TEPM to simulate multi-pass welding, taking into account heat convection and radiation, and obtained relatively accurate results. Sun et al. [6] used the TEPM to simulate the laser-MIG hybrid welding process. They compared the weld pool shape, residual stress, and deformation obtained from the simulation and tests, which were in good consistency. Li et al. [7] established a three-dimensional finite element model based on the TEPM to study the effects of different bevel shapes on the residual stresses of dissimilar metal welding and carried out the residual stress detection using the blind hole method, which showed that the simulation results were in good agreement with the test.

At the same time, numerous scholars have conducted extensive research on the effects of the welding process on both the temperature and stress–deformation fields. Zubairuddin et al. [8] investigated the impact of preheating temperature on welding residual stress in P91 steel and discovered that preheating to 200 °C can effectively reduce both residual stress and deformation. Ghafouri et al. [9] developed a three-dimensional TEP finite element model and found that external constraints have a greater effect on the final residual stress and deformation of fillet welds than the welding sequence. Raftar et al. [10] investigated the effects of plate thickness, welding sequence, and leg size on residual stress and deformation in cross-shaped welded structures using numerical simulation. The results were found to be in close agreement with the experimental data. Hu et al. [11] used ABAQUS to simulate the welding process of an aluminum alloy bicycle frame, optimized the welding process parameters, and verified the effectiveness of the welding process through experiments.

The TEPM can obtain relatively accurate calculation results of temperature and stress–deformation fields. However, due to its complex calculation process, high hardware requirements, and extended calculation time, it is only suitable for small structures or typical joints to carry out process research, and it is difficult to be used in the prediction of the overall weld deformation of large structural components.

In this regard, the Japanese scholar Ueda [12,13] was the first to introduce the concept of inherent strain, positing that welding residual stress and deformation during the welding process are caused by inherent strain. For large and complex welded structures, only the inherent strain needs to be calculated, and then the residual stress and welding deformation can be obtained through a linear elastic calculation [14]. Since then, many scholars have begun using the ISM to predict welding deformations [15,16,17]. Vishvesha et al. [18] used the ISM to predict the welding deformation of the turbine guide vane’s outer ring. The results of the calculations matched the experimental measurements well, and the deformation of the outer ring was reduced by changing the welding sequence. Lu et al. [19] applied the inherent strains extracted from the TEP calculation results to solid and shell mesh models, respectively, and confirmed that accurate results can also be obtained by using the shell mesh model for the calculation. Wu et al. [20] introduced an equivalent thermal strain method for predicting welding deformation in thin metal plates, building on inherent strain theory. Test verification and comparison revealed that this method offers high calculation accuracy and requires a short computation time. Zhou et al. [21] summarized an empirical formula for the inherent strain in the lifting platform using the TEPM. The results from elastic calculations matched the measured data well, and the welding deformation of the platform was effectively controlled by modifying the welding sequence.

Based on the analytical properties of TEPM and ISM, the welding process of the upper frame of the hydropower unit is studied in this paper. Based on the weld structure type of the upper frame, typical T-joints were simulated using the TEPM, and the influence of welding processes such as welding speed and interlayer cooling time on the temperature field and stress field was studied. The welding process meeting the requirements was obtained, and the accuracy of the established finite element model was verified by experiments. The optimal welding sequence of the upper frame is determined by using the ISM, which can provide a reference for the actual welding of the upper frame.

2. Experiments

The structure of the T-shaped test plate used in welding test is identical to that of the upper frame; neither side is beveled, and the welding gap is 0. The dimension of the flange is 200 mm × 200 mm × 20 mm, the dimension of the web is 200 mm × 100 mm × 20 mm. When welding the T-shaped test plate, three weld seams were welded on each side of the web, totaling six weld seams. Figure 2 illustrates the size of the test plates, the distribution of weld passes, and the welding sequence.

The material of the test plate is the same as that of the welding base material of the upper frame of the hydropower unit, which is Q345 structural steel. The filler wire used is ER50-6 solid core wire with a diameter of 1.2 mm. The chemical composition of the Q345 steel and ER50-6 welding wire is detailed in

Table 1. Chemical compositions of the Q345 steel and ER50-6 welding wire.

Material	Chemical Composition (%)
	C	Mn	Si	P	S	N	Cu	Cr	Ni	V
Q345	≤0.20	≤1.60	≤0.55	≤0.025	≤0.010	≤0.010	≤0.55	≤0.30	≤0.012	≤0.15
ER50-6	0.06–0.15	1.40–1.85	0.80–1.15	≤0.025	≤0.025	-	≤0.020	≤0.15	≤0.015	≤0.03

.

Semi-automatic MAG shielded welding technology was used, with a shielding gas mixture of 80% argon and 20% carbon dioxide. The welding test was conducted using a YD-500FR2 welding machine. The specific welding process parameters are shown in

Table 2. The specific welding process parameters.

Welding Sequence	Current/A	Voltage/V	Welding Speed/ (mm·s−1)	Gas Flow Rate/ (L·min−1)
1, 2	260~270	28~29	6.67	20~25
3, 4, 5, 6	260~270	28~29	4.50	20~25

.

Five K-type thermocouples were arranged on the surface of the welded flange plate to acquire temperature data. The size of the welding foot of the T-shaped joint on the upper frame is approximately 12 to 14 mm. To avoid interfering with the welding process, to prevent the arc from damaging the thermocouple’s temperature measurement junction, and to ensure the temperature did not exceed the measuring range, the thermocouples were placed 20 mm and 30 mm away from the web’s edge, as depicted in Figure 3.

The residual stress was measured by blind hole method. Five points near the weld and parallel to the welding direction were selected for residual stress measurement, with each point 20 mm apart, as shown in Figure 4.

3. Simulation Analysis of T-Joint Welding Based on TEPM

3.1. Finite Element Modeling

According to the size of typical welded T-joint samples, 1:1 modeling and meshing were carried out, and transitional meshing was adopted to balance the computational efficiency and simulation accuracy [22]. The mesh in the weld- and heat-affected zones, which have large temperature gradients, was finely divided, while the mesh size became progressively coarser away from the weld zone. The grid type used throughout was the eight-node hexahedral grid, with each grid node ensured to be connected. The results of the grid division are depicted in Figure 5. The model comprises a total of 149,800 elements and 161,118 nodes.

In the simulation process, the chewing gum method was employed to simulate the filling process of the weld material [23]. The material used in this study is Q345 alloy steel, which is chemically and mechanically similar to S355J2G3, as named by the European standard and available in the simulation software’s material library. S355J2G3 was selected as the base material for the simulation. Since the performance of the welding wire is similar to that of the base metal, the weld material was also assumed to be S355J2G3. The simulation took into account the variation in the material’s thermal physical and mechanical properties with temperature during the welding process.

Heat radiation and heat convection phenomena exist between the weldment and the outside world during the welding process. Two-dimensional elements on the surface of the finite element model were extracted and set as boundary conditions for heat exchange, following Newton’s law of cooling and the Stefan–Boltzmann law [24]. The temperature of the external environment was set to 20 °C, based on the actual indoor temperature during welding. Heat dissipation was considered throughout the entire welding process, with the process duration set from 0 to 3600 s.

During the welding test, no additional external constraints were imposed on the sample. Therefore, only the three nodes of the finite element model’s bottom plate were constrained during the welding simulation. During the subsequent cooling stage, these constraints were removed to allow free deformation. The heat dissipation and displacement boundary conditions applied are depicted in Figure 6.

According to the design of the typical T-joint welding test scheme, the welding mode was selected as MAG welding in the simulation software, and the corresponding welding parameters were set.

The heat source model, a mathematical function expression describing the heat input density distribution during welding, significantly influences the temperature and stress field calculations in welding simulations [25]. Based on the heat input characteristics of the welding method used in this paper, the double ellipsoid model was chosen for the simulation. The double ellipsoid heat source model is divided into front and back parts bounded by the center of the arc, which are characterized by two 1/4 ellipsoids, and its heat source density distribution is shown in Figure 7.

The front and back ellipsoids are characterized by the following mathematical formulas:

$${\mathrm{Q}}_f\left(x,y,z\right)=\frac{6\sqrt{3}Q{f}_f}{\pi a_{f}bc\sqrt{\pi }}\exp \left\{-3\left(\frac{x^2}{a_f^2}+\frac{y^2}{b^2}+\frac{z^2}{c^2}\right)\right\},x>0$$

(1)

$${\mathrm{Q}}_r\left(x,y,z\right)=\frac{6\sqrt{3}Q{f}_r}{\pi a_{r}bc\sqrt{\pi }}\exp \left\{-3\left(\frac{x^2}{a_r^2}+\frac{y^2}{b^2}+\frac{z^2}{c^2}\right)\right\},x\le 0$$

(2)

where Q is the power of the heat source, Q = ηUI, U is the arc voltage, I is the welding current, and η is the heat source efficiency, taken as 0.8; f_f and f_r are the heat distribution functions of two different half ellipsoids at the front and rear, and f_f + f_r = 2; a_f and a_r are the lengths of the front and rear half ellipsoids, respectively; b is half of the width of the ellipsoid; c is the depth of the ellipsoid.

After the heat source model was determined, its shape parameters were verified and adjusted to ensure that the simulated molten pool’s morphology aligned with the actual one. In this paper, the finalized shape parameters for the double ellipsoidal heat source model are as follows: 4.833 for parameter a_f, 9.667 for parameter a_r, 5.5 for parameter b, and 6 for parameter c. Figure 8 shows a comparison between the simulated and actual molten pool morphologies. The similarity in shape and size between the two molten pools demonstrates the model’s accuracy.

3.2. Comparison of Simulation Results

From the simulation results of the welding temperature field, the thermal cycle curves at the attachments of the thermocouple nodes during the welding test were extracted and compared with the actual measurement results, as shown in Figure 9.

It can be seen from the figure that the thermal cycle curves obtained by simulation agree well with the measured values both in terms of value and trend. The maximum measured temperature during the welding process of the first weld is 100.8 °C, while the simulated temperature is 102.6 °C. The position of the third weld that started welding around 200 s is closer to the measurement point, so the acquisition temperature is higher, the measured temperature is 296.4 °C, the simulated temperature is 306.3 °C, the maximum error is not more than 10 °C, and the coincidence is good. The simulated temperature during the cooling process is slightly higher than the measured temperature, and the reason for this gap may be that the heat dissipation conditions are complicated during the actual welding process, and there is a certain deviation in the calculation of heat loss in the simulation. Overall, it is basically considered that the results of the temperature field calculation coincide with the actual welding situation, which verifies the validity of the finite element model and the reliability of the calculation results.

In the calculation results of the finite element stress field, the distribution of longitudinal and transverse residual stress along the path of the stress detection points was extracted and compared with the test results, as shown in Figure 10. Comparing with the calculated results, it can be seen that although the values of the two are slightly different, the distribution pattern is similar, verifying the effectiveness of the finite element model and the accuracy of the calculated results. Subsequently, the welding process of the typical T-joint of the upper frame can be further analyzed and studied using this model. The numerical deviation may be caused by model simplification, drilling errors, and other factors.

3.3. Welding Process Impact Analysis and Optimization

The typical T-joint weldments obtained from welding experiments exhibit good surface quality. However, after inspection of the weld pool morphology, quality inspectors noted slight deficiencies in penetration depth for the first and second weld passes, which only meet the minimum quality requirements, and subsequent weld passes merge well with the preceding ones. During the formulation of the test scheme, welding current and voltage were in accordance with the welding process specifications set by the company. Additionally, frequent adjustments to welding current and voltage during the welding process, which change the welding heat input, will affect the welding efficiency. Therefore, only two welding processes, welding speed and interlayer cooling time, were studied in this paper to analyze their effects on welding residual stress and deformation.

3.3.1. Analysis of the Influence of Welding Speed

In order to solve the problem of insufficient penetration of the first and second welds, in this paper, the welding speed of the first and second welds was changed for simulation calculation while the heat input power was kept unchanged, and the subsequent welding speed was kept unchanged to analyze the impact on the overall welding results.

The welding speeds selected in the simulation analysis were 5 mm/s, 5.5 mm/s, 6.67 mm/s, and 8 mm/s, where 6.67 mm/s was the previous welding test parameter, and the other conditions were consistent with the previous finite element model. The calculation results of the steady-state temperature field of the first weld at different welding speeds were intercepted, as shown in Figure 11.

The size of the molten pool morphology obtained at different welding speeds is different, the smaller the welding speed, the larger the molten pool morphology and the wider the spread of isotherms. This is because the welding speed decreases, resulting in greater line energy. When the welding speed is 5 mm/s and 5.5 mm/s, the molten pool morphology can meet the engineering requirements; when the welding speed is 8 mm/s, there is a failure to melt through.

Figure 12 shows the equivalent residual stress clouds diagram of the specimen cooled to 3600 s. The maximum value of equivalent residual stress is 682.78 MPa, 681.89 MPa, 684.03 MPa, and 690.89 MPa, respectively. There is no significant fluctuation in equivalent residual stress following changes in welding speed for the first two welds, because the heat input for subsequent weld passes is higher, and thus has a more significant impact on equivalent residual stress.

Figure 13 shows the Z-displacement cloud diagram of the specimen cooled to 3600 s. Unlike changes in residual stress, variations in welding speed significantly affect the z-displacement of the specimen. This is because as the welding speed decreases, the heat input into the weldment increases, leading to more pronounced deformation in the Z-direction.

In order to further compare the influence of several welding speeds on deformation, the Z-direction deformation of the bottom of the flange perpendicular to the middle line of the welding direction was extracted, as shown in Figure 14. The maximum Z-displacement caused by four different welding speeds is 1.33 mm, 1.28 mm, 1.18 mm, and 1.10 mm, respectively. When the heat input power remains unchanged, the welding deformation in the Z direction increases by more than 5% when the welding speed of the first two welds is reduced by 0.1 mm/s.

In summary, the results show that satisfactory weld pool morphology can be obtained when the first two welds are welded at speeds of 5 mm/s and 5.5 mm/s. When welding is performed at a speed of 5.5 mm/s, post-welding deformation is minimal and production efficiency is high. Therefore, a welding speed of 5.5 mm/s is more appropriate for the first two welds.

3.3.2. Analysis of Influence of Interlayer Cooling Time

Based on the analysis that the optimal welding speed for the first two welds is 5.5 mm/s, the influence of interlayer cooling time on the overall welding result is analyzed. Simulation calculations were carried out for five cases of interlayer cooling time: 0 s, 30 s, 60 s, 90 s, and 120 s, respectively.

When the interlayer cooling time is determined, the temperature between the layers before the final weld reaches its maximum value, as shown in Figure 15. According to the calculation results, the maximum temperature before the last weld with five different cooling times is 1090.6 °C, 286.9 °C, 220.2 °C, 187.5 °C, and 167.8 °C, respectively. In the welding manufacturing standard for the upper frame of the hydropower unit, it is stipulated that the interlayer temperature of the weld seam cannot exceed 200 °C during welding. This requirement can only be met when the interlayer cooling time is greater than 90 s.

A longer interlayer cooling time is conducive to the uniform distribution of the weld temperature field after welding, and the final residual stress distribution cloud diagram calculated for different interlayer cooling times is shown in Figure 16.

Different interlayer cooling times did not change the distribution trend of residual stress. The maximum equivalent residual stress obtained by simulation was 736.19 MPa, 701.67 MPa, 687.78 MPa, 684.30 MPa, and 688.85 MPa, respectively. The final residual stress of the specimen was higher when the interlayer cooling time was short. This may be because with shorter cooling times, the interlayer temperature of the weld is higher, and the material remains in the high-temperature region for a longer period, which leads to a more thorough transformation process from austenite to bainite and martensite. When the interlayer cooling time is 90 s, the maximum residual stress is reduced by 51.89 MPa compared to 0 s.

Figure 17 shows the Z-direction deformation of the specimen’s flange bottom perpendicular to the welding direction centerline under different interlayer cooling times. With the increase in interlayer cooling time, the maximum Z-direction deformation slightly increases, but the variation is not significant.

The effects of different interlayer cooling times on welding temperature field, residual stress, and deformation are analyzed comprehensively. When the interlayer cooling time is 90 s, the welding process requirements can be met, and the residual stress and deformation after welding are small. Compared with the 120 s interlayer cooling time, the 90 s interlayer cooling time is more conducive to improving the manufacturing efficiency of welds in actual welding operations.

4. Simulation Analysis of Welding Deformation of Upper Frame Based on ISM

4.1. The Theory of Inherent Strain

In general, the total strain $\epsilon$ includes elastic strain ${\epsilon }^e$, plastic strain ${\epsilon }^p$, thermal strain ${\epsilon }^T$, and phase change strain ${\epsilon }^{tr}$, as follows:

$$\epsilon ={\epsilon }^e+{\epsilon }^p+{\epsilon }^T+{\epsilon }^{tr}$$

(3)

For the welding of low-carbon steel, the effect of phase transformation and thermal strain on the final welding residual stress and deformation is very small, which can often be ignored [4]. In this case, the inherent strain is equal to the residual plastic strain.

$${\epsilon }^{*}=\epsilon -{\epsilon }^{\mathrm{e}}={\epsilon }^p+{\epsilon }^T+{\epsilon }^{tr}={\epsilon }^p$$

(4)

Currently, the primary methods for obtaining inherent strain include the experimental method and TEP-FEM. However, due to the difficulty in accurately measuring welding shrinkage through experiments, this paper employed the TEPM to obtain inherent strain. The inherent strain value was extracted from the finite element model of the typical T-joint of the upper frame and then applied to the whole model of the upper frame model. The whole welding deformation can be predicted by a single elastic calculation.

4.2. Simulation of Welding Deformation for the Upper Frame of Hydropower Unit

4.2.1. Extraction and Verification of Inherent Strain

On the basis of verifying the validity of the finite element model and obtaining the welding process that meets the requirements, the inherent strain extracted from the TEP calculation results is used. However, in the simulation software, the inherent strain value cannot be directly applied as the initial load to the weld and its vicinity. Instead, it must be indirectly applied by modifying the thermal expansion coefficient in the material database. When the inherent strain value of the weld is known, the thermal expansion coefficient of the material can be calculated using Equation (5), which relies on the difference between the melting point of the material and the room temperature [20,26].

$${\epsilon }^{*}=\alpha \cdot \Delta T$$

(5)

where ${\epsilon }^{*}$ is the inherent strain value; α is the thermal expansion coefficient; ΔT is the difference between the melting temperature of the material and the environmental temperature, taken as 1280 °C.

The inherent strain value of all weld joints was extracted and averaged. Figure 18 shows the change in the average inherent strain of a typical T-joint over time. After the welding process was completed, the average inherent strain in the weld area eventually tended to a fixed value of 0.0386. According to the formula, the thermal expansion coefficient should be set to 0.000030.

In order to verify the accuracy of deformation calculation using the ISM, a shell element model with the same size as the TEP finite element model was established in the deformation prediction software based on inherent strain. The thickness of the flange plate and web was set at 20 mm, and the constraints remained unchanged. The shell element model and constraints are shown in Figure 19.

The thermal expansion coefficient of the material was modified to 0.000027 to apply the inherent strain effect, and then elastic calculations were conducted. The comparison of the overall deformation between the two methods is shown in Figure 20. The welding deformation obtained by the ISM is very similar to that obtained by the TEP-FEM. The maximum deformation calculated by the TEP-FEM is 1.438 mm, while the maximum deformation calculated by the ISM is 1.426 mm, resulting in an absolute error of 0.012 mm and a relative error of 0.83%.

The Z-direction deformation of the two methods and the Z-direction deformation of the bottom of the flange perpendicular to the center line in the welding direction are shown in Figure 21. The maximum deformation value calculated by both methods appears at the sides of the flange. The absolute value of the Z-directional displacement obtained by the TEP-FEM is 1.27 mm, while that obtained by the ISM is 1.20 mm, resulting in an absolute error of 0.07 mm and a relative error of 5.5%.

Comparative analysis shows that the ISM can obtain accurate post-welding deformation, and the calculation time is short, so it can be used to predict the overall welding deformation of the upper frame. The inherent strain is affected by groove form, material thickness, welding process, and other factors. The thickness of the oil tank bottom plate of the upper frame is 30 mm. Therefore, a finite element model with a flange thickness of 30 mm and a web thickness of 20 mm was established using the TEPM, and the inherent strain value is 0.0361. In the subsequent deformation prediction, the thermal expansion coefficient of the T-weld material at the bottom of the oil tank was modified to 0.000028.

4.2.2. Welding Sequence Planning for the Upper Frame of Hydropower Unit

Due to the large number of welds in the upper frame, the welds are described first in order to facilitate the description of the welding sequence. The upper frame of a certain model hydropower unit studied in this paper is mainly assembled and welded from components such as the upper ring, lower ring, brace ring, small rib plates, large rib plates, oil tank bottom plate, oil tank wall, upper wing plates, lower wing plates, and web plates. Except for the oil tank bottom plate with a thickness of 30 mm, the thickness of other components is 20 mm. The overall diameter is 3400 mm, and the height is 840 mm, as shown in Figure 22.

Before the overall welding of the upper frame, the upper rings were already integrated with the upper wing plates, and the lower rings were integrated with the lower wing plates to ensure a certain strength during frame positioning assembly. Therefore, in this study of deformation prediction, they were considered as wholes, with the main focus on investigating the influence of the welding sequence of T-shaped welds on the overall deformation.

The entire upper frame has a total of 136 T-shaped welds: the brace ring is located between the lower ring and the oil tank bottom plate, and due to the presence of small rib plates, it needs to be divided into 8 segments during welding, resulting in a total of 32 welds inside and outside; each of the 4 small rib plates has two T-shaped fillet welds and four T-shaped welds, totaling 24 welds; the large rib plates, along with the lower ring, brace ring, oil tank wall, upper and lower wing plates, and web plate, all have welds. Each large rib plate has six T-shaped fillet welds and ten T-shaped welds, totaling sixty-four welds; the oil tank wall is located between the upper ring and the oil tank bottom plate, and due to the presence of the large rib plate, it needs to be divided into four segments during welding, resulting in a total of sixteen T-shaped welds.

To reduce the number of workpiece flips during welding and improve efficiency, it is necessary to weld the bottom welds and fillet welds first, then flip the assembly after welding, and finally weld the upper welds. According to the welding process requirements for the upper frame, the fillet welds of the small and large rib plates need to be completed first, followed by the T-shaped welds. Based on this, the most common welding sequence currently used is as follows: complete the welding of the bottom large rib plates first, followed by the small rib plates; weld the inner T-shaped welds of the brace ring first, followed by the outer T-shaped welds; weld the outer T-shaped welds of the oil tank wall first, followed by the inner T-shaped welds.

Due to the large number of welds involved in the upper frame, the overall welding deformation simulation is complex, and it is not feasible to simulate all scenarios. Therefore, the most commonly used welding sequence is taken as scheme 1, and two additional welding schemes are designed for the inner and outer welds of the brace rings, the tank wall, and the T-shaped welds of the small and large rib plates. The criterion for evaluating the superiority and inferiority of the schemes is to minimize the welding deformation.

Scheme 2 is as follows: first complete the welding of the bottom small rib plates, followed by the large rib plates; weld the outer T-shaped welds of the brace rings first, followed by the inner T-shaped welds; and weld the inner T-shaped welds of the upper ring first, followed by the outer T-shaped welds.

Scheme 3 is as follows: alternate welding of small and large rib plates at the bottom; both the brace rings and upper ring are welded with outer T-shaped welds first, followed by the inner T-shaped welds.

4.2.3. Establishment of Finite Element Model of the Upper Frame

The overall size of the upper frame is large, and using hexahedral meshing will result in a huge number of elements, leading to low computational efficiency. Due to the relatively small thickness of the plates compared to the overall size, 2D shell elements were used for meshing. Tetrahedral shell elements were mainly used for meshing, with a few areas meshed with triangular elements. The mesh near the welds and their adjacent areas was dense. The finite element model of the upper frame shell is shown in Figure 23, which has a total of 61,607 nodes and 57,155 2D elements.

The upper frame mesh model was imported into the welding deformation prediction software, where the thermal expansion coefficients of the materials at the corresponding welds were modified, and boundary conditions were set. Different welding sequences were simulated by changing the application sequence of inherent strains and elastic calculations were conducted.

5. Results and Discussion

For the convenience of viewing the results, a local coordinate system was established, with the X-direction perpendicular to a certain large rib plate, the Y-direction parallel to the bottom weld of the large rib plate, and the Z-direction representing the thickness direction of the upper frame. The upper frame is a symmetrical structure, and the deformation results in the X and Y directions are similar, so only the welding deformation in the X-direction of the local coordinate system is shown. The overall welding deformation prediction results of the upper frame of the hydropower unit are shown in Figure 24.

Figure 24a shows the overall welding deformation of the upper frame in Scheme 1. As depicted in the figure, the deformation of the upper frame is relatively symmetrical, with the maximum deformation occurring at the middle of the outer edge of the upper ring, reaching a maximum value of 3.153 mm. This area is located between the two arms, where the constraint from the large rib plates is weakest, resulting in the greatest deformation. The deformation in the middle of the tank wall is relatively small, mainly due to its distance from the welds, resulting in minimal influence from welding.

Figure 24b shows the welding deformation in the X-direction of the upper frame in Scheme 1. The maximum deformation occurs at the middle edge between the two belly plates, with a maximum deformation value of 1.959 mm in the positive X direction and 2.028 mm in the negative X-direction. The deformation on the side welded later is smaller, mainly because it is constrained by the weld on the side welded first.

Figure 24c shows the deformation in the Z-direction of the upper frame. The maximum deformation in the Z-positive direction occurs at the bottom wing plate, measuring 1.779 mm, while the maximum deformation in the Z-negative direction occurs at the middle of the outer edge of the upper ring, measuring 3.149 mm. Significant deformation is also observed in the area between the two rib plates.

Comparing the overall deformation of the upper frame under three different welding sequences, it can be observed that the overall deformation trends of the three schemes are consistent. The areas with significant welding deformation are the outer edges between the two rib plates, the edges of the web plates, and the upper and lower wing plates.

The maximum deformations produced by the three schemes in each direction are shown in

Table 3. Maximum deformation value in each direction for different welding sequences (mm).

Scheme	Overall Deformation	X-Direction	Y-Direction	Z-Direction
1	3.153	2.028	1.990	−3.149~1.779
2	2.186	2.025	1.989	−2.181~1.777
3	3.162	2.026	1.988	−3.158~1.791

. From the table, it can be seen that there is almost no difference in the deformations in the X and Y directions among the three schemes, and the change in welding sequence in the central area has little effect on the two side arms. The maximum overall deformation for Scheme 2 is 2.188 mm, which is approximately 30.6% lower than the maximum deformation of 3.153 mm produced by the currently most commonly used welding sequence, Scheme 1.

According to Figure 25, the Z-directional deformations of the upper ring outer path 1, upper ring inner path 2, lower ring outer path 3, and lower ring inner path 4 were extracted to further analyze the influence of different welding sequences. The deformations of different path schemes are shown in Figure 26.

Figure 26a shows the Z-direction deformation on the outer side of the upper ring. From the graph, it can be observed that the post-welding deformation in Scheme 2 is the smallest, with a maximum value of 1.648 mm. This is a reduction of 1.501 mm compared to Schemes 1 and 3, which had a maximum deformation of 3.149 mm. This is because in Scheme 2, the inner T-shaped welds of the upper ring were welded first. During the welding of the outer T-shaped welds, the outer side of the upper ring was constrained by the inner T-shaped welds, resulting in less deformation. In Scheme 2, the constraint is more significant at the middle position between the two arms of the outer side of the upper ring due to the combined effect of the inner T-shaped welds and the arms, leading to a reduction in deformation four times. In Schemes 1 and 3, the outer side of the upper ring was welded first, and there is no constraint from the inner T-shaped welds. As a result, the constraint at the middle position between the two arms of the outer side is minimal, leading to larger deformation, and the deformation curves of both schemes almost overlap.

Figure 26b shows the Z-direction deformation on the inner side of the upper ring. Based on the previous analysis of deformation, it is observed that larger deformations occur on the side welded first, while smaller deformations occur on the side welded later. Therefore, in this case, the deformation in Scheme 2 on the inner side of the upper ring is larger compared to the deformations generated by welding the outer side first in the other two schemes, increasing by 0.832 mm. Although the deformation in Scheme 2 on the inner side of the upper ring is slightly larger than in Schemes 1 and 3, the distribution of deformation between the inner and outer sides of the upper ring is more uniform at this point. This is beneficial for the overall balance and stability of the structure, and the overall maximum deformation is smaller. Therefore, when welding the upper ring, it is more reasonable to weld the outer T-shaped welds first and then the inner T-shaped welds, indicating that the welding sequence of Scheme 2 is more reasonable.

Figure 26c shows the Z-direction deformation on the outer side of the lower ring. It can be observed that the deformation trends produced by the three welding sequences on the outer side of the lower ring are quite similar, with the lower edges between the two rib plates showing an upward curling trend. The Z-direction deformation of the lower ring in Scheme 2 is the smallest, decreasing by 4.2% compared to Scheme 1, and the difference in deformation compared to Scheme 3 is not significant. Therefore, when welding the rib plates to the lower ring, welding the T-shaped welds of the small rib plates first to form a certain rigidity, and then welding the large rib plates, can effectively reduce the degree of curling at the lower ring edges. Thus, the welding sequence of Scheme 2 is more reasonable.

Figure 26d shows the Z-direction deformation on the inner side of the lower ring. It can be seen from the figure that the deformation trends on the inner side of the lower ring caused by the three welding sequences are similar. Both Scheme 2 and Scheme 3 result in smaller maximum Z-direction deformation values than Scheme 1. Therefore, when welding the brace ring, it is more reasonable to weld the outer T-shaped welds first, followed by the inner T-shaped welds. Thus, the welding sequences of Scheme 2 and Scheme 3 are more reasonable.

Comparing the deformation caused by the three different welding sequences, Scheme 2’s welding sequence is more favorable. That is, during welding, the small rib plates should be welded first, followed by the large rib plates; the brace ring should be welded with the outer T-shaped welds first, followed by the inner T-shaped welds; and the upper ring should be welded with the inner T-shaped welds first, followed by the outer T-shaped welds.

6. Conclusions

This paper used the TEPM to simulate and analyze the typical T-joint welding process of the upper frame. It analyzed the influence of welding speed and interlayer cooling time on its welding results and obtained a welding process that met engineering requirements. Based on the TEP calculation results, ISM was used to perform elastic calculation of the overall welding deformation of the upper frame, predicting its deformation. The main research conclusions are as follows:

• The results obtained from the established thermoelastic–plastic finite element model are in good agreement with the experiments. Therefore, this model can be used to study the typical T-joint welding process.
• When welding the first two welds of the T-joint at a welding speed of 5.5 mm/s and an interlayer cooling time of 90 s, the welding results meet the engineering requirements.
• Extracting the inherent strain from the thermo-elastoplastic calculation results and using the ISM to calculate welding deformation have high accuracy, significantly reducing computational workload. This is of great significance for predicting welding deformation in large and complex welded structures.
• Using the ISM to predict the overall welding deformation of the upper frame, the results indicate that significant post-welding deformation occurs at the outer edge of the upper ring, the edge of the web plates, and the edges of the upper and lower wing plates. Adopting the welding sequence of first welding the small T-shaped rib plates, then welding the large T-shaped rib plates; welding the outer T-shaped welds of the brace ring first, then welding the inner T-shaped welds; and welding the inner T-shaped welds of the upper ring first, then welding the outer T-shaped welds, can result in smaller post-welding deformation. This provides a reference for the actual welding of the upper frame.