Hallo everyone, I have problems with my modal analysis in Abaqus.
Firstly, I will describe my model. The assembly consists of two parts. The first part is sleeve with an inner chamber, which will be pressured with the fluid cavity method. The second is an axle. There is a clearance fit between the two parts. The interaction is modeled with surface to surface method, small sliding with a clearance of 5 um.
Boundary condition: the upper side of the sleeve is fully constrained with the Encastre and the axle is constraint with YSYMM.
Step: the fluid cavity is created at the initial step with a 0 value. Also, the boundary conditions described before is created in this step. Then at the first step it is set to 100 MPa to model the axle being clamped. The next step is the Eigen frequency analysis using lanczos method. The number of modes is specified to 10.
Here comes the problem. When I change the preload in Fluid cavity from 100 MPa to 200 MPa, there is not a single change in the Eigen frequency or the eigenvalue. This should be wrong because the stiffness of the model changes as the preload changes.
Can somebody help me with this problem?
99.99% when this issue comes up, the user does not have non-linear geometry turned on, so the "load stiffness" is not included in the base state for frequency extraction.
Line 24 of your attached file: *Step, name=fd_load, nlgeom=NO
Simply turn on the non-linear geometry to include these effects in the next step.
In addition to what has been usggested above, you also need to remember that stiffness change (stress stiffening) is completely dependent on stress state in the body. Many times marginal change in stress does not affect total stiffness of an object.
- Badges
- Science topic