The scope of my research focuses on developing efficient surrogate models using machine learning, particularly artificial neural networks to predict welding-induced residual stress. Our key focus is on addressing how to automate data generation for welding simulation to enhance efficiency. We established that automating data generation with Python scripts and macro functions significantly reduces simulation setup time, enabling large dataset creation.
Additionally, our artificial neural network-based circuit model accurately predicts welding-induced residual stress, achieving a relative root mean square error of 0.0024. achieving a relative root mean square error of 0.0024. Our protocol offers advantages by automating data generation through Python scripts and macro functions, reducing the time and effort required for simulation setup and data extraction.
This ensures consistency and enables the creation of extensive dataset for training machine learning models. To begin, open Abaqus and click on file, followed by set work directory to set the working directory. Then sequentially click on file macromanager work and create a macro named thermal recording.
Create a model for welding specimens. Use a single weld bead on plate structure benchmark case as an example. Click on part followed by create part.
Create a 3D deformable half model of the specimen by extruding a square sketch on the XY plane. Now click on part, navigate to create datum plane, and select offset from principle plane. Define the start and end points of welding by specifying offsets from the YZ plane based on bead length.
Then create two additional datum planes for bead depth and width by specifying offsets from the XY plane and XZ plane respectively. Click on part and select the partition cell use datum plane option to create cell partitions of the specimen using the four datum planes. Then click on part and select create solid extrude.
Create a sketch on one of the datum planes to define the part of the weld bead underneath the top surface of the specimen. Use an arc and two lines following the bead dimensions. Extrude the sketch to the depth of the bead length to create the cut.
Next, extrude the sketch to the bead length while selecting keep internal boundaries. Click on part, then select create datum plane, and offset from principle plane. Sketch the weld bead using two arcs in one line on one of the datum planes.
Click on part, select partition cell, and use datum plane to create cell partitions of the specimen using the four datum planes to find. To define the material of stainless steel AISI 316 LN, click on property and create material, then define density in the general menu and conductivity and specific heat in the thermal menu using temperature dependent data. Next, assign material to the model.
Click on property, then create section to create a homogeneous solid section with the defined material. Click on property, assign section to assign the created section to the model. Now click on step, followed by create step to create a heat transfer step named welding with a time period of 26.43 and a fixed time increment of 0.1, ensuring no non-linearity of geometry.
Create another heat transfer step named cooling one with a time period of 70 using adaptive time increments with initial, minimum, and maximum increment sizes set to 0.1, 0.05, and 5 respectively. set to 0.1, 0.05, and 5 respectively. Lastly, create a heat transfer step named cooling two with a time period of 2, 000 using adaptive time increments with initial, minimum, and maximum increment sizes set to 5, 1, and 100 respectively.
To set the model attributes, click on model, edit attribute. to access the attribute settings. Set the absolute zero temperature to 273.15.
Set the absolute zero temperature to 273.15. Specify the Stefan-Boltzmann constant as 5.67 x 10 to the power of 11. Click on step and create field output to set a nodal temperature request for the entire model.
Then click on assembly and create instance to create a dependent instance. Next sequentially click on interaction, create interaction and surface film condition to create a surface film condition interaction with a film coefficient to 15 and a sink temperature of 20 on all surfaces of the model except the symmetric plane. Set the start step as welding.
Now sequentially click on interaction, create interaction, and surface radiation to create a surface radiation interaction with an emissivity of 0.7 and an ambient temperature of 20 on all surfaces of the model except the symmetric plane. Set the start step as welding, define loads in the load module. Click on load, create load thermal and body heat flux to create a user-defined body heat flux load that starts in the welding step and is inactive during the two cooling steps.
Then click on load, create predefined field, other, and field to create a predefined temperature field starting from the initial step to represent a room temperature of 20. To create a mesh in the mesh module, click on mesh, select the object to be part and seed part to seed the part by a global size of 0.0024. Click on mesh, then seed edges to seed the edges of bead depth and bead width by a number of 3.
Seed the edge of the arc by a number of 3 and the edge of bead length by a size of 0.0015. Next, click on mesh, assign mesh controls, and use the TET shape element with the free technique for the bead region. Click on mesh, assign element type, and set the element type to DC 3D 10, then mesh the part.
Use mesh, then seed edges to seed edges collinear to the X-axis within the fine mesh region with a size of 0.0015, the Y-axis edges with a size of 0.0011, and the Z-axis edges with a size of 0.00075. and the Z-axis edges with a size of 0.00075. Now click on mesh, followed by assigned mesh controls to assign mesh control for the remaining region, using the hex shape element with the sweep technique.
Then click on mesh, assign element type, and set the element type to DC 3D 20, followed by meshing the part. Click on job, create job to create a job named thermal analysis and attach the D flux user subroutine. Stop the macro recording.
Confirm that a Python file named abaqusMacros. py is generated in the working directory. Finally, click on job, job manager, and submit.
A result file named ThermalAnalysis. odb will be generated. Longitudinal stresses along the BD line showed consistent variation across different combinations of arc travel length, arc advanced speed, and net energy input rate with stress peaking closer to the surface and decreasing at deeper depths.
The majority of discrepancies between finite element simulation and artificial neural network predictions fell within the range of 0 to 2 Megapascals, accounting for 45.2%of test data. Stress level bins with fewer training data points exhibited higher maximum discrepancies in the test dataset as seen in absolute residuals of specific bins. Artificial neural network predictions matched finite element simulation results closely with a mean square error of 0.0024.
