1. Introduction
Cold-formed steel (CFS) members are manufactured at room temperature, offering benefits such as high strength, ease of transportation, and rapid erection and construction. However, the thin-walled characteristic of CFS members makes them sensitive to strength variations based on their geometries [
1]. Although manufacturing tolerances are well controlled, transportation and storage can introduce additional geometric imperfections to the CFS members [
2,
3]. Consequently, predicting structural performance becomes more challenging due to random geometry deviations during numerical simulations. Traditional numerical simulations typically introduce an initial imperfection to the CFS models, with shapes based on the first buckling modes [
4]. The magnitude of the imperfection is determined as L/960 by both Chinese [
5] and North American standards [
4]. However, modern structural design trends lean towards analysis-based or simulation-based approaches, wherein nonlinear structural performance is a crucial consideration [
6,
7]. Traditional numerical simulations fall short of meeting the demands of structural analysis, particularly for CFS members [
8]. Accurate simulations for strength predictions must consider the real-world conditions of CFS members, such as their true geometry.
Measurement techniques are crucial for obtaining geometric information about CFS members. Over the past decades, measurements have evolved from contact-based to non-contact approaches [
9,
10]. Traditional contact measurements employ displacement sensors, calipers, and rulers to gauge geometric surface textures, cross-section dimensions, and specimen length. Consequently, the geometric imperfections incorporated into numerical simulations might not adequately represent the actual impacts of geometry on the strength of CFS members. On the other hand, non-contact measurements of CFS members predominantly utilize optical measurement techniques, such as laser-scanning triangulation (
Figure 1) [
10,
11] and photography DIC techniques [
12]. Such member-level measurements are more common in laboratories than in the industry. Limitations of these techniques include cost and efficiency. DIC techniques necessitate multiple high-resolution cameras and specialized software for measurements. Both research costs and device expenses can be prohibitive. Furthermore, the precision of these measurements might exceed the necessary qualifications [
13]. Laser-based measurement seems more pragmatic, but challenges arise in reconstructing measurements and their application in structural analysis.
Reconstruction of laser measurements has advanced in recent years. While commercial software is not yet tailored for structural member applications, fundamental surface registration from scanned segments is achievable. Users can register scanned segments of items from various angles using geometric features or calibration markers [
14,
15]. Additionally, such software can only compute the area and dimensions of regions specified by users. The level of automation in image processing for measurements is not satisfactory, especially considering the unstructured data in structural applications. As a solution, Zhao et al. [
11] proposed a post-processing algorithm that can automatically filter measurement noises and reorganize data for Zee-shaped section members. The post-processing algorithm processes data section by section. Section positions were determined through hardware records. A maximal curvature test was conducted on segments sequentially within a cross-section, identifying four maximum curvatures. These maximal curvatures were deemed the corners of the cross-section, while other segments represented flat regions such as webs, flanges, and lips. This method organized the data structure of the Zee-shaped sections for simpler structural and dimensional analysis. However, this approach was solely applied to Zee-shaped sections measured on a laboratory laser platform.
Feng et al. [
10] and Xu [
16] also introduced a post-processing method for measurements from a hand-held laser scanner, specifically RASNAC and geometric model reconstruction. Given that the targets are thick, hot-rolled steel sections, the resolution requirements for measurements are not as stringent as those for CFS members. Cross-sectional features are defined using several straight lines, enabling the intelligent identification of flanges and webs. Zhao [
8] later proposed a new robust feature recognition method that fits other shapes of CFS members. The new robust feature recognition method is suitable for various shapes of CFS members. This method is globally optimized, ensuring more accurate feature recognition. The data structure is organized based on the geometric features of structural members, such as webs, flanges, lips, and corners. This geometric feature data structure can be utilized for various applications in the field, including identifying geometric imperfections [
10,
11,
17] or detecting deformations [
16]. The reorganized reconstructed models can be viewed as digital twins, where the organized point clouds accurately represent the genuine geometric conditions of the measured structural members [
18,
19].
The cutting-edge technology, digital twin, is being explored for broader applications in structural research fields, such as numerical simulations of structural members [
20]. The geometric properties of steel members play a pivotal role in structural analysis and can be accurately characterized using laser measurements [
21]. Meanwhile, researchers have identified imperfections in measured CFS members [
22,
23], the magnitudes of which were statistically analyzed and incorporated into numerical simulations. Nevertheless, there is potential for further development in this application. Specifically, the geometry of digital twins could be directly integrated into finite element modeling [
11,
24]. However, the practical application of this research has been limited due to the computational demands of processing large point clouds and the potential for divergence in numerical simulation. Moreover, these DT-based finite element models have yet to undergo validation through testing.
This research focuses on developing a DT-based numerical simulation method for CFS members to achieve enhanced computational speeds in finite element models. These models are calibrated using axial compression tests on 27 Cee-shaped CFS members. The subsequent section introduces the research background. In
Section 3, we detail the DT-based numerical simulation methods.
Section 4 provides testing methodologies, leading to model validation discussions in
Section 5.
Section 6 contrasts the DT-based numerical simulations against traditional approaches. Additionally, this section delves into the implications of varying simulation parameters. Conclusions and prospects for future research are encapsulated in
Section 7.
3. A Simulation Method for Digital Twins of CFS Members
Digital twins accurately represent the real geometries of CFS members derived from post-processed laser measurements. However, the high density of these point clouds isn’t always necessary, especially for numerical simulations considering CFS members’ as-true geometry. The density of the point clouds should be reduced to a suitable amount to facilitate structural analysis via numerical simulation. This section introduces a simulation method using finite element modeling paired with digital twins of CFS members. The finite element analysis is executed using the ABAQUS CAE 2019 software, and appropriate modeling input files are generated accordingly.
3.1. Node Formation
Both material and geometric properties influence numerical simulations of structural members. While material properties can be ascertained through coupon testing, the geometric properties in simulations are derived from laser-based digital twins. However, the dense point clouds can’t be used directly as nodes due to their high point density. Therefore, it’s crucial to establish an appropriate mesh node configuration that reflects the accurate geometry while also de-sampling the measurement points for efficiency.
Given the assumption of a uniform cross-sectional thickness throughout a CFS member, the geometric characteristics of its central surface closely mirror that of its outer surface, as illustrated in
Figure 4. Owing to the thin-walled nature of the member, points on the centerline section can be straightforwardly acquired by translating the outer surface points by half the thickness, represented as
.
The node formation begins with the line segments of a cross-section, such as the web, flanges, and lips. Considering the left-side flange as an example (
Figure 7a), the flange is characterized through post-processing where the boundary points
are identified. The points
and
are linearly connected, setting the direction of this line as a local axis, represented by
. The lower point
, is designated as the origin. The perpendicular direction to the axis
is set as another principal axis
. Since the mesh size of the FE model is predetermined, the number of nodes on the cross-section and the distance between them can be ascertained. For instance, the left-side flange would have
nodes, as shown in
Figure 7a. A linear interpolation is carried out with boundary points
. As a result, a series of points
with uniform distances are obtained.
The node formation continues with its foundation on the measurement point clouds. Since the points are sorted and organized in sequence, adjacent points line up in a cross-sectional array. For each interpolated point , there are measurement points in its vicinity. These points are linearly fitted, and then short line segments are obtained. The intersection between a fitted line segment and the axis is considered a node . This procedure is repeated for the remaining mesh nodes of the flange till equal-interval nodes are found. The final phase involves the formulation of mesh nodes for the centerline model. The normal direction of the flange, which coincides with the direction of the axis , is identified. The translation displacement is half of the thickness . Thus, the nodes are all shifted by along the direction and the mesh nodes are obtained.
The above line-segment nodes formation method applies to all linear regions of the cross sections. However, the corners of these cross-sections require a slightly modified approach due to their distinct geometry. Take the corner between a flange and a web, for example. The boundary points of this corner, denoted by
, are obtained through the previously described post-processing algorithm. It is assumed that the corner can be fitted with an arc with radius R, the center of (
), which is set as the origin of the local polar coordinate. Similar to the line-segment formation, the number
and the angles
interval of nodes of the corner are determined in advance, as shown in
Figure 7b. The angle theta can be ascertained using Equation (1).
where
θ is the angle of the corner obtained using the dimension-finding method applied to the measurement [deg.].
A series of interpolated points can be obtained using Equations (2) and (3):
where
represents the found point in the local coordinate;
are the coordinates of the interpolated points in the cross-section coordinate system.
The second step is the same as the process for line segments. Measurement points within a density distance
around
, determined by Equation (4), are utilized to fit a short line segment. The intersection between this short line segment and the fitted arc is treated as the desired node, translated by half of the thickness
in the direction pointed to the origin
. Upon completion of this process, the node formation for corner segments is finalized. This methodology applies to all corner regions of standard CFS cross-sections.
where
represents the point cloud node coordinates;
is the distance between point cloud coordinates and short lines [mm].
3.2. Finite Element Modeling
A script file for the ABAQUS software has been developed, a sample of which is attached in the Appendix. Key parameters related to the laser-measurement point clouds are listed in the section verified in the following sections.
3.2.1. Mesh Formation
The thickness of thin-walled members is comparatively minor relative to their other dimensions. Therefore, the simulation of CFS members, uses the S4R shell element for mesh. The mesh size typically necessitates an element with approximately equal length and width dimensions. The nodes along the member thus are established based on the total number of cross-section nodes, denoted as
, where
is the number of cross-section nodes, and
is the number of longitudinal nodes. As illustrated in
Figure 8, the nodes presented in the Script file comprise four columns, preceded by the ‘*NODE’ keyword where “*” represents the beginning of the keyword in ABAQUS. The initial column indicates the numerical order, while the subsequent three columns delineate the coordinates relative to the
axes. Generally, the numerical order should be structured such that individual cross-sections are distinguishable. A recommended sequence is provided below in Equation (5):
where
is the
cross-section along the member, and
is the
node across the section.
The node’s coordinates, especially the longitudinal coordinates, must be carefully treated. The original cross-section density is set at . The value of , representing the number of longitudinal nodes, should be calculated such that the result of is an integer. Under this condition, the nodes of the cross-sections can be directly derived from the corresponding mesh nodes obtained from the previous step. Conversely, if does not yield an integer, the nodes of the cross-sections can be obtained through interpolation from the neighboring nodes of the cross-sections.
Once the mesh nodes are determined, the mesh element can be formed using the S4R element type—a linear 4-node shell element with uniformly reduced integration. This is specified in the script file with the keyword ‘*Element, type S4R’. The data structure for this section is presented in five columns, as illustrated in
Figure 9. The first column is the mesh element number order; a patch of typical mesh order numbers is illustrated in
Figure 9. The subsequent four columns represent the number of orders of nodes. The second and third columns detail adjacent nodes, specifically the
and
nodes in the
cross-section, while the fourth and fifth columns describe the
and
nodes in a
cross-section.
3.2.2. Material Properties
In a finite element model, material properties typically encompass Young’s modulus (), Poisson’s ratio (), the , the yield strength (), and the ultimate strength (). Additionally, for nonlinear analysis in finite element assessments, the stress-strain matrix is essential. These attributes are derived from material testing or existing experimental data in scholarly literature.
3.2.3. Boundary Condition
The boundary conditions in this research comprise the loading conditions and the restraint conditions. The boundary condition is assumed to be simply supported. A reference point at one end, RP1, is set to coincide with the centroid of the end cross-section. RP1 is rigidly tied to the end nodes, where it is permitted to have axial displacement and weak axis rotation. A reference point at the other end, RP2, is positioned at the centroid of the opposite end cross-section. Similarly, RP2 is rigidly tied to the end nodes, and this end is restricted to allow only weak-axis rotation.
Furthermore, the loading condition is displacement-controlled, a common approach in nonlinear structural analysis. The displacement is applied at RP1, permitting axial deformation. The initial displacement is set at of the member’s length.
3.2.4. Analysis Step
The analysis step is essential in finite element modeling. Both the robustness and accuracy of the analysis are influenced by this step. Three main types of analyses are employed in thin-walled structural analysis: ‘*Static, general’, ‘*Static, Riks’, and ‘*Static, Stabilize’. The application of these steps is slightly different. The measurement contains a number of surface imperfections that result in divergence of ‘*Static, Riks’ analysis method. The general method of ‘*Static, Riks’, is unsuitable for large high-precision models based on laser measurement. The analysis step adopts ‘*Static, Stabilize’. A more comprehensive discussion of the analysis step can be found later in
Section 6.2.2.
The energy consumption fraction is specified as 0.0002. This introduces an added viscous force to all nodes within the model. The magnitude of this force is dictated by the node’s bit removal during time increments, stabilizing the model’s computation. Additionally, parameters are set for the incremental steps: the maximum is 300, the initial is 0.001, the minimum increment is , and the maximum increment is 0.05. These step parameters can be auto-generated for comparative analyses when executing the respective script files, ultimately determining the optimal input values.