Home → Gantry crane → Finite Element Analysis of Truss Girder of Long Span Double Girder Gantry Crane
Finite Element Analysis of Truss Girder of Long Span Double Girder Gantry Crane
Abstract
This paper uses finite element analysis to evaluate the structural performance and optimize the design of the truss girder of a 75t+75t, 42m long-span, double-girder gantry crane. A parametric finite element model was established using ANSYS software. Loading was performed according to the corresponding operating conditions specified in the crane design specification to analyze the strength, stiffness, and stability of the girder structure. The study demonstrates that finite element analysis can accurately identify the stress distribution and deformation of the girder, effectively improve structural weaknesses, and ultimately determine a truss girder structure that meets design requirements. This paper systematically describes the entire process, from model establishment, load calculation, boundary condition setting, to results analysis, providing a reliable theoretical basis and technical support for the design of long-span gantry cranes.
Introduction
Gantry cranes are essential equipment in modern industrial production and logistics transportation. The performance of their girder structures is directly related to the operational safety and service life of the entire crane. For long-span double-girder truss gantry cranes (e.g., 42m), the main girder design presents a particularly challenging challenge: ensuring sufficient strength and stiffness while minimizing deadweight to maximize economic efficiency. Traditional design methods rely primarily on empirical formulas and analogical design, making it difficult to accurately predict structural response under complex loading conditions. Finite element analysis (FEA) technology provides an effective means to address this problem. Computer simulations can visually display the stress distribution and deformation of the structure, significantly improving design efficiency and reliability.
Truss structures, with their advantages of light weight, high rigidity, and low wind resistance, are particularly suitable for the design of main girders for long-span gantry cranes. Compared with box girders, truss girders more fully utilize material strength, with each member primarily bearing axial tension or compression, resulting in a more balanced stress distribution. However, truss structures have complex joint connections and significant localized stress concentration, necessitating detailed FEA analysis to assess their safety.
This article, drawing on engineering examples, details the FEA method for the truss main girder of a long-span double-girder gantry crane, including model simplification principles, load combination methods, boundary condition processing, and result evaluation criteria, providing a reference for the design of similar structures.
Crane Parameters and Model Establishment
Main Technical Parameters of the Crane
The double-girder truss gantry crane studied in this paper has the following main technical parameters:
Outrigger configuration: One rigid outrigger, one flexible outrigger
Total beam length: Approximately 45m (including the cantilever)
Steel material: Q345B
Geometric model simplification
When establishing the finite element model, appropriate simplifications were made to the actual structure while ensuring accuracy:
Main beam structure: Main load-bearing chords and web members were retained, while small-sized connecting plates and non-load-bearing components were ignored.
Joint treatment: Welded nodes were simplified as rigid connections, taking into account the stiffness effects of the node area.
Outriggers and end beams: Outriggers and end beams were treated as boundary conditions, focusing on the load state of the main beam itself.
Connection components: High-strength bolt connections were simplified as bound contact or coupling constraints.
Finite Element Model Creation
A parametric finite element model was created using ANSYS software. The specific steps are as follows:
Element Type Selection: Beam188 beam elements were used to simulate truss members. Beam188 is a two-node, three-dimensional element based on Timoshenko beam theory. Each node has six degrees of freedom, allowing for shear deformation effects and making it suitable for analyzing slender members.
Material Property Definitions:
Elastic Modulus E = 2.06 × 10⁵ MPa
Poisson’s Ratio ν = 0.3
Density ρ = 7850 kg/m³
Yield Strength σs = 345 MPa
Sectional Properties:
Top Chord: 400 × 400 × 12 Box Section
Bottom Chord: 400 × 400 × 10 Box Section
Web: 200 × 200 × 8 Box Section or H-Beam
Meshing:
Use segmented sizing to ensure each member is divided into at least three elements.
Mesh refinement is applied to node areas to capture local stress concentrations.
The total number of nodes in the model is approximately 8,500, and the number of elements is approximately 12,500.
Table: Cross-sectional parameters of main members of truss main beam
Member type
Cross-sectional form
Size(mm)
Cross-sectional area(cm²)
Moment of inertiaIx(cm⁴)
Upper chord
Box type
400×400×12
185.6
52300
Lower chord
Box type
400×400×10
156.0
45600
Vertical abdominal bar
H type
HW200×200
64.3
4770
Oblique abdominal bar
Round tube
Φ219×8
53.0
2510
Boundary condition simulation:
Apply fixed constraints (full constraints) at the connection between the outrigger and the end beam.
Considering the elastic support characteristics of the actual structure, set appropriate spring stiffness to simulate foundation flexibility.
Load Analysis and Working Condition Combination
Load Types and Calculations
The loads acting on the truss main beam primarily include the following:
Permanent Loads (Dead Loads):
Structural Weight: Automatically calculated by the software based on material density and geometric dimensions, with a 1.1 magnification factor to account for the added weight of welds, connecting plates, and other components.
Fixed Equipment Weight: This includes walkways, railings, electrical equipment, and other components, applied as a uniformly distributed load, totaling approximately 18.5 kN.
Variable Loads (Live Loads):
Lifting Load: Rated lifting capacity is 75 tons (735 kN). Considering a dynamic load factor of φ₂ = 1.15, the design load P = 735 × 1.15 = 845.25 kN.
Trolley Weight: A single trolley weighs approximately 12 tons (117.6 kN), with a double trolley weighing a total of 24 tons.
Inertial Load: Caused by crane starting and braking, calculated as 10% of the vertical load and 5% of the horizontal load. Lateral force during skew operation: Consider 10% of the maximum wheel pressure.
Environmental loads:
Wind load: Calculated in operating mode at wind speed level 6 (wind pressure 250Pa); in non-operating mode at maximum wind speed level 12 (wind pressure 1200Pa).
Temperature load: Consider a temperature fluctuation of ±30°C.
Combination Analysis of Load Conditions
According to GB/T 3811-2008 “Crane Design Code,” the following four typical load conditions were selected for combined analysis:
Load Condition 1: Vertical Static Load Condition
1.0 × Deadweight + 1.4 × Hoisting Load
Used to evaluate the static strength and stiffness of the main beam.
Concentrated Load: Trolley wheel pressure is converted to nodal forces using the MPC184 multi-point constraint element to avoid local stress distortion.
Uniformly Distributed Load: The weight of the walkway, railing, etc. is converted into linear loads and applied to the chord.
Wind Load: Calculated using the shape coefficient method and applied perpendicular to the windward surface.
Temperature Load: A uniform temperature field is applied using the thermal analysis module.
Finite Element Calculation Results and Analysis
Stress Analysis Results
ANSYS calculations were used to obtain stress distribution contours for the main beam under various load conditions. Overall, the maximum stress occurs at the mid-span junction between the lower chord and the web, as well as near the outriggers, consistent with theoretical expectations.
Condition 1 (vertical static load):
Maximum stress in the lower chord at midspan (σmax) = 187 MPa
Maximum compressive stress in the upper chord (σc) = 156 MPa
Maximum stress in the web (σw) = 132 MPa
Local peak stress concentration area reaches 215 MPa
Condition 2 (vertical dynamic load):
Dynamic effects increase stress by approximately 15%
Maximum stress in the lower chord at midspan (σmax) = 218 MPa
Stress fluctuations at locations with significant impact effects reach ±25 MPa
Condition 3 (horizontal load):
Lateral forces cause significant torsion in the main beam
Stress in the unilateral chord increases by 20-30%
Maximum combined stress (σcomb) = 245 MPa
Condition 4 (special load):
Structural stress levels are low under non-operating wind loads
Maximum stress (σmax) = 168 MPa
Local high stress occurs in the leg connection area
The maximum equivalent stresses under all conditions are below the allowable stress of 295 MPa for Q345B steel (calculated at 0.85 σs), meeting strength requirements.
Deformation Analysis Results
The main girder’s stiffness is a key indicator for evaluating the performance of long-span cranes. According to GB/T 3811, for double-girder truss gantry cranes, the vertical static deflection of the main girder should be controlled within L/700 (L is the span). This means that for a 42m span, the allowable deflection is 60mm.
Vertical Static Deflection:
Under Condition 1, the maximum deflection at midspan, fmax, is 52.3mm.
The deflection-to-span ratio, fmax/L, is 1/803, less than 1/700.
Meets the stiffness requirements.
Horizontal Displacement:
Under Condition 3, the horizontal displacement at midspan, d, is 38.7mm.
The horizontal displacement-to-span ratio, d/L, is 1/1085.
Sufficient lateral stiffness reserve is achieved.
Dynamic Deflection:
Under Condition 2, the deflection fluctuation range is 45-58mm.
The vibration frequency is 1.2Hz, far below the trolley operating frequency (0.5-0.8Hz).
No resonance risk.
Table: Summary of main beam deformation calculation results
Working conditions
Maximum vertical deflection(mm)
Allowed values(mm)
Maximum horizontal displacement(mm)
Stress/deflection safety margin
Working conditions1
52.3
60
–
15%
Working conditions2
58.0
–
–
12%
Working conditions3
–
–
38.7
18%
Working conditions4
22.5
–
15.2
30%
Buckling Stability Analysis
Long-span truss structures require special attention to both global and local stability. ANSYS eigenvalue buckling analysis is used to calculate the buckling modes and critical load factors of the structure under ultimate loads.
Based on initial finite element analysis results, the main beam exhibited localized stress concentration and uneven material utilization. The following optimization measures were implemented to improve the design:
Topology Optimization
Web Member Layout Optimization:
Web member spacing in the mid-span area was reduced from 2.1m to 1.8m.
K-type trusses were used near the outriggers to replace the original cross-web members.
Stress concentration factors were reduced by 27%.
Chord Cross-Section Optimization:
The upper chord remained unchanged at 400×400×12 mm.
The lower chord was thickened to 400×400×14 mm in the middle 20m.
The ends were restored to 400×400×10 mm.
Maximum stress Force reduced to 202 MPa
Parameter optimization
Height adjustment:
Main beam height increased from 3.8m to 4.2m
Deflection reduced by 18.5%
Weight increased by approximately 5%
Material optimization:
Q390B steel replaced Q345B in high-stress areas
Q235B steel used for non-critical web members
Overall cost reduced by 3.2%
Joint optimization
Gust plate design:
Increased gusset plate radius in stress concentration areas
Used arc transitions instead of right-angle connections
Local peak stress reduced by 35%
Connection improvements:
Used a hybrid of high-strength bolts and welding at key nodes
Improved joint fatigue life
Table: Comparison of main beam performance before and after optimization
Performance indicators
Initial Design
Optimized design
Improvement
Maximum equivalent stress(MPa)
245
202
↓17.6%
Mid-span deflection(mm)
52.3
42.6
↓18.5%
Structural deadweight(t)
86.7
84.3
↓2.8%
First-order buckling load factor
4.27
5.12
↑19.9%
Manufacturing cost (10,000 yuan)
124.5
120.5
↓3.2%
The optimized main beam structure has significantly improved in strength, stiffness and stability, while achieving the goals of lightweight and economy.
Conclusions and Recommendations
Research Conclusions
Finite element analysis verified the safety and reliability of the main girder design for a 42m span double-girder truss gantry crane. Stress and deformation under all operating conditions met regulatory requirements.
The truss main girder demonstrates significant advantages in long-span applications. Compared to a box girder of the same span, it reduces deadweight by approximately 25% and wind load effects by over 30%.
The structural weaknesses primarily occur at the mid-span lower chord node and outrigger connection area. Targeted optimization can effectively improve stress distribution.
The parametric finite element model provides a convenient tool for the rapid design and analysis of similar structures, significantly shortening the design cycle.
Design Recommendations
Manufacturing Process Control:
Strictly control chord straightness deviation (≤L/2000)
Ensure welding quality and dimensional accuracy at the node locations
Material Selection:
Use high-strength steel (Q390 and above) in high-stress areas
Q235B can be used for non-critical components to reduce costs
Corrosion Protection Design:
Use a thermal zinc spraying + heavy-duty anti-corrosion coating system
The interior of the closed box section should be treated with anti-rust treatment
Monitoring and Maintenance:
Establish long-term strain monitoring points at the mid-span and support legs
Regularly inspect key nodes for cracks
Future Research Directions
Fatigue Performance Analysis:
Fatigue life prediction based on professional software such as FEMFAT
Study the fatigue characteristics of different node types
Wind Vibration Analysis:
Consider the dynamic response under pulsating wind loads
Evaluate aerodynamic stability
Application of Intelligent Optimization Algorithms:
Use genetic algorithms, particle swarm algorithms, etc.
Contact our crane specialists
Send us a message and we will get back to you as soon as possible.
