Optimization of simple linear and advanced nonlinear problems using TOSCA and ABAQUS R. Meske and M. Friedrich FE-DESIGN GmbH, Haid-und-Neu Str. 7, 76131 Karlsruhe, Germany “The world is non-linear.” This statement is familiar to all ABAQUS users. In their daily work there are a lot of problems which are not to be only analyzed, but should be improved or optimized. This demands the availability of an optimization system which can handle not only simple linear but also advanced non-linear problems. The optimization system TOSCA with interfaces to industry standard solvers like ABAQUS offers the capability to treat linear and non-linear problems in an optimization. Topology and shape optimization of ABAQUS models with an ar bitrary number of load cases and boundary conditions can be performed with TOSCA. A parameterization of the model is not needed, which reduces the modeling effort and allows greater flexibility in the optimized structure. Most features of ABAQUS like contact, non-linear material and special elements can be used.
1. The optimization system TOSCA TOSCA is a modular system for non-parametric structural optimization. Topology and shape optimization of FE models with an arbitrary number of load cases and boundary conditions can be performed with TOSCA. A parameterization of the model is not needed, which reduces the modeling effort and allows greater flexibility in t he optimized structure. The optimization algorithms are based upon mechanical optimality criteria, which makes t he optimization fast and robust (Bakhtiary et al., 1996). The optimization procedure with TOSCA is sketched in Figure 1. Th e structural response of the component is calculated in each iteration with an external FE solver. The high quality of the results is guaranteed by using approved and accepted industry standard solvers like ABAQUS. The user can work with his favorite solver in his favorite pre- and postprocessing environment and does not need additional training for a new solver. Already existing FE models can be used directly in the optimization. The result of the o ptimization can be visualized with most common FE-postprocessors like ABAQUS/Viewer and is available in various formats for the further processing in the virtual product development process. A closed development process can be achieved by the interaction of the components of TOSCA from the first concept to the optimized geometry in the CAD system.
2003 ABAQUS Users’ Conference
1
FEM-Preprocessing
model.fem
Opt-Preprocessing
model.par
model_xxx.fem
FEM-Postprocessing
model_xxx.res
Opt-Postprocessing
OPT Results
Figure 1. The optimization process with TOSCA. The principal capabilities of TOSCA are: •
Stable and fast optimization algorithms based on optimality criteria
•
Efficient handling of very large models
•
Optimization with an unlimited number of load cases
•
Use of various different stress hypothesis
•
•
•
•
•
2
Graphical user interface TOSCA.gui for definition, start and post processing of the optimization Solver interfaces: ABAQUS, ANSYS, I-DEAS and MSC.Nastran. Postprocessor interfaces: ABAQUS/Viewer, ANSYS, FEMAP, I-DEAS, MEDINA, MSC.Patran. Nearly all continuum, shell and membrane elements are supported in the optimization. The remaining elements can be used outside t he optimization domain. Optimization possible with a non-linear analysis (contact, non-linear material, large deformation)
2003 ABAQUS Users’ Conference
TOSCA is based on the optimization kernel CAOSS and is d eveloped and distributed by FEDESIGN. More information about TOSCA can be found on www.fe-design.com.
2. Linear or non-linear analysis within the optimization? Topology optimization is used to find a structure within a given design space, which carries the specified loads in the best way, such that the strain energy density in the structure is minimal with respect to other possible structures. Because th e iterative optimization procedure needs 15 ABAQUS analysis for the topology optimization and the whole design space has to be meshed with elements, it has always to be considered whether the relevant load cases and the system behavior can be described with a linear analysis in order to get a fast response. In some cases, a non-linear analysis must be used to model the problem correctly, especially if the system behavior is changed significantly during the optimization. Shape optimization is used to perform improvements of existing designs. Five design cycles are usually sufficient to get a significant improvement. If an already sophisticated non-linear ABAQUS model exists to describe the component, this should always be preferred to the creation of a new linear model. Another advantage of an optimization with a non-linear model is that no non-linear verification analysis has to be performed with the modified component after the optimization.
3. Optimization with contact The exact boundary conditions can very often not be given exactly during the design process of a new component. Non-linear boundary conditions may occur due to contact problems. The contact conditions should be taken into account during the optimization of the component, because the transmission of forces and therefore the bound ary conditions may change due to the iterative modification of the geometry and stiffness of the component. A substitution of the contact conditions by equivalent nodal forces is a simplification, which may result in less optimal results. Moreover, this substitution is a time-consuming manual process, which should be avoided to guarantee a fast and reliable development process. Therefore it is desirable to allow general contact definitions at the boundary of the optimization domain in structural optimization. Due to the modular structure of TOSCA this is possible for ABAQUS users in the usual way. The user creates an ABAQUS model with the required contact definitions. Afterwards the optimization task is defined. The existence of the contact definition does not need to be taken into account b y the optimization algorithm. The contact problem is implicitly included in the optimization by the contact forces and the resulting stresses. Thus the user can take full advantage of the capabilities ABAQUS in contact calculation.
3.1
Topology Optimization with Contact
The application of topology optimization with TOSCA with non-linear boundary conditions was shown first in (Meske, Sauter & Güngör, 2001) w ith a simple connection rod with contact 2003 ABAQUS Users’ Conference
3
conditions. An industrial application was shown in (Sauter & Meske, 2001), where a complete linear guidance system was investigated. The contact deformation between rolling elements and raceway was defined b y a series of non-linear spring elements, which allowed a realistic description of the system. For topology optimization the user has to decide if it is necessary or not to consider contact conditions within the optimization. A linear analysis should always be preferred due to the iterative procedure, because this analysis must be performed 15 times for one optimization. Nevertheless, a contact analysis must be used, if a change in the transmission of forces due to the modification of the stiffness of the component is expected. A classical example for such a component is an engine rocker arm.
3.2
Shape Optimization with Contact
The following real industry example for shape optimization with contact was first presented at a local NAFEMS seminar (Meske, Mulfinger & Warmuth, 2002). The component investigated is the current connection rod in the Ford 1.25/1.4 ZETEC-SE engine. A connection rod is a classical example for shape optimization because it has to endure high loads, should not have more mass than absolutely necessary and a modification of the surface geometry is admissible during the virtual development process. An ABAQUS model of the connection rod was provided by courtesy of Ford AG. The model corresponds to the final d esign of the component, hence stress and other properties were already improved manually to a sufficient level. The model consists of 8 parts according to Figure 2. The parts interact via contact definitions with each other.
Figure 2. Assembly of connection rod Ford 1.25/1.4 ZETEC-SE The load history was divided in 6 steps:
4
1.
Pressing in the piston pin, tighten the bolt
2.
Fix the bolt load
3.
Initializing contact for the tension load case by applying a controlled displacement
4.
Assembly loads and inertia forces at maximum overspeed (maximum tensile load)
2003 ABAQUS Users’ Conference
5.
Initializing contact for the compression load case by applying a controlled displacement
6.
Gas pressure and inertia forces at maximum torque speed (maximum compressive load)
Important to notice is that the inertia forces were modeled as true inertia loads on element basis. A modification of the geometry during the optimization process led therefore to an automatic correct update of the applied forces. Furthermore has to be mentioned that the model could be used in the optimization without any modifications. This offers a great flexibility for the ABAQUS user, because very sophisticated models can be used for analysis and optimization. The target of the shape optimization of the connection rod was the minimization of the maximum von Mises stress of step 4 and 6 in the inner contour of the shaft. The volume has to remain constant during the optimization. This target allows Ford to have an additional reserve for future power enhancements for this component. The design area was chosen from all nodes from the in ner contour and defined via a node group. The element group of the shaft was used to defined the area for mesh smoothing, which is important to guarantee a sufficient mesh quality after the modification of the position of the design nodes. The optimization should terminate after 5 optimization cycles.
Figure 3. Maximum Equivalent Stress of Initial and Optimized Geometry The maximum von Mises stress for the initial and the optimized geometry after 5 design cycles is shown in Figure 3. A moderate stress concentration can be observed on the inner contour of the initial model near the crankshaft, which was caused by the compression load case. This stress concentration was reduced and the homogenization of the stress in the design area can be clearly seen. The evolution of the maximum von Mises stress during the optimization is plotted in Figure 4 for the compression and tension load case. A reduction of 17% of the original maximum stress was
2003 ABAQUS Users’ Conference
5
reached in only 5 design cycles. This fast and robust optimization behavior is especially important for real-world analysis models in order to keep the total computation time manageable. Maximum Equivalent Stress 100%
80%
60%
40%
20% Tension Compression
0% 0
1
2
3
4
5
Optimization Cycle
Figure 4. Maximum von Mises stress in the design area for step 4 and 6. It has to be emphasized that the start m odel was already improved manually in several d esign cycles. It is obvious that the improvement would be even stronger for an unimproved design. The modified geometry can be obtained either directly from the final FE-model or exported as surface mesh in STL or IGES format and imported into the CAD system. Another real world example for shape optimization with contact was presented at the German ABAQUS Users Conference 2002 (H affner, 2002). A towing hoe was improved from a first design with maximum equivalent stress of more than 1500 MPa to a final design with a m aximum equivalent stress of about 1000 Mpa. This was reached with a volume increase of only 7%. The final design is now realized as series component in the new Audi A8.
6
2003 ABAQUS Users’ Conference
Figure 5. Towing Hoe from new Audi A8 (Haffner, 2002) (Image courtesy Audi AG) 3.3
Direct Optimization of Contact Surfaces
Another application of TOSCA is the direct optimization of contact surfaces with the objective to receive a homogeneous distribution of contact stresses. This is possible with TOSCA.shape and can be used to remove singular stress fields at the edge of two contact partners of different geometry like a shrink fit or the contact of a small body with a larger body. The example in Figure 6 shows the optimization of the contact surface of a shirnk-fit. The radius of the shaft was 310.6 mm, the radius of the hub 310 mm. An A BAQUS model with axisymmetric elements was used. High stresses arise due to the corner singularity. The design area were all nodes of the inner contour of the hub, the objective was to reach a homogeneous von Mises stress of 250 MPa in the contact zone. The optimization created a profile for the inner contour from 310 mm to 310.08 mm which led to a nearly homogeneous stress at the contact sur face. This technology can be used to obtain the contour of a profiled bore in the piston or connection rod for the piston pin.
2003 ABAQUS Users’ Conference
7
Singularity
500 SIGV (Start) SIGV (Opt) 450
] 400 a P M [ V G I S350
300
250 0
50
100
150
200
250
300
350
x [mm]
Figure 6. Shape Optimization of the Contact Surface of a Shrink-Fit
4. Optimization with hyperelastic material Finite Element Analysis of rubber p arts normally contain at least two nonlinearities: large deformation and nonlinear (hyperlastic) material. There are commercial material laws available as well as own developed ones, which can be integrated as user subroutine in ABAQUS. For the optimization of those problems it is necessary to use all the n onlinearities to get the right response from the system (Friedrich et. al. 2001; Friedrich et al. 2002; Meske, Sauter, Friedrich, 2001). A standard requirement in design of rubber parts for vibration control systems is to create a design with certain stiffness(es) and high durability. The technique of topology and shape optimization can fulfill those requirements. The following example will show the application of ABAQUS and TOSCA for the optimization of a camshaft amortizer. The torsional load and the function of the rubber part is similar to a torsional vibrational damper which is shown in Figure 7.
8
2003 ABAQUS Users’ Conference
Belt disk Rubber Rubber
Hub
Slide bearing Impetus flange
Figure 7: Torsional vibration damper (TVD) (Images Courtesy of Freudenberg Forschungsdienste KG) For a customer, a design change of an camshaft amortizer had to be done. For the original design the torsional stiffness and durability had already been prooved, but now openings for the assembly had to be included. Including circular openings in the existing part means lower stiffness and higher stresses.
Requested Properties: Same Stiffness Same Durability Same Volume • • •
Figure 8: Requested Design Change (Images Courtesy of Freudenberg Forschungsdienste KG) Therefore the question was how to design the cross section of the part and the shape of the holes to reach the same stiffness and same durability. As the reason for failure is to see in stresses and strains, those parameters should not increase in comparison to the reference part. The rubber volume should remain more or less the same.
2003 ABAQUS Users’ Conference
9
To find a new desig whi ch fulfills all the requests, an optimization procedure including various steps had to be performed: Topology optimization of the cross s ection • Shape optimization of the cross section • Shape optimization of the openings •
Reference Part
Optimized Part
Prototype
Figure 9: From Design Space to Prototype (Images Courtesy of Freudenberg Forschungsdienste KG) A very important information was the torque stiffness comparison of the reference and optmized part. As shown in Figure 10, the difference is negligible. The volume of the new design is about 4% higher which is acceptable.
Figure 10: Torque Moment (Images Courtesy of Freudenberg Forschungsdienste KG) Stresses (1st principle stress) and strains are smaller than in the reference part which affects the durability. Based on the results of the optimization, a prototype was built and durability testing
10
2003 ABAQUS Users’ Conference
performed. The results in Figure 11 show that the new design has – although with openings – better properties than the reference part. The whole optimization and design process up to prototype was performed in about 4 weeks.
Figure 11: Durability Testing (Images Courtesy of Freudenberg Forschungsdienste KG)
5. Optimization using ABAQUS/Explicit Many physical problems inhibit contact, large deformation and plasticity. These class of problems can be solved very efficiently using ABAQUS/Explicit. Due to the compatibility of the input syntax of Standard and Explicit it was possible to extend the A BAQUS interface of TOSCA to support ABAQUS/Explicit. This combination offers new possibilities for the optimization of complex problems. The following example of a clip should demonstrate the procedure. The clip consist of a polymeric material and should hold a steel bar. The model consists of 531 nodes, the clip is a linear-elastic material, the steel bar is modeled as rigid surface. A pull out test is performed with constant acceleration. Contact with friction is defined between clip and bar. The explicit analysis with ABAQUS/Explicit need about 25000 increments, which take 32 CPU seconds per analysis on a current PC.
2003 ABAQUS Users’ Conference
11
Figure 12. Explicit model of a clip (design nodes highlighted) The model of the clip is shown in Figure 12. The design nodes are defined as n ode set. Each node in this set can be translated by the shape o ptimization. Two cylindrical restriction areas were defined on the tips of the clip and another rectangular restriction are at the bottom. The objective was to reach a homogeneous strain energy density distribution on the outer contour, which results in a decrease of the maximum strain energy density in the inner contour. This is a special case of shape optimization, because the location of the maximum stress in the model is not in the design area. The volume was kept constant during the optimization and the optimization was terminated after 5 cycles. The strain energy density w as extracted from quasi-static time history at 20 intervals which were interpreted from TOSCA as single load cases.
Figure 13. Shape optimization of a clip (left: initial model, right: optimized model)
12
2003 ABAQUS Users’ Conference
The optimization results in a decrease of the maximum von Mises stress in the inner contour by 7% and an increase of the stiffness of the clip by 6.5% (see Figure 13). If a special stiffness is required for this component, it can be reached by modification of the target volume. Table 1 shows the reaction force and the maximum von Mises stress of the optimized clip in relation to the initial model as function of the target volume.
Table 1. Reaction force and maximum stress of optimized clip. Target Volume
Reaction Force
90% 100% 110%
81% 107% 138%
Maximum von Mises stress 89% 93% 102%
This example was used to demonstrate the principal procedure with TOSCA and ABAQUS/Explicit. In fact, a linear static analysis with fixed widening of the clip leads almost to the same result. The integration of ABAQUS/Explicit becomes important as soon as non-linear material behavior is involved or the quasi-static contact analysis is required. The next example is the optimization of a ball joint. Again a pull-out test is performed to evaluate the maximum reaction force. The pull-out test is a misuse load case and very strong plastic deformation take place. The initial configuration and the position of maximum stress is shown in Figure 14. Such an application cannot be handled with a linear static analysis and therefore must be optimized with a non-linear explicit analysis, as well.
Figure 14. Pull-out test of a ball joint, von Mises stress (Images courtesy of TRW Automotive) The design target was to increase the reaction force. D ue to geometric restriction from the functionality of the ball joint only the nodes on the top surface can be changed by the optimization. For the optimization, the volume was held constant and a minimization of the total strain energy density was set as objective function. The total strain energy density is the sum of plastic and elastic strain energy density. It has to be used as design response due to the strong plastic deformations and is a good measure for both elastic and plastic deformations.
2003 ABAQUS Users’ Conference
13
Figure 15. Optimization of ball joint, total strain energy density (left: initial model, right: after 5 design cycles) (images courtesy of TRW Automotive) The distribution of the total strain energy density is shown in Figure 15. A reduction of 25% of the initial value was reached after 5 optimization cycles. The reaction force in this case was increased only slightly by 2%. A further increase would be reached by a volume increase of the component, which was not performed because of a not sufficient mesh quality.
6.
Conclusions
The use of structural optimization tools in the early stage of the development process offers new potential in the virtual product development. T he development process becomes faster and more efficient by using topology and shape optimization. This results in structures which are lighter, stronger and more durable w hich constitutes a competitive advantage for the companies that use this solutions. The optimization system TOSCA provides an integrated solution for structural optimization of realworld applications. It has reached wide spread acceptance in industry and offers interfaces to all mayor FE-solvers. The combination of TOSCA and ABAQUS offers the possibility to perform not only structural optimization of linear problems, but also of advanced non-linear applications.
7.
Acknowledgement
The research for the optimization based on a non-linear analysis was partly funded by the German research project Elano (see www.elano.org).
14
2003 ABAQUS Users’ Conference
8.
References
The listed publications are available as do wnload from www.fe-design.com.
1.
Bakhtiary, N; Allinger, P; Friedrich, M; Mulfinger, F; Sauter, J; M üller, O; Puchinger, M. “A new Approach for Sizing, Shape and Topology Optimization”, SAE International Congress and Exposition 1996, 26.-29. February 1996, Detroit/Michigan, USA.
2.
Friedrich, M., Meske, R., Sauter, J., “Optimierung von Gummi-Metall-Bauteilen mit TOSCA und ABAQUS”, 2001 ABAQUS Users’ Conference, Freiburg, 24.-25. September 2001.
3.
Friedrich, M., Boggasch, M., Auslegung eines N ockenwellentilgers mit ABAQUS und TOSCA, 2002 ABAQUS Users’ Conference, Wiesbaden, 23.-24. September 2002.
4.
Haffner, P., “Nichtlineare Strukturoptimierung mit ABAQUS und TOSCA – SHAPE”, 2002 ABAQUS Users’ Conference, Wiesbaden, 23.-24. September 2002.
5.
Meske, R; Sauter, J; Güngör, Z. “Recent improvements in topology and sh ape optimization and the integration into the virtual product development process ”, NAFEMS World Congress 2001, Como, Italy, 24.-28. April 2001.
6.
Meske, R., Sauter, J., Gölzer, P., Binderszewsky, J., “Topologieoptimierung einer Linearf ührung mit TOSCA und ABAQUS”, VDI Konstruktion 9, Springer VDI Verlag, pp. 5254, 2001.
7.
Meske, R.; Sauter, J.; Friedrich, M. “Optimization of Elastomer-Metal Components with TOSCA and ABAQUS” 2nd European Conference on Constitutive Models for Rubber (ECCMR) , Hannover, 10.-12. September 2001
8.
Meske, R.; Mulfinger, F.; Warmuth, O. “Topology and Shape Optimization of Components and Systems with Contact Boundary Conditions ”, NAFEMS Seminar “Modellieren von Baugruppen und Verbindungen f ür FE-Berechnungen” , Wiesbaden, 24.-25. April 2002.
9.
Sauter, J.;Meske, R. “Industrial Applications of Topology and Shape O ptimization with TOSCA and ABAQUS”, 2001 ABAQUS World Users’ Conference, Maastricht, The Netherlands, 29.5 - 1.6.2001.
2003 ABAQUS Users’ Conference
15
