Consider an elastic structure fixed to a base by means of bolts. How can the natural frequencies of this structure be predicted using ANSYS? How can the contact interaction be taken into account? Any ideas or comments are appreciated.
The problem at the first approximation can be solved as just fixing the nodes at the position of bolt connection (fully fixed connection or so-called tying contact). In this case the modal analysis is straightforward.
The next approximation step is highly depends on your needs.
It can be the modal analysis after the perfoming the full contact analysis (after solution of the contact problem). In this case it is necessary to keep in ANSYS the updated tangent matrix ( keeping PSTRES, ON)
The problem at the first approximation can be solved as just fixing the nodes at the position of bolt connection (fully fixed connection or so-called tying contact). In this case the modal analysis is straightforward.
The next approximation step is highly depends on your needs.
It can be the modal analysis after the perfoming the full contact analysis (after solution of the contact problem). In this case it is necessary to keep in ANSYS the updated tangent matrix ( keeping PSTRES, ON)
Dear Alexander,
Thank you very much for your response. The first approximation you mentioned is the first thing that comes to one’s mind, but the vibration modes don’t appear to be consistent with reality. When the bolted parts are pressed together during motion, this is one situation, but when they go apart, this is another. The standard modal analysis doesn’t see the difference between these two cases.
Can this contact interaction be more or less accurately described by the linear equations, this is the question. I’m afraid, the answer is negative.
The static problem of contact interaction can be solved. We can take the initial stresses into account using the PRESTRESS option, but in this case we have to bond nodes on the contact interface, which is not correct. As far as I know, the contact elements are not supported in the modal analysis. Or do I misunderstand something?
Dear Stanislav, as far as I know, the natural frequency and normal modes concepts imply that the system is linear, then contact can not play a role.
Thank you for response.
The modal analysis deals with linear equations of the form Kx-w2Mx=0. We can only adjust the stiffness matrix K taking into account the initial stresses that occur owing to bolt pretension. The problem is to describe the boundary conditions at the interface of the parts in contact. These conditions are of nonlinear type.
In MIT, they succeeded in solving the problem. Some results are given at
http://www.adina.com/newsgH-31.shtml. But details are not discussed.
Use Spring element like Combin14 in place of a bolt. Try different stiffness values of spring constant and see if you get closer to reality.
Stanislav, probably ADINA is taking the tangent stiffness matrix to build the eingensystem. But in any way this implies that if the contact is intermittent you can use this modes to understand the response... As far as I know,an intermittent contact problem has generally a non-harmonic response.
Since the matrices in modal analysis shouldnot depend on the solution itself (i.e. the system is linear) another way to go around finding the natural frequencies of a nonlinear system is using nonlinear dynamics and then apply fast fourier transform to convert the behavior into frequency domain. For a numerical simulation, if you conduct in ansys transient harmonic sweep analysis and pick up some "representative" dof and converted its time response to frequency response (by FFT) then you might get peaks for the natural frequencies. obviously this results depends highly on the dof you pick.
- Badges
- Science topic
- Similar topics
- Engineering
- Materials Engineering