Finite element simulation method for laser shock forming ribbed wall plate

Abstract

This invention provides a finite element simulation method for laser-shock-formed stiffened panels, comprising: determining the initial temporal and spatial distribution of laser shock pressure corresponding to laser process parameters; applying it as a load to a finite element model of laser multi-point continuous dynamic impact to obtain the simulated impact crater size; determining whether the simulated and experimental impact crater sizes are within the allowable error range; acquiring the strain field and residual stress field after laser impact, and outputting the average inherent strain distribution along the depth direction; introducing the average inherent strain distribution into the layered shell element model of the stiffened panel and solving it to obtain the deformation results of the stiffened panel impacted by laser process parameters. This invention achieves dynamic simulation of laser multi-point continuous impact through explicit analysis and deformation simulation of laser-shock-formed stiffened panels through thermoelastic analysis, thereby enabling effective forming simulation of complex stiffened panels, achieving the effects of low cost, high efficiency, and accurate prediction results.

Description

Technical Field

[0001] This invention relates to the field of laser shock forming technology, and more specifically to a finite element simulation method for laser shock forming of ribbed panels. Background Technology

[0002] Laser shock forming is a novel surface strengthening and forming technology that, while shaping a part to its target shape, introduces residual compressive stress and microstructural changes to the part's surface, thereby improving the mechanical properties of the formed part. Since current laser shock forming technology is moldless, optimizing the laser shock process parameters is necessary to obtain the desired part shape. However, due to the complexity of the laser shock forming mechanism and the influence of numerous variable factors during the forming process, optimizing process parameters solely through experiments and operational experience is extremely difficult. Therefore, combining finite element simulation with laser shock forming process parameter optimization is a simpler, more effective, and lower-cost method.

[0003] Chinese patent CN107633115 discloses a "finite element simulation method for multi-point laser shock forming," which uses characteristic elements to perform multi-point laser shock simulation, obtains the residual stress distribution, and uses it as the initial stress field to simulate the forming result. This patent uses the direct stress method to simulate the laser shock forming of flat plates, but it does not consider the error between simulation and experimental results. Furthermore, this patent is only applicable to flat plates and does not cover the forming simulation of ribbed panels. In addition, existing technologies mainly focus on forming simulations of simple structures without ribbed panels, and existing forming simulation methods all start from known stress distributions or inherent strains, failing to correlate laser process parameters with deformation simulation.

[0004] Therefore, there is an urgent need for a complete method that can simulate laser shock forming of stiffened panels based on laser process parameters, so that the inherent strain method can be applied to the simulation of laser shock forming of stiffened panels. Summary of the Invention

[0005] The present invention provides a finite element simulation method for laser shock forming of stiffened panels, which is mainly used to solve the problem that existing laser shock forming technology combined with finite element simulation cannot effectively simulate the forming of stiffened panels. Thus, it can effectively simulate the forming of complex stiffened panels, with low cost, high efficiency and accurate prediction results.

[0006] The present invention achieves the above objectives through the following technical solutions:

[0007] A finite element simulation method for laser-shock-formed ribbed panels includes:

[0008] Step 1: Determine the initial temporal and spatial distribution of laser shock pressure corresponding to the laser process parameters.

[0009] Step 2: Establish a finite element model of laser multi-point continuous dynamic impact, and apply the preliminary laser impact pressure time-space distribution as a load to the finite element model of laser multi-point continuous dynamic impact to obtain the simulated impact crater size of the laser process parameters.

[0010] Step 3: Correct the temporal and spatial distribution of laser shock pressure, and determine whether the error between the simulated impact crater size and the experimental impact crater size under the same laser process parameters is within the allowable error range. If yes, output the temporal and spatial distribution of laser shock pressure corresponding to the laser process parameters and proceed to the next step. If no, adjust the laser absorption coefficient and return to step 1.

[0011] Step 4: Apply the time-space distribution of the laser shock pressure to the finite element model of the laser multi-point continuous dynamic shock and solve it to obtain the strain field and residual stress field after the laser process parameters are impacted, and extract the inherent strain distribution along the depth direction, thereby outputting the average inherent strain distribution along the depth direction corresponding to the laser process parameters.

[0012] Step 5: Introduce the average inherent strain distribution along the depth direction into the layered shell element model of the stiffened wall panel and solve it to obtain the deformation results of the stiffened wall panel impacted by the laser process parameters.

[0013] A further approach is to have the initial laser shock pressure temporal and spatial distribution in step 1 as follows:

[0014]

[0015] Where τ is the laser pulse width; α p α is the laser absorption coefficient; γ is the coefficient of internal energy to heat conversion; R is the specific heat capacity of air; I is the laser spot radius; Z is the laser power density; and Z is the total impact impedance.

[0016] A further approach is to use a three-dimensional deformable solid type for the laser multi-point continuous dynamic impact finite element model, with its finite element region located in the middle of the three-dimensional model and containing 4×4 arranged laser spot impacts.

[0017] The boundary of the finite element region is 1 mm larger than the boundary of the light spot impact region.

[0018] The edges of the three-dimensional model are infinite element regions, and the width of the infinite element regions is greater than 2mm.

[0019] A further approach is to set the material of the laser multi-point continuous dynamic impact finite element model as an isotropic Johnson-Cook material constitutive model.

[0020] A further proposed solution is that step 2 also includes:

[0021] Step 21: Load application settings: The Vdload subroutine is used to apply the laser shock multi-spot position and the temporal and spatial distribution of the shock pressure, and the application position is the top surface of the finite element region.

[0022] Step 22: Analysis step time setting: Three analysis steps need to be set for each single spot application. The analysis step time is divided into the analysis step time for the pressure rise stage, the analysis step time for the pressure fall stage, and the analysis step time for the stabilization stage.

[0023] Step 23: Boundary condition setting: Set the bottom surface of the finite element region of the three-dimensional model to a completely fixed constraint.

[0024] Step 24: The preliminary laser shock pressure temporal and spatial distribution is written into the Vdload subroutine using Fortran language.

[0025] A further proposed solution is that step 3 also includes:

[0026] Step 31: Extract the deformation profile of the impact crater from the simulation results of the finite element method for multi-point continuous dynamic impact of laser.

[0027] Step 32: Calculate the depth and width errors between the simulated impact crater and the experimental impact crater, and determine whether they are within the allowable error range.

[0028] The allowable error range is less than 5%.

[0029] A further proposed solution is that step 4 also includes:

[0030] Step 41: Divide the average inherent strain into several layers along the depth direction, and perform linear interpolation processing with each layer having a thickness of 0.1 to 0.3 mm.

[0031] A further proposed solution is that step 5 also includes:

[0032] Step 51: Establish the layered shell element model of the ribbed wall panel using three-dimensional shell elements, and divide the wall panel into strips.

[0033] The material of the layered shell unit model with stiffened wall panels is set as a composite material shell unit.

[0034] A further proposed solution is that step 5 also includes:

[0035] Step 52: Divide the shell unit in the layered shell unit model of the stiffened shell panel into several layers in the thickness direction, and set the average inherent strain distribution along the depth direction as the coefficient of thermal expansion in the shell panel material properties.

[0036] Step 53: Obtain the inherent strain using the coefficient of thermal expansion and temperature rise, and apply the inherent strain to the laser shock region.

[0037] A further proposed solution is that step 5 also includes:

[0038] Step 54: Analysis Step Setup: Set strips on the wall panel of the layered shell unit model with ribbed wall panel, and calculate the width and number of the strips. The number of analysis steps is consistent with the number of strips.

[0039] Step 55: Boundary condition setting: Apply a fully fixed constraint to the center point of the bottom surface of the ribbed layered shell unit model.

[0040] Therefore, the present invention has the following beneficial effects:

[0041] 1. This invention achieves dynamic simulation of continuous multi-point laser impact through display analysis and deformation simulation of laser-impact formed stiffened panels through thermoelastic analysis. This enables effective forming simulation of complex stiffened panels, providing a basis for parameter control of deformation. It also has the advantages of low cost, high efficiency, and accurate prediction results, and has good prospects for engineering applications.

[0042] 2. The laser shock pressure temporal and spatial distribution proposed in this invention has only a single unknown parameter. Through single-spot shock experiments, a database with a one-to-one correspondence between laser process parameters and laser shock pressure temporal and spatial distribution was established, and an inherent strain database corresponding to the process parameters was also established. Furthermore, the laser shock pressure distribution correction is simple and can effectively control the error between simulation results and experimental results.

[0043] 3. This invention proposes a simulation method for the dynamic response process of laser multi-point continuous impact. This method differs from the explicit-implicit alternating analysis simulation method. Its steps are simpler, and it can calculate the continuous dynamic process of multi-point laser impact in one go, thereby obtaining the complete strain distribution, residual stress distribution and deformation distribution of the laser impact process. The method is simpler and more effective.

[0044] 4. The layered shell element model of the stiffened wall panel proposed in this invention transforms the complex dynamic process of laser shock forming stiffened wall panels into a thermoelastic deformation process, and improves the prediction accuracy and computational efficiency of laser shock forming stiffened wall panels by optimizing the number of analysis steps.

[0045] The present invention will now be described in further detail with reference to the accompanying drawings and specific embodiments. Attached Figure Description

[0046] Figure 1 This is a flowchart of the finite element simulation method for laser-shock-formed stiffened wall panels in an embodiment of the present invention.

[0047] Figure 2 This is a schematic diagram of the dimensions of the stiffened wall panel structure in an embodiment of the present invention.

[0048] Figure 3 This is a laser shock time distribution diagram in an embodiment of the present invention.

[0049] Figure 4 This is a spatial distribution diagram of laser shock in an embodiment of the present invention.

[0050] Figure 5 This is a schematic diagram of the establishment and mesh generation of the finite element model of laser multi-point continuous dynamic impact in an embodiment of the present invention.

[0051] Figure 6 This is a deformation result diagram of the laser multi-point continuous dynamic impact model in an embodiment of the present invention.

[0052] Figure 7 This is a schematic diagram of the deformation dimensions of the impact crater in an embodiment of the present invention.

[0053] Figure 8 This is an average intrinsic strain depth distribution diagram in an embodiment of the present invention.

[0054] Figure 9 This is a simulated deformation result diagram of a laser-shock-formed ribbed wall panel in an embodiment of the present invention.

[0055] Figure 10 This is a comparison diagram of simulated and experimental deformation of a laser-shock-formed ribbed wall panel in an embodiment of the present invention. Detailed Implementation

[0056] To make the objectives, technical solutions, and advantages of the embodiments of the present invention clearer, the technical solutions of the embodiments of the present invention will be clearly and completely described below with reference to the accompanying drawings. Obviously, the described embodiments are only some, not all, of the embodiments of the present invention. All other embodiments obtained by those skilled in the art based on the described embodiments of the present invention without creative effort are within the scope of protection of the present invention.

[0057] An Example of a Finite Element Simulation Method for Laser Shock Forming Ribbed Panels

[0058] See Figure 1 The present invention relates to a finite element simulation method for laser-shock-formed ribbed panels, comprising:

[0059] Step 1: Determine the initial temporal and spatial distribution of laser shock pressure corresponding to the laser process parameters.

[0060] Step 2: Establish a finite element model of laser multi-point continuous dynamic impact, and apply the preliminary laser impact pressure time-space distribution as a load to the finite element model of laser multi-point continuous dynamic impact to obtain the simulated impact crater size of the laser process parameters.

[0061] Step 3: Correct the temporal and spatial distribution of laser shock pressure, and determine whether the error between the simulated impact crater size and the experimental impact crater size under the same laser process parameters is within the allowable error range. If yes, output the temporal and spatial distribution of laser shock pressure corresponding to the laser process parameters and proceed to the next step. If no, adjust the laser absorption coefficient and return to step 1.

[0062] Step 4: Apply the time-space distribution of the laser shock pressure to the finite element model of the laser multi-point continuous dynamic shock and solve it to obtain the strain field and residual stress field after the laser process parameters are impacted, and extract the inherent strain distribution along the depth direction, thereby outputting the average inherent strain distribution along the depth direction corresponding to the laser process parameters.

[0063] Step 5: Introduce the average inherent strain distribution along the depth direction into the layered shell element model of the stiffened wall panel and solve it to obtain the deformation results of the stiffened wall panel impacted by the laser process parameters.

[0064] Specifically, in step 1 of this embodiment, the corresponding temporal and spatial distribution of laser shock pressure P(t,x,y) is calculated using formula (1) based on the laser process parameters:

[0065]

[0066] Where τ is the laser pulse width, in nanoseconds (ns); α p α is the laser absorption coefficient; γ is the coefficient of internal energy to heat energy conversion; R is the laser spot radius (mm); I is the laser power density (GW / cm²); Z is the total impact impedance (g / cm²s).

[0067] Specifically, in this embodiment, the laser power density I is calculated using formula (2):

[0068]

[0069] Where E is the laser energy, in J.

[0070] Specifically, in this embodiment, the total impact impedance Z is obtained through formula (3):

[0071]

[0072] Z1 and Z2 represent the impact impedances of the target material and the confinement layer material, respectively.

[0073] Specifically, in this embodiment, a laser is used to perform full-area laser shock blasting on the upper surface of the ribbed wall panel. The laser shock blasting process parameters are as follows:

[0074] The laser energy is E = 9J; the laser pulse width is τ = 20ns; the laser spot radius is a circular spot with a value of R = 1mm; the overlap rate of the spots in the X and Y directions is 0%. Substituting these values ​​into formula (2) yields:

[0075]

[0076] In this embodiment, the target is made of aluminum alloy 7075-T651, and the constraint layer is water flow. Therefore, Z1 = 0.165 × 10⁻⁶. 6 g / cm 2 s; Z2 = 1.71 × 10 6 g / cm 2 Substituting s into formula (3) yields the total impact impedance Z.

[0077] In this embodiment, α is the coefficient for converting internal energy into heat energy, α = 0.2; γ is the specific heat capacity of air, γ = 1.4. Substituting the above parameter values ​​into formula (1) yields:

[0078]

[0079] Where, α p Let α be the laser absorption coefficient, ranging from 0.8 to 1. First, let's take α... p =0.9, with the laser shock temporal and spatial distribution as the applied load of a single spot in the laser multi-point continuous dynamic shock model.

[0080] See Figure 3 and Figure 4 From the above equation P(t,x,y), we can obtain the time distribution and spatial distribution of laser shock pressure.

[0081] Specifically, in step 2 of this embodiment, the finite element simulation of continuous dynamic laser impact at multiple points includes:

[0082] See Figure 5 Model establishment and mesh generation: The laser multi-point continuous dynamic impact finite element model adopts a three-dimensional deformable solid type. Its finite element region is located in the middle of the three-dimensional model and contains 4×4 arranged laser spot impacts. The boundary of the finite element region is 1mm larger than the boundary of the laser spot impact region. The edge of the three-dimensional model is an infinite element region, and the width of the infinite element region is greater than 2mm.

[0083] See Figure 2Specifically, the ribbed wall panel described in this embodiment is a ribbed wall panel with a cross-shaped grid distribution of ribs, its upper surface is flat and its lower surface is ribbed. The material of this ribbed wall panel is 7075-T651 aluminum alloy, its external dimensions are 100mm×100mm×6mm, the thickness of the sheet is 3mm, and the height and width of the ribs are both 3mm.

[0084] Specifically, in this embodiment, based on the aforementioned ribbed wall panel structure, the dimensions of the three-dimensional model are 12mm × 12mm × 4mm; the finite element region is 10mm × 10mm × 4mm in size and is located in the middle of the three-dimensional model, containing 4×4 arranged light spot impacts; the element type in the finite element region is C3D8R, and the infinite element type in the infinite element region is CIN3D8; the mesh size in the X and Y directions is 0.05mm, and the mesh size in the Z direction is 0.025mm.

[0085] In this embodiment, the material of the laser multi-point continuous dynamic impact finite element model is set as a Johnson-Cook material constitutive model of the Homogeneous type.

[0086] In this embodiment, step 2 further includes:

[0087] Step 21: Load application settings: The Vdload subroutine is used to apply the laser shock multi-spot position and the temporal and spatial distribution of the shock pressure, and the application position is the top surface of the finite element region.

[0088] Specifically, in this embodiment, a user-defined load distribution type is selected, and the amplitude value is set to 1.

[0089] Step 22: Analysis step time setting: Three analysis steps need to be set for each single spot application. The analysis step time is divided into the analysis step time for the pressure rise stage, the analysis step time for the pressure fall stage, and the analysis step time for the stabilization stage.

[0090] Specifically, in this embodiment, the total analysis step time for a single light spot is 1.02 × 10⁻⁵ s, and the analysis step times for the pressure rise phase, pressure fall phase, and stabilization phase are 2.6 × 10⁻⁸ s, 1.74 × 10⁻⁷ s, and 1 × 10⁻⁵ s, respectively.

[0091] Step 23: Boundary condition setting: Set the bottom surface of the finite element region of the three-dimensional model to a completely fixed constraint.

[0092] Step 24: The preliminary laser shock pressure temporal and spatial distribution is written into the Vdload subroutine using Fortran language.

[0093] Specifically, in this embodiment, an Abaqus job is created, the path of the Vdload subroutine is added in the job creation window, the load is applied, and then the job is submitted for calculation to obtain the deformation results and residual stress field of the laser process parameter impact, thereby completing the finite element simulation of laser multi-point continuous dynamic impact.

[0094] When submitting a job, add the path to the Vdload subroutine in the User subroutine file field under the General options, and then submit the Abaqus job for computation.

[0095] See Figure 6 As can be seen, this embodiment obtained the 4×4 spot continuous laser shock plastic deformation result of the Z-shaped scanning path.

[0096] In this embodiment, step 3 further includes:

[0097] Step 31: Extract the deformation profile of the impact crater from the simulation results of the finite element method for multi-point continuous dynamic impact of laser.

[0098] Specifically, the method for extracting the deformation contour of the impact crater in this embodiment is as follows: using a Python script to extract the deformation of the impact crater along the Z direction at the last moment, along the X and Y directions of the light spot center respectively.

[0099] Step 32: Calculate the depth and width errors between the simulated impact crater and the experimental impact crater, and determine whether they are within the allowable error range.

[0100] The allowable error range is less than 5%.

[0101] See Figure 7 Specifically, in this embodiment, the depth of the impact crater is the difference between the Y values ​​of the highest and lowest points, and its width is the difference between the X values ​​of the two highest points.

[0102] Specifically, this embodiment compares the impact crater deformation dimensions measured with those of an experimental plate under the same parameters. The method involves calculating the impact crater depth and width separately until the error between the simulated and experimental impact crater dimensions is less than 5%. Otherwise, the laser absorption coefficient α is adjusted. p The value of α is returned, and steps 1 and 2 are executed; when α p When the value is 0.93, the difference in depth and width of the impact crater between the simulation and the experiment is both <5%, then proceed to the next step 4.

[0103] In this embodiment, step 4 further includes:

[0104] See Figure 8Step 41: Divide the average inherent strain into several layers along the depth direction, and perform linear interpolation processing with each layer having a thickness of 0.1 to 0.3 mm.

[0105] Specifically, the method for extracting the average natural strain described in this embodiment is as follows: the average natural strain along the depth direction of the finite element region at the last moment is extracted using a Python script.

[0106] Specifically, in step 5 of this embodiment, the following steps are included:

[0107] Step 51: Model building and mesh generation: A three-dimensional shell element model of the stiffened wall panel is built, and the wall panel strips are divided into layers.

[0108] Specifically, in this embodiment, the S4R four-node reduced integral shell element is selected, and the global element size is 500um.

[0109] The material of the layered shell unit model with stiffened wall panels is set to composite shell unit, which is of type Composite of Shell category.

[0110] In this embodiment, step 5 further includes:

[0111] Step 52: Divide the shell unit in the layered shell unit model of the stiffened wall panel into several layers in the thickness direction, and set the average inherent strain distribution along the depth direction as the coefficient of thermal expansion in the wall panel material properties.

[0112] Specifically, the material properties of the ribbed structure in the layered shell unit model with ribbed wall panel described in this embodiment do not include the coefficient of thermal expansion.

[0113] Step 53: Obtain the inherent strain by using the thermal expansion coefficient and the value of the inherent strain, and apply the inherent strain to the laser shock region.

[0114] The inherent strain is obtained by formula (4):

[0115] ε e =A*ΔT, ΔT=1 (4)

[0116] Where A is the coefficient of thermal expansion and ΔT is the temperature rise.

[0117] In this embodiment, step 5 further includes:

[0118] Step 54: Analysis Step Setup: Set strips on the wall panel of the layered shell unit model with ribbed wall panel, and calculate the width and number of the strips. The number of analysis steps is consistent with the number of strips.

[0119] Specifically, in this embodiment, the number of stripes corresponds to the number of laser shock paths in the Y direction.

[0120] Specifically, the strip width described in this embodiment is obtained using formula (5):

[0121] Δd=2R(1-η y )=2×1×(1-0)=2mm (5)

[0122] The number of stripes is obtained by formula (5):

[0123]

[0124] Where, η y L represents the overlap rate of the light spot in the Y direction. y Let Y be the length of the impact region in the Y direction.

[0125] Step 55: Boundary condition setting: Apply a fully fixed constraint to the center point of the bottom surface of the ribbed layered shell unit model.

[0126] Specifically, in this embodiment, Abaqus / Standard is used to solve the problem and obtain the deformation results of the laser-impact formed stiffened panel, thus completing the finite element simulation of the laser-impact forming of the stiffened panel.

[0127] See Figure 9 This embodiment obtains the complete deformation process and final deformation result of the ribbed wall panel under the laser process parameters. Since the laser shock processing process is difficult to observe, this simulation is beneficial to the study of laser shock forming process.

[0128] See Figure 10 In this embodiment, the simulated deformation results were compared with the experimental forming results. The error values ​​between the simulated deformation profile results in the X and Y directions and the experimental results were less than 3%, which showed that the forming prediction of this example was relatively good.

[0129] The above embodiments are merely preferred embodiments of the present invention and should not be construed as limiting the scope of protection of the present invention. Any non-substantial changes and substitutions made by those skilled in the art based on the present invention shall fall within the scope of protection claimed by the present invention.

Claims

1. A finite element simulation method for laser-shock-formed ribbed panel, characterized in that, include: Step 1: Determine the initial temporal and spatial distribution of laser shock pressure corresponding to the laser process parameters; Step 2: Establish a finite element model of laser multi-point continuous dynamic impact, and apply the preliminary laser impact pressure time-space distribution as a load to the finite element model of laser multi-point continuous dynamic impact to obtain the simulated impact crater size of the laser process parameters; Step 3: Correct the temporal and spatial distribution of laser shock pressure, and determine whether the error between the simulated impact crater size and the experimental impact crater size under the same laser process parameters is within the allowable error range. If yes, output the temporal and spatial distribution of laser shock pressure corresponding to the laser process parameters and proceed to the next step; if no, adjust the laser absorption coefficient and return to step 1. Step 4: Apply the time-space distribution of the laser shock pressure to the finite element model of the laser multi-point continuous dynamic shock and solve it to obtain the strain field and residual stress field after the laser process parameters are impacted, and extract the inherent strain distribution along the depth direction, thereby outputting the average inherent strain distribution along the depth direction corresponding to the laser process parameters. Step 5: Introduce the average inherent strain distribution along the depth direction into the layered shell element model of the stiffened wall panel and solve it to obtain the deformation results of the stiffened wall panel impacted by the laser process parameters; The temporal and spatial distribution of the initial laser shock pressure in step 1 is as follows: Where t is time; x and y are spatial coordinate variables; The laser pulse width; The laser absorption coefficient; γ is the coefficient for converting internal energy into heat energy; γ is the specific heat capacity of air; R is the laser spot radius; I is the laser power density; Z is the total impact impedance.

2. The finite element simulation method for laser-shock-formed ribbed panels according to claim 1, characterized in that: The laser multi-point continuous dynamic impact finite element model is a three-dimensional deformable solid type, and its finite element region is located in the middle of the three-dimensional model and contains at least 4×4 arranged laser spot impacts. Wherein, the boundary of the finite element region is at least 1 mm larger than the boundary of the light spot impact region; The edges of the three-dimensional model are infinite element regions, and the width of the infinite element regions is greater than 2mm.

3. The finite element simulation method for laser-shock-formed ribbed wall panels according to claim 2, characterized in that: The material of the laser multi-point continuous dynamic impact finite element model is set as an isotropic Johnson-Cook material constitutive model.

4. The finite element simulation method for laser-shock-formed ribbed panels according to claim 2, characterized in that, Step 2 also includes: Step 21: Load application settings: The Vdload subroutine is used to apply the laser shock multi-spot position and the temporal and spatial distribution of the shock pressure, and the application position is the top surface of the finite element region; Step 22: Analysis step time setting: Three analysis steps need to be set for each single spot application. The analysis step time is divided into the analysis step time for the pressure rise stage, the analysis step time for the pressure fall stage, and the analysis step time for the stabilization stage. Step 23: Boundary condition setting: Set the bottom surface of the finite element region of the three-dimensional model as a completely fixed constraint; Step 24: The preliminary laser shock pressure temporal and spatial distribution is written into the Vdload subroutine using Fortran language.

5. The finite element simulation method for laser-shock-formed ribbed panels according to claim 1, characterized in that, Step 3 also includes: Step 31: Extract the deformation profile of the impact crater from the simulation results of the finite element method of laser multi-point continuous dynamic impact. Step 32: Calculate the depth and width errors between the simulated impact crater and the experimental impact crater, and determine whether they are within the allowable error range. The allowable error range is less than 5%.

6. The finite element simulation method for laser-shock-formed ribbed panels according to claim 1, characterized in that, Step 4 also includes: Step 41: Divide the average inherent strain into several layers along the depth direction, and perform linear interpolation processing with each layer having a thickness of 0.1~0.3mm.

7. The finite element simulation method for laser-shock-formed ribbed panels according to claim 1, characterized in that, Step 5 also includes: Step 51: Establish the layered shell element model of the ribbed wall panel using three-dimensional shell elements, and divide the wall panel into strips; The material of the layered shell unit model with stiffened wall panels is set as a composite material shell unit.

8. The finite element simulation method for laser-shock-formed ribbed panels according to claim 7, characterized in that, Step 5 also includes: Step 52: Divide the shell unit in the layered shell unit model of the stiffened shell panel into several layers in the thickness direction, and set the average inherent strain distribution along the depth direction as the coefficient of thermal expansion in the shell panel material properties; Step 53: Obtain the inherent strain using the coefficient of thermal expansion and temperature rise, and apply the inherent strain to the laser shock region.

9. The finite element simulation method for laser-shock-formed ribbed panels according to claim 8, characterized in that, Step 5 also includes: Step 54: Analysis Step Settings: Set strips on the wall panels of the layered shell unit model with ribbed wall panels, and calculate the width and number of the strips. The number of analysis steps is consistent with the number of strips. Step 55: Boundary condition setting: Apply a fully fixed constraint to the center point of the bottom surface of the ribbed layered shell unit model.

Images