A 3D Tire/Road Interaction Simulation by a Developed Model (ABAQUS code)

Size: px

Start display at page:

Download "A 3D Tire/Road Interaction Simulation by a Developed Model (ABAQUS code)"

Edmund Fields
6 years ago
Views:

1 A 3D Tire/Road Interaction Simulation by a Developed Model (ABAQUS code) M. Zamzamzadeh 1,*, M. Negarestani th Km Joupar Road, Kerman Tire & Rubber Co. R&D Dep., Kerman, Iran Tel:+98(341) Fax:+98(341) th Km Joupar Road, Kerman Tire & Rubber Co. R&D Dep., Kerman, Iran meh_negarestan@yahoo.com Tel:+98(341) Fax:+98(341) * Corresponding author: mah_zamzamzadeh@yahoo.com Abstract In the case of tire development many types of Finite Element Modeling have been performed to date, but in most of them, tire models were either static or simplified models, but this paper presents a 205/60 R 14 radial tire simulation under different loading conditions using ABAQUS Code.1 st we modeled a 2D axisymmetric model & then a full 2D model was created, Finally we developed a full 3D model that tire model components were included according to the real tire components, our tire model comprised one body ply, two steel belts & two capplies, In axisymmetric model two element groups (CGAX3H,CGAX4H) from ABAQUS were selected to represent our rubbery components which these elements have bilinear hybrid behavior with twist to model incompressible rubber behavior, reinforcement materials in ply, belts & capplies were modeled with rebar in surface elements, SFMGAX1 embedded in continuum elements, it is a generalized two node element with twist that can be used in conjunction with other geometrical parameters to model rebar elements. Different hyperelastic models for rubbery Components as mooney rivlin, Ogden, arruda boyce were compared in our projects and then we chose the best one and brought its results to this paper. The 3D model was generated by revolving the 2D mesh developed from the tire cross section about the tire symmetry axis. One of the major application of creating this model is to evaluate the behavior of the tire when has contact with a road during rolling on it, as we know it is very complicated problem to examine stress/strain status in real situation, so this model will help us a lot in this matter & we can predict footprint stress distribution & optimize tire construction to better performance. In the load steps condition, initially we mounted tire on a standard rim then applied inflation pressure, we simulated steady state analysis as relatively high ground velocity and finally contact it with a rigid surface as a road and evaluate different parameters as footprint Stress distribution, we claimed that our results are very close to the experimental result. KEY WORDS: Tire, finite element modeling, footprint, contact, steady state, rolling tire Introduction The finite element method is a very useful numerical tool in evaluating different effects on components of tire in performance. It can predict different behavior of tire in various conditions. as we know design and production process of a new tire will cost a lot for tire manufacturing. So we should approach in tire simulation with real condition to save money and time. The use of predictive finite element models in tire design and analysis has become widely popular in recent times. This largely due to the introduction of high performance computers in edition to the enhancement in the capabilities of exciting proprietary finite element software, those enabling the efficient use of such tire model in saving the challenging problems of pneumatic tire behavior as an alternative, to experimental tests carried out routinely on prototypes tires, for example by FEA we can predict distribution of internal stress/strain that it is very difficult to measure them experimentally. Moreover these days tire engineers tried to develop more useful models to produce realistic tire simulation with finite element model. we can model tire geometry, boundary conditions, loading conditions and material properties 189

2 of a tire in service conditions Therefore this is reasonable to expect that the use of FEA can lead to better understanding of how tire functions and fails by reveal the critical region. Furthermore FEA can provide very useful information thereby reducing the need for building prototypes tires for new design. So we save cost of extensive trial producing or extensive testing. A lot of finite element models for tire have been worked to evaluate new design and predict the tire performance, also several papers have been published in this way, Rolling tire (Shiraishi et al., 2000), Stress and deformation of tire (Ridha, 1980), transient analysis (Nakajima and Padovan, 1987). With the recent advances in digital computers and software, axisymmetric analysis of tires subjected to inflation pressure and free rotation is computationally inexpensive and represents screening in the design of tire. The current work is a part of an on going development of an integrate tire design and visual testing for purpose of design verification and optimization. Such a numerical tire model would reduce the cost of carrying out routine time consuming tests on tire prototypes. To this end a new tire model is developed and used to simulate the tire reaction with the road in different conditions. Model description with ABAQUS Code In this work, a 205/60 R 14 steel belted radial tire was analyzed using ABAQUS/Standard code 6.4 to obtain footprint solution in different condition with a flat rigid surface, subjected to an inflation pressure and concentrated load on the axle. First we modeled a 2D axisymmetric model then a full 2D model was created. In the first stage of modeling it was tried that the geometry of tire profile and its components be completely the same as reference tire. It comprised one body ply, two steel belts, two cap plies, tread, side wall, layer gum, inner liner, anti abrasion, filler and bead. In our modeling of tire we have two groups of components: 1 st group that is made just by rubber as tread, layer gum, side wall, anti-abrasion, inner liner and the other group that is made by reinforced materials as belts, capplies and layer. The rubber is modeled as an incompressible hyperelastic material. In our FE model for choosing a material model that has the best compatibility with our Compounds, we tried a lot of models, in this way first we obtained Stress/Strain Curve in the lab for all of our compounds, compared it with different hyperelastic models in the ABAQUS then chose the best compatible model which it was arruda boyce, one of the S/S graphs which shows the comparison between our test S/S and Arruda boyce model, is shown in Figure 1. Figure 1: Stress & Strain for different hyper elastic models compare with lab results for tread compound. 190

3 The fiber reinforcement as a linear elastic material a small amount of skew symmetry is presented in a geometry of the tire due to the placement and +/-18º orientation of the reinforcing belts. the 2D axisymmetric model is discretized with CGAX3H and CGAX4H for rubbery elements, the belts, ply & capplies reinforced cords are modeled with rebar in surface elements embedded in continuum SFMGAX was selected from the ABAQUS element library. The 3D model is generated by revolving the axisymmetric model cross section about the rotation symmetry axis. 3D model is used for 3D analysis of mounting tire on the rim and applying the inflation pressure, contact with a rigid road, steady state of rolling tire, braking and traction of tire. Large deformation effects were talent into account by using Finite Element allowing geometry nonlinearity. The road was modeled as flat rigid surface that in the vertical loading of tire analysis no friction was considered between tire and road, but in the other analysis as traction, braking and etc, the real friction between tire and road is mentioned. For wheel modeling only the part of rim which is in contact with the tire was modeled, the inner and outer profile were modeled with axisymmetric rigid surfaces. Two dimensional model The mounting of the tire on the rim is preformed by pushing the rigid standard rim surfaces against the tire bead and inflation pressure of Mpa was then applied to complete the mounting process, stress distribution after mounting on the rim and inflation pressure is shown in Figure 2. Figure 2: Stress Distribution after mounting tire on the rim & applied pressure Three dimensional model For the 3D model, steps were devoted to the analysis of the tire according bellow steps: Mounting tire on the standard rim - Inflate tire to Mpa - Static vertical loading of 560 Kg Finally the last loading case, corresponding to a Steady State Free Rolling of tire at a relatively high ground velocity 110 km/hr. 3D tire model after mounting on the rim & applying inflation pressure was shown in Figure

Figure 3: Full 3D configuration depicts mounting on the rim & inflation pressure It has to be mentioned that there is slight differences between the equilibrium solution

Vertical loading In this step of simulation 560 Kg load was applied vertically on the axes of tire and then tire was contacted with the road, at this step friction was

4 Figure 3: Full 3D configuration depicts mounting on the rim & inflation pressure It has to be mentioned that there is slight differences between the equilibrium solution generated by 2D & 3D models. Vertical loading In this step of simulation 560 Kg load was applied vertically on the axes of tire and then tire was contacted with the road, at this step friction was supposed to be zero, the contact area of tire for 100% standard load according to ETRTO for 205/60 R 14 tire was shown in Figure 4. Figure 4: The footprint stress distribution for 100% load ETRTO The shape of footprint that was measured in the test center of tire for 100% ETRTO load was shown in Figure

5 Figure 5: Reference tire Footprint at 100% load ETRTO measured in the lab. The laboratory measurement for width, length, and area of footprints for original tire, and model were shown in Tables 1 and 2. It was found from the model that in small deformation the maximum stress is in the center of contact, as we increase the load, the footprint area increases and the edges of tread contact with the road and it causes which the maximum of stress comes to the edge, especially shoulder of tire. Table 1: Laboratory and model footprints dimension comparison Load 25% ETRTO 50% ETRTO (SI units) Length Width Area Length Width Area Model Reference tire Table 2: Laboratory and model footprints dimension comparison Load 75% ETRTO 100% ETRTO mm^2 Length width Area Length width Area Model Reference tire Steady state free rolling of tire At this step we modeled tire with a relatively high ground velocity 110 km/hr, the purpose of this analysis is to obtain free rolling equilibrium solution, An equilibrium solution for the rolling tire problem that has zero torque,, applied around the axle is referred to as a free rolling solution. An equilibrium solution with a nonzero torque is referred to as either a traction or a braking solution depending upon the sense of. The objective of these steps is to obtain the straight line steady state rolling solutions. Figure 6 shows Rolling resistance of tire at different spinning velocity ( rad/s). This analysis is useful because it can find free rolling velocity of tire and optimized it for reducing rolling resistance of tire. 193

6 Figure 6: Rolling resistance at different angular velocities Conclusion The scope of this study was to establish the ability to predict behavior of tire for different conditions and provide a model for simplifying the evaluation of tire functions after design or optimization with skipping over expensive and time consuming process of prototype tires production, so 1 st a 205/60 R 14 Steel belted tire was modeled by a Finite Element Model using ABAQUS Code, then different analysis were modeled for that tire as deflection of tire on standard loading, evaluation of braking and traction in different angular velocity. The accuracy of this numerical simulation technology is confirmed by the comparison with the results obtained by experimental tests, Finally a three dimensional loaded tire analysis can be accomplished within a reasonable period of time.it is believed that the three dimensional finite element analysis with such efficiencies can be routinely carried out to meet the design needs of tire engineers. At the end It has to be mentioned that we write a program for modeling and analysis of tire in ABAQUS environment, so easily we can repeat all of these steps for every Steel Belted Radial Tire and it is not necessary to model another tires from beginning, just by input some data from the new tire as profile, loaded conditions, etc the model gives its analysis results at short intervals (Zamzamzadeh, 2006). References Nakajima, Y., and Padovan, J Finite element analysis of steady and transiently moving/rolling nonlinear viscoelastic structure--iii. Impact/contact simulations. Computers and Structures 27(2): Ridha, R.A Computation of stresses, strains, and deformations of tires. Rubber Chemistry and Technology 53(4): Shiraishi, M.,Yoshinaga, H., Miyori, A., and Takahashi, E Simulation of Dynamically Rolling Tire. Tire Science and Technology 28(4): Zamzamzadeh, M., and Negarestani, M A 3D Tire/Road Interaction Simulation by a developed Finite Element Model. Tire Society Conference, Sep. 2006, Akron, USA. 194

American Engineering Group 934 Grant Street, Suite #101 Akron, OH Phone : Fax :

ISO 9001:2000 American Engineering Group 934 Grant Street, Suite #101 Akron, OH 44311 Phone : 1-330-375-1975 Fax : 1-330-645-9385 www.engineering-group.com Challenges in the Finite Element Analysis of