This example models a tire. The substructure is created after solving a highly nonlinear prestress problem to account for inflating the tire and giving it a footprint due to contact with the road.
To perform the analysis for the tire:
Enter the following commands to extract the input files from the compressed archive files provided with the Abaqus release:
abaqus fetch job=adams_ex3A abaqus fetch job=adams_ex3A_nodes abaqus fetch job=adams_ex3B abaqus fetch job=adams_ex3C
You must perform three Abaqus analyses.
Enter the following command to solve an axisymmetric model for the tire inflation:
abaqus job=adams_ex3A
Enter the following command to create the three-dimensional model of the tire from the axisymmetric model and its results and to calculate the footprint of the tire in contact with the road:
abaqus job=adams_ex3B oldjob=adams_ex3A
Enter the following command to create the substructure model:
abaqus job=adams_ex3C oldjob=adams_ex3B
Enter commands to execute the Abaqus Interface for MSC.ADAMS and to create a modal neutral file for use with ADAMS/Flex.
On UNIX platforms enter the following commands:
setenv MDI_MNFWRITE_OPTIONS negative_roots_OK abaqus adams job=adams_ex3C unsetenv MDI_MNFWRITE_OPTIONS
On Windows platforms enter the following commands:
set MDI_MNFWRITE_OPTIONS=negative_roots_OK abaqus adams job=adams_ex3C set MDI_MNFWRITE_OPTIONS=
This example extends the discussion of the model described in “Symmetric results transfer for a static tire analysis,” Section 3.1.1 of the Abaqus Example Problems Manual. The Abaqus analyses of adams_ex3A and adams_ex3B essentially replicate the inflation and footprint analysis of the tire as described in that section. However, a few modifications have been made to adams_ex3B to prepare it for the substructure analysis that follows:
The rim and hub are modeled as a rigid body, whose reference node is located at the axle. Six degrees of freedom of the reference node will be among the retained degrees of freedom of the substructure.
The footprint analysis is controlled by applying loads and boundary conditions to this reference node.
The *MODEL CHANGE, ACTIVATE option is used in the first step of the analysis. This option does not affect the results of that step but is required so that the road-tire contact pair can be removed before creating the substructure in the Abaqus restart analysis of adams_ex3C.
The third step has output requests for CDISP and CSTRESS to determine the tire nodes in contact with the road at the end of the footprint analysis. A subset of these nodes will be among the retained nodes of the substructure.
The tire model in its original and deformed states is shown in Figure 4–2 and Figure 4–3.
The Abaqus analysis of adams_ex3C restarts from the inflation and footprint analysis of adams_ex3B and consists of the following three steps:
The tire is isolated from the road. The *MODEL CHANGE, REMOVE, TYPE=CONTACT PAIR option is used to remove the rigid surface representing the road. The mechanics of the solution are unchanged, since the *BOUNDARY, FIXED option is used to specify that the nodes in node set FOOTPR have displacements identical to their computed values at the end of the previous step.
One effect of this step is to reformulate the stiffness matrix of the tire without the Lagrange multipliers that were used to enforce the contact constraints; this leads to a more realistic substructure matrix.
This step writes displacements for all nodes to the results file so that deformed nodal coordinates will be written to the results file.
Twenty normal modes of the tire are computed. This step has boundary conditions to restrain all degrees of freedom that will be retained in the substructure, plus additional restraints to maintain the footprint shape.
This step writes element mass matrices for all elements and eigenvectors for all modes to the results file. The eight lowest vibration frequencies computed in this step are shown in Table 4–4.
Table 4–4 Fixed-interface vibration frequencies for the prestressed tire.
| Frequency, Hz |
|---|
| 57 |
| 65 |
| 70 |
| 83 |
| 94 |
| 99 |
| 108 |
| 118 |
Table 4–5 Eigenvalues computed by Abaqus for the unrestrained prestressed tire, using all DOFs of the FEA model.
| Eigenvalue |
|---|
| –3743 |
| –1970 |
| 0 |
| 0 |
| 0 |
| 0 |
| 3.048E+05 |
| 3.208E+05 |
The substructure is created. The list of retained nodal degrees of freedom includes six degrees of freedom at the hub and three degrees of freedom at 35 nodes of the footprint. These contribute 111 degrees of freedom to the substructure. In addition, 20 fixed-interface normal modes are retained, so the substructure mass and stiffness matrices have 131 degrees of freedom. Depending on the engineering use of the substructure, you can choose other retained degrees of freedom. You can experiment with retaining a different number of nodes or possibly only the normal component of displacement at some nodes. In addition, the number of fixed-interface normal modes can be varied.
The *SUBSTRUCTURE MATRIX OUTPUT option uses the optional parameter SLOAD=YES to write the modal load components to the results file. Thus, after translation, the loads corresponding to the fraction of vehicle weight that prestressed the tire will be in the modal neutral file used by ADAMS/Flex.
After reorthogonalizing the component modes computed by Abaqus, the Abaqus Interface for MSC.ADAMS reports the eigenvalues and frequencies of the modes it will store in the modal neutral file. As written to the screen during that translation step, the eigenvalues for the first eight modes are shown in Table 4–6.
Table 4–6 Eigenvalues computed by the Abaqus Interface for MSC.ADAMS for the tire, using component modal synthesis with 20 vibration modes and 111 static modes.
| Eigenvalue |
|---|
| –3741 |
| –1969 |
| 0 |
| 0 |
| 0 |
| 0 |
| 3.139E+05 |
| 3.289E+05 |
The Abaqus input files, adams_ex3B.inp and adams_ex3C.inp, are shown below.
adams_ex3B.inp
*heading tire superelement w/ symmetric results transfer step 0: generate full 3d model using tiretransfer_axi_full step 1: equilibrate results step 2: footprint analysis (displacement control) step 3: footprint analysis (load control) units: kg, m *preprint,model=yes,history=yes *node,nset=road 9999, 0.0, 0.0, -0.02 *symmetric model generation,revolve,element=200,node=200 0.0, 0.0, 0.0, 0.0, 1.0, 0.0 0.0, 0.0, 1.0 90.0, 3 70.0, 3 15.0, 7 10.0, 4 15.0, 7 70.0, 3 90.0, 3 *symmetric results transfer,step=1,inc=4 *elset,elset=foot,gen 1001, 4801, 200 1002, 4802, 200 1003, 4803, 200 1004, 4804, 200 1005, 4805, 200 1007, 4807, 200 1008, 4808, 200 1009, 4809, 200 1010, 4810, 200 1011, 4811, 200 1012, 4812, 200 1014, 4814, 200 *surface,type=cylinder,name=sroad 0., 0.,-0.31657, 1., 0.,-0.31657 0., 1.,-0.31657 start, -0.3, 0. line, 0.3, 0. *rigid body,ref node=9999,analytical surface=sroad *surface,name=stread foot, s3 *contact pair,interaction=srigid stread, sroad *surface interaction,name=srigid *friction 0.0 *elset,elset=sect,generate 2800, 3200, 1 *nset,nset=sect,generate 2800, 3400, 1 *nset,nset=foot,elset=foot *nset,nset=noutp,generate 1055, 5055, 200 *file format,zero increment ************************************************** *step,inc=100,nlgeom=yes 1: inflation *static, long term ** 0.25, 1.0 1.,1.,1. *model change, activate *restart,write,overlay *boundary rim_ref, 1, 6 *dload belt,p5, 200.e3 side,p5, 200.e3 *node print,nset=road,freq=100 u, rf, *el print,freq=0 *node file,nset=foot,freq=100 *output,field,freq=100 *element output s,le *node output,nset=foot u, *contact output, var=preselect *output,history,freq=1 *node output, nset=road u, rf *end step ************************************************** *step,inc=100,nlgeom=yes 2: footprint (displacement controlled) *static, long term 0.2, 1.0 *restart,write,overlay *print,contact=yes *boundary,op=new rim_ref, 1, 6 road, 1, 2 road, 4, 6 road, 3, , 0.02 *node print,nset=road,freq=100 u, rf, *el print,freq=0 *end step ************************************************** *step,inc=100,nlgeom=yes 3: footprint (load controlled) *static, long term 1.0, 1.0 *boundary,op=new rim_ref, 1, 6 road, 1, 2 road, 4, 6 *cload,op=new road, 3, 3300. *contact print cdisp,cstress *end step **************************************************
adams_ex3C.inp
*heading tire superelement w/ symmetric results transfer Restart to identify nodes in footprint step 4: remove contact constraints step 5: extract fixed interface modes step 6: generate superelement units: kg, m *preprint,model=yes,history=yes *restart,read,step=3,write,overlay *elset,elset=eall tread,side,belt ** ************************************************** *nset,nset=footpr,unsorted ** ** This is the list of tire nodes found to be in contact with the ** road at the end of the previous step. ** (These nodes had status CL in the contact print table.) ** 1850, 1855, 1905, 2045, 2050, 2055, 2100, 2105, 2245, 2250, 2255, 2300, 2305, 2440, 2445, 2450, 2455, 2495, 2500, 2505, 2640, 2645, 2650, 2655, 2695, 2700, 2705, 2840, 2845, 2850, 2855, 2895, 2900, 2905, 3040, 3045, 3050, 3055, 3095, 3100, 3105, 3240, 3245, 3250, 3255, 3295, 3300, 3305, 3440, 3445, 3450, 3455, 3495, 3500, 3505, 3640, 3645, 3650, 3655, 3695, 3700, 3705, 3845, 3850, 3855, 3900, 3905, 4045, 4050, 4055, 4100, 4105, 4250, 4255, 4305 ************************************************** *nset,nset=footpr_retnodes ** ** This is the list of nodes in the above footprint that will be ** retained in the substructure. ** 1850, 1855, 1905, 2045, 2100, 2440, 2445, 2450, 2455, 2505, 2500, 2495, 3040, 3045, 3050, 3055, 3105, 3100, 3095, 3640, 3645, 3650, 3655, 3705, 3700, 3695, 4045, 4050, 4105, 4100, 4250, 4255, 4305, 2050, 2105 ** ************************************************** *step,inc=1,nlgeom 4: remove contact constraints *static 1.,1. *boundary,fixed,op=new rim_ref,1,6 footpr,1,3 road,1,6 *model change, type=contact pair, remove stread, sroad ** ** Write displacements for all nodes to the results file. ** (Needed so the MNF contains deformed nodal coordinates) *node file U, *end step ** ************************************************** *step 5: extract fixed interface modes *frequency, eigensolver=lanczos 20, ** *boundary,op=new road, 1, 6 rim_ref,1,6 footpr,1,3 ** ** Write element mass matrices to the results file. *element matrix output, mass=yes, elset=eall ** ** Write eigenvectors to the results file. *node file U, *end step ** ************************************************** *step 6: generate superelement *substructure generate, type=z101, overwrite, recovery matrix=yes, mass matrix=yes ** *boundary,op=new road, 1, 6 *retained nodal dofs, sorted=no rim_ref,1,6 footpr_retnodes,1,3 *select eigenmodes, generate 1,20,1 *substructure matrix output, stiffness=yes, mass=yes, sload=yes, recovery matrix=yes *end step ** **************************************************
