proceeding of fifteenth abaqus user group2000p02_W

1、SUSPENSION SYSTEM LOADS TRANSMISSIBILITY USING MULTIBODY DYNAMICS MODELLINGN. MantikasMSX International, Basildon, EssexABSTRACTMultibody mechanical structures can be composed of interconnected rigid and flexible components forming open or closed-loop systems. ABAQUS Standard version 6.1 offers exte

2、nsive capabilities for modelling complex multibody systems. Vehicle suspensions are typical closed-loop multibody systems with components connected via joints and nonlinear forcing elements such as springs, dampers and bushes.The primary scope of the proposed work has been, using ABAQUS Standard 6.1

3、, to derive the time domain forcing response at a vehicles suspension-to-body attachments using real-time input data collected at the wheel knuckles. Accurate representation of the response time histories is important for the prediction of the durability of the vehicle body structure. A front MacPhe

4、rson strut suspension has been modelled in ABAQUS. All components have been modelled as rigid attached to each other with connector elements and bushes.The solution of highly non-linear closed-loop multibody systems, such as suspension systems, is a fairly complex mathematical problem, especially so

5、 for stochastic input forcing. Typically, a set of nonlinear ordinary differential equations coupled with algebraic equations has to be formulated and solved in the time domain. ABAQUS Standard version 6.1 automatically formulates the differential algebraic equations (DAEs) and uses the Hilber-Hughe

6、s-Taylor algorithm, along with an automatic step increment scheme, offering accurate and cost-effective solution.1INTRODUCTIONThe aim of this work is to derive the forces acting on the vehicle body due to road input forces. An accurate description of these forces is essential for stress analysis and

7、 subsequent body durability investigations. The nature of this problem is fairly complex since it involves large angular displacements of articulated closed-loop mechanical systems excited by random input forces.Modelling suspension systems requires software capabilities that can handle closed-loop

8、formations and nonlinear force elements such as bushes, spring and dashpot elements. The large angular displacement assumption requires nonlinear descriptions of the system dynamics resulting in nonlinear sets of ordinary differential equations of motion coupled by algebraic equations, representing

9、the joints of the system.ABAQUS Standard 6.1 can easily handle closed-loop multibody systems and nonlinear forcing elements. Joints between rigid or flexible bodies can be modelled using connector elements. A large number of connector elements included in the software library allow the analyst to mo

10、del any joint configuration needed. Moreover connector element descriptions can be used to monitor2001 ABAQUS UK Users Group Conference1relative or absolute displacements, velocities and accelerations of coordinate systems. Force elements can have linear or nonlinear properties and can be incorporat

11、ed in the model in a straightforward manner.In the solution phase ABAQUS formulates the differential algebraic system of the equations of motion, which is integrated using the Hilber-Hughes-Taylor algorithm. This is an implicit algorithm and it has been shown to be unconditionally stable for at leas

12、t linear system formulations. Additionally, ABAQUS uses an automatic step increment based on Hibbitt and Karlsson algorithm. Adaptive step incrementation is particularly useful for complex nonlinear problems, especially so with inputs that are of random nature. Artificial damping is introduced to re

13、move numerical instability.Outputs can be animated, plotted and mathematically processed in ABAQUS Viewer.2MODELLINGA front MacPherson strut suspension system has been used in this work. The locations of the joints and bushes, along with the meshed suspension components - control arm, knuckle, MacPh

14、erson strut, anti-roll bar and link, and steering rod were supplied by chassis engineering. Force element properties for the bushes, springs and dampers are known. The suspension configuration is illustrated in Figure 1.ABAQUS Standard 6.1 has the ability to incorporate directly the finite element d

15、iscretised components in the analysis. Each component finite element model is declared rigid and a body reference frame is attached to it. The body frame rotates and translates with the rigid body and its initial location is arbitrary in space. All the nodal degrees of freedom of the rigid body are

16、dependent on the motion of the body reference frame. It is therefore expected that forces can be applied in any nodal degree of freedom, whereas external boundary conditions only to the body reference frame degrees of freedom.Incorporating the finite element discretised components directly into the

17、analysis is practical since in some occasions the rotary inertia of components may not be readily available. In other instances the rotary inertia matrix may be supplied in a rotated reference frame along with a parametric description of the reference frame orientation and may need additional treatm

18、ent before it can be used in the analysis. Additionally, animation of the simulation is facilitated using a finite element discretised model.In this work all simulation analysis has initially been performed using discretised models. Adjustments on the mass and inertia properties of components have b

19、een undertaken in a couple of occasions as to allow for the inertia of the brake disc, caliper and hub in the case of the knuckle assembly, and similarly for the case of the strut to account for internal damping mechanisms. The concentrated mass and rotary inertia of these additional parts has been

20、attached to the respective components.22001 ABAQUS UK Users Group Conference1.MacPherson Strut ConfigurationIn the second stage of the modelling the connector elements, spring, damper and bushes were incorporated in the model. Connector elements represent kinematic constraints and can be used to con

21、nect the rigid and flexible bodies that compose the multibody system. Unlike multi-point constraints, connector elements do not eliminate degrees of freedom and kinematic constraints are enforced with Lagrange multipliers. There are a number of benefits in using connector elements in multibody dynam

22、ic analysis. Since connector elements do not eliminate degrees of freedom they can be used to connect rigid bodies at any dependent degree of freedom, unlike multi-point constraints. The connector elements are mathematically presented with algebraic equations, whichcomplement the differential equati

23、ons of the bodies. The resulting Differential Equations (DAEs) are solved simultaneously. The Lagrange multipliers, which2001 ABAQUS UK Users Group ConferenceAlgebraic physically3represent interface forces, are additional solution variables of the dynamic system. Extracting therefore the constraint

24、forces and moments is directly obtained in the solution of the differential algebraic system of equations, not available for multi-point constraints. Moreover, not all interface configurations can be modelled with multi-point constraints. Nevertheless, since multi-point constraints eliminate degrees

25、 of freedom, thus reducing the size of the problem, they should be used when appropriate.Connector elements for the description of any joint configuration are available in ABAQUS element library and their implementation is straightforward. Local reference frames have been assigned to the connector e

26、lements, which rotate and translate with the bodies they attached to. They can therefore also furnish the relative displacement and rotations of adjacent bodies. The local connector element frames can be oriented to align with particular connector element axes.Cylindrical, spherical and fixed joints

27、 have been used in this work. More specifically a fixed joint has been modelled between the knuckle assembly and the strut. Spherical joints have been used to joint the control arm to the knuckle, and the steering rod to the knuckle and steering rack. A cylindrical joint connects the strut to the da

28、mper rod. Spring and dashpot properties have been assigned to the cylindrical joint to represent the spring and damper units of the MacPherson suspension. The elastic and dissipative behaviour of the connector elements can be linear or non- linear and provided by tabular data to ABAQUS.The rest of t

29、he component interfaces are modelled as bushes. These include the upper strut mount to the vehicle body and the control arm to the subframe attachments. Bushes rotate and translate with the reference frame that they are attached to, modelling essential for components performing large angular displac

30、ements. Bushes can have both elastic and dissipative properties and are modelled using spring and dashpot elements oriented in the various directions. The inclusion of linear or non-linear force element properties is straightforward, since their mathematical description is automatically formulated b

31、y ABAQUS.Finite element discretised rigid components connected with connector elements and bushes have been used with success to model the suspension system. Nevertheless, due to the large number of finite elements the computational cost of the exercise is high in the case that the forcing histories

32、 are long. The alternative approach that follows has been implemented with the purpose to reduce computational cost. Fictitious bodies have been used to represent the actual finite element discretised components. These bodies are composed of massless beam elements connecting the components centre of

33、 mass to its hardpoint locations. Each body has been assigned the calculated mass and inertia properties of the corresponding component calculated by ABAQUS in the initial simulation runs. The rotary inertia properties can be obtained in the ABAQUS results files and can be calculated around the cent

34、re of mass of the component in the global reference coordinate system. This is helpful since these values can be directly assigned to the fictitious bodies. Each fictitious body is given a body reference frame at the centre of mass location and declared rigid. Such a modelling approach is shown to b

35、e two orders of magnitude more cost efficient than utilising the full finite element discretised rigid components.ABAQUS Standard 6.1 has the ability to incorporate flexible bodies in the multibody system. This can be done by including directly the flexible component into the nonlinear formulation,

36、thus utilising a non-linear finite element approach. Alternatively, the analyst can use a super-element analysis mehtodology. Nevertheless, for the purposes of this work and for reducing the simulation42001 ABAQUS UK Users Group Conferencetime by a considerable amount, the anti-roll bar has been mod

37、elled as an equivalent bush component. In doing so, it has been assumed that the inertia properties of anti-roll bar will have a negligible effect on the response of the overall system compared to its stiffness characteristics. For the calculation of the equivalent stiffness properties, a static ana

38、lysis with anti-roll bar restrained completely at one end and with the subframe bushes attached on it has been performed in ABAQUS.The final stage of the modelling process requires the incorporation of the input forces at the knuckle. Longitudinal, lateral and vertical forces and the corresponding m

39、oments have been included in the analysis. These forces and moments have been modelled in ABAQUS so as to follow the rotation of the local reference system they are applied to. This is real time testing data of a particular event of interest and is measured with the use of load cells. The data has b

40、een processed in nsoft software and provided to ABAQUS in a tabular format. The random forces and moments acting on the knuckle are presented in Figure 2.3SOLUTIONABAQUS offers several methods for performing dynamic analysis of problems in which inertia effects are important. Direct integration of t

41、he system is used when non-linear dynamic response is investigated. Large angular displacement of the articulated components in a multibody system causes non-linear response. Moreover, in rare cases, non-linearities can be introduced due to large deflection in flexible articulated components or non-

42、linear material properties.The equations of motion for closed-loop constrained mechanical systems are typically presented in the form of second order Differential and Algebraic Equations (DAEs). They exhibit particular characteristics which make their numerical treatment difficult, and distinguish t

43、hem from the solution of systems of explicit differential Equations (ODEs).ABAQUS Standard uses Hilber-Hughes-Taylor algorithm for the direct integration of the equations of motion. The main advantage of the particular operator is that it is unconditionably stable for linear systems, i.e. there is n

44、ot mathematical limit on the size of the time increment that can be used to integrate a linear system. Although it would be difficult to generalise this finding for non-linear systems, it is generally true that linear stability is an indication of an operators good properties for integrating non-lin

45、ear systems.The Hilber-Hughes-Taylor operator is implicit; the integration operator matrix must be inverted, and a set of dynamic equilibrium equations need to be solved at each time step. The solution of the dynamic equations of equilibrium is performed in an iterative process using Netwons method.

46、 This operation is computationally expensive especially so for highly non-linear systems. Nevertheless, as it has been noted above, the Hilber-Hughes-Taylor algorithm exhibits good properties and the step of integration can typically be large, one or two orders of magnitude larger than time steps as

47、sumed by explicit schemes.Moreover, in ABAQUS/Standard the time step for implicit integration may be chosen automatically on the basis of the half step residual, first introduced by Hibbitt and Karlsson. The half step residual is the equilibrium residual error halfway through a time increment. If th

48、e highest out of balance force (residual error) is small relative to the typical time-averaged force value of the problem, then the accuracy of the solution is assumed to be high and the time step can safely be2001 ABAQUS UK Users Group Conference5increased. In the opposite case the time increment i

49、s automatically decreased. The adaptive time incrementation scheme provided by ABAQUS has a number of advantages relative to fixed time step procedures. Briefly, the problems directly associated with a fixed time step would be the following: If the time step is too large, the error in the computed r

50、esponse will be large, masking important aspects of the response. A large time step would also increase the degree of non-linearity of the algebraic system, with consequent increase in the number of iterations per time step, or creating divergence problems in the Netwon algorithm. If the selected ti

51、me step is too small, the cost for obtaining a solution could be raised to unacceptable levels.In general flexibility in multibody systems generates higher frequency modes in the resulting numerical system which generally play a secondary role in the response, but which are responsible for numerical

52、 instability if not filtered in the proper way. Additionally, slight high frequency numerical noise is introduced when the time step is altered during the analysis. For these purposes artificial damping is incorporated in the Hilber-Hughes-Taylor algorithm to remove numerical instabilities. It has b

53、een demonstrated that Hilber-Hughes-Taylor operator numerical damping can be introduced without degrading the order of the accuracy. Artificial damping can take values 1/3a 0.The numerical damping used in this work is a=0.15, and was shown, using energy balance monitoring, that it caused only minima

54、l artificial energy dissipation. The half step residual tolerance value has been chosen in the region of 10 times the typical magnitude of real forces in the system. This is a justified choice since it offers a highly accurate solution for systems with high energy dissipation mechanisms, keeping at

55、the same time the computational cost low.4RESULTSForces and moments at the control arm bushes and the strut-top mount have been obtained in all directions. The output forcing histories were plotted in ABAQUS Viewer, the post-processing module of ABAQUS/CAE, and are shown in figures 3,4 and 5.For val

56、idation purposes two forcing cases are compared to results obtained by an established commercial multibody dynamics code. The two cases of interest were the forces transmitted to the control arm bush at the X direction and top strut mount at the Z direction, presented in Figure 6. In qualitative ter

57、ms there is an excellent agreement between ABAQUS and the baseline results. In quantitative terms there are discrepancies which can be contributed mainly to small differences in the component inertia properties between the models, the MacPherson spring pre-load values, and the anti-roll bar modellin

58、g. In addition the spikes appearing in the baseline results are due to spikes in the input data; these have been removed in the ABAQUS simulation. Moreover, different numerical solvers may furnish slightly different results, especially so in a highly nonlinear simulation.62001 ABAQUS UK Users Group

59、ConferenceThe CPU time required to simulate 70 second history was approximately 3403 seconds on an ORIGIN 3400. In order to achieve as low CPU time as this, and without sacrificing accuracy of results, the half step residual was kept fairly low and the minimum, maximum and initial time steps were adjusted to the p