Soporte al Usuario de COSMOS/™ -- Nota Técnica Nº 76
NONLINEAR STATIC ANALYSIS OF IRON COVER PLATE
Productos: COSMOS/DesignSTAR y COSMOS/NonLinear
Versión: Todas las Versiones
Categoría: Preprocesado, Análisis y Postprocesado
Ultima revisión: Febrero-2002
This document describe the benchmark FEA on COSMOS/DesignSTAR in order to obtain accurate results of stress, displacements and residual plastic deformation of an "iron cover plate" under a compressive load of 26.6 Tm, see image below:
Problem Description
The target of the FEA simulation is to achieve the following results & benefits:
- Plastic Deformation: to obtain the plastic deformation (residual
vertical displacement) after applying 5 cycles of loading/unloading. The load applied here
is 2/3 of the nominal load, ie, (2/3) x 40 Tm = 26600 kg. The target is to obtain a
permanent plastic deformation less than 2 mm. Real life test measurements found a
permanent plastic deformation of 0.4 mm << 2 mm admisible, so model need to be
optimized in order to reduce design weight.
- Failure Load: obtain the failure load that cause the part to fail. The test is done applying (2/3) x 40 Tm = 26600 kg in 5 cycles and at the end to increase loading till 40 Tm (ie, 40e3 kg) and maintain loding level during 30 seg., and then to increase loading till reaching fracture of the part. Real life test measurements found a fracture load = 500 KN, where the norm EN-124 requires a minimun fracture load = 400 KN, so model need to be optimized in order to reduce design weight.
The "Test Data" are obtained after 5 cycles loading & unloading between load 0 kg and 26.6 Tm.
1. Analysis Type:
Nonlinear static analysis, Plasticity vonMises with solid TETRA10 elements.
2. Geometry Description:
The geometry is a solid part created in SW 2001, see image below:
SW model of the part
3. Loads & Boundary Conditions:
The load applied is 2/3 of the nominal load, ie, (2/3) x 40 Tm = 26600 kg using a rigid piston of outside Diameter Ø250 mm:
Contact between rigid piston &
cover plate
The part exhibit load & geometry symmetry, allowing to study half cover plate:
Loading & Supports details
The load is applied on 5 cycles of loading/unloading, according the figure below:
Loading Curve
4. Material Properties:
The material is Malleable Cast Iron, with the following properties :
- EX = 1.85E6 kg/cm2
- NUXY = 0.275
- SIGYLD = 4390 Kg/cm2
- ULTIMATE STRESS = 6280 kg/cm2
5. Linear Static Solution: Contact Model (
conjunto_sw.ZIP -- 210 kb)
The first task was to investigate the effect of contact between rigid piston cover plate, creating two models: one with contact and the other with the cover plate only, applying the load directly to the plate. Because symmetry, only half model was used, splitting the load as well and imposing the corresponding displacement boundary conditions:
Loads & BCs in the COSMOS/Works
model
The assembly was meshed with high order TETRA10 elements with Elemento Size = 10 mm, applying a mesh control in component "rigid piston" using a coarse element size = 30 mm in order to reduce the total size of the model.
Mesh Details in COSMOS/Works model
The following image shows the resultant vertical displacement for the applied load of 26.6 Tm -- please note that the maximun displacement is less than 1.8 mm, where the measured values (Test Data) indicate values bigger then 4 mm (!!).
Results of Vertical Displacement UY
Results of linear vonMises stresses
(not sense, only included for comparison purposes)
6. Linear Static Solution: Model without Rigid Piston (
Blas_1160_lin.ZIP -- 20 Kb)
The following step was to open the SW part in DesignSTAR and apply loads directly to the cover plate without considering contact between rigid piston and cover plate, and compare results. Both the mesh & material properties are the same as C/W model.
COSMOS/DesignSTAR model meshed with
solid elements (Element Size = 8.0 mm)
The maximun values of UY displacements results were at the same level of the CW model (about 1.8 mm), validating this way not need to consider the rigid piston in the model + contact, but their load applied directly
Results of Vertical Displacement UY
Results of linear vonMises stresses
(not sense, only included for comparison purposes)
7. Nonlinear Static Analysis: Solid Model (
Blas_1160_nonlin.ZIP -- 20 Kb)
This model includes all the steps to define a nonlinear static analysis: the plasticity model used in the analysis is based on von Mises yield criterion with bilinear isotropic hardening rule, defining the bilinear stress-strain curve by EX, SIGLYD and ETAN. EX defines Youngs´s modulus, ETAN defines the Tangent Modulus, and SIGYL defines the Yield Stress Sy.
We also consider in the analysis the geometric nonlinearity using large displacement formulation with total lagrangian method to take into consideration the large displacement effect, but induced strains to remain small. The image below shows the material properties used in the analysis (ETAN was assigned a value of 20% of Elastic modulus):
Results of linear vonMises stresse
The next step is to define the "Time Curve" to control the incremental application of loads vs. time. The Time curve defined is the following (between start time = 0 sec. till end time = 350 sec.):
T I M E C U R V E S :
(Defining forces, pressures, & nodal temperatures)
Curve number . . . . . . . . . . . . . . . . . = 1
Number of points . . . . . . . . . . . . . . . = 11
Time Value
0.00000 0.00000
60.000 1.0000
70.000 0.00000
130.00 1.0000
140.00 0.00000
200.00 1.0000
210.00 0.00000
270.00 1.0000
280.00 0.00000
340.00 1.0000
350.00 0.00000
Definition of Time Curve
The applied load of 13300 kg was associated to time Curve#1
Load associated to Time Curve
X-Y Plot of resulting Vertical Load
FY vs. Time
The following step is to setup the nonlinear analysis parameters:
Parameters for NonLinear Analysis
The Nonlinear solution Time parameters defined are the following:
- Time at the start of step-by-step solution . . = 0.00000
- Time at the end of step-by-step solution . . . = 70.000
- Time step increment . . . . . . . . . . . . . = 2.5000
- Total number of solution steps . . . . . . . . = 28
Force Control information:
- Iterative technique used: Regular Newton-Raphson
- Stiffness matrix reformation interval = 1
- Number of steps between equilibrium iterations = 1
- Maximum number of equilibrium iterations allowed . . . = 20
- Displacement tolerance for equilibrium iterations . . = 0.10000E-02
Deformed shape plots at steps:
- First time step . . = 1
- Last time step . . = 70
- Time step Increment . . = 1
The solid part was meshed using TETRA10 high order elements with element size = 8 mm, see image of mesh details below:
- Number of Equations . . . . . . . . . . . . . .(NEQ) = 148428
- Number of Nodal points . . . . . . . . . . . (NUMNP) = 49476
- Number of Elements. . . . . . . . . . . . . . (NUME) = 25170
- Number of Blocks. . . . . . . . . . . . . . . (NBLK) = 1
- Number of solution steps . . . . . . . . . . (NSTEP) = 28
Detail Mesh Information
All required steps to perform the nonlinear static analysis are finished, so the following task is to run the nonlinear solution solver. Here you are a copy of the solution process:
To see how solution progress ...
The total Solution Time for this NonLinear Static Analysis is the following (Hardware: Pentium 4 at 1.7 GHz, 1 GB RAM Memory & Windows XP):
- Time for Input Data Transfer from Database . . . . = 9
- Time for Address, Block and (Mass) Computation . . = 0
- Time for Structure Stiffness Matrix Calculation . . = 0
- Time for Computation of load vectors . . . . . . . = 22
- Time for LDL Decomposition . . . . . . . . . . . . = 4466
- Time for Forward reduction and Backsubstitution . . = 0
- Time for Gap iterations . . . . . . . . . . . . . . = 0
- Time for Printout of Displacement solutions . . . . = 63
- Time for Stress Calculation and Stress printout . . = 178
- Time for writing Postprocessing information . . . . = 80
- Time for Miscellaneous operations . . . . . . . . . = 43
- T O T A L S O L U T I O N T I M E . . . . . . . = 4860 sec. (81 min.)
The results of maximun displacements and streses at time T = 60 sec. (maximun value of load) are the following:
NonLinear Displacement Results at
Step = 24 (Time = 60 sec.)
X-Y Plot of UY displacement vs. Time
von Mises Stress Results for Step =
24 (Time = 60 sec.)
8. Conclusion
Un summary, nonlinear static results of max. displacements are UY = 1.8 mm, and are in agreement with those results obtained using the linear static solution. Also, the X-Y plot of response shows a linear behaviour till reaching the total load of 26.6 Tm.
