Influence of clamping (ANSYS)

[vidiii]

When one clamps an area in the real world it is not perfectly clamped like it is defined in Finite Element Software.

So I tried to test out what the influence of clamping was, in ANSYS. I had an idea to connect every node on the area of the clamping with springs. The springs would have a high K (stiffness). And the other end of the springs would be constrained.

However that seems to be alot of work. I wondered if someone had a better idea. Is it possible to do this automatically in ANSYS.

I would appreciate any advice. Thanks in advance and hope to hear from you.

Kindest regards,
mab

 

[johnhors]

I'll probably get shot to pieces for saying this, but using springs in FE analysis (at least with solids) is a really bad idea. They do not and cannot accurately represent the stiffness of your supporting structure. A high or low stiffness can cause numerical problems with the solver due to ill conditioning of the system stiffness matrix. If you use the same stiffness for all your nodes, then a variable mesh density will just add to the debacle. Another way to think of springs is that they are simple 1D elements with incompatible shape functions to what ever continuum element you are attaching them to (it's never a good thing to attach incompatible elements together). Finally how can you derive a meaningful value for the spring stiffness to be used?

A better way is to model at least a part of your supporting structure, or include it as a super-element (a stiffness matrix derived from a model of the support structure).

 

[cbrn]

Hi,
Johnhors is basically true, but there is at least one method in order to improve implementation of this technique: uniformly-spaced quadrilateral mesh on "elastically-constrained" surface with MESH200 elements, then mesh the volume with the appropriate solid elements (must support pyramidal transition). Then the "constraint" stiffness is uniformly distributed on surface.
This method has to be implemented with caution, of course, but I have plenty of examples where it works very great.

Regards

 

[meshparts]

Another simple way, that work also for variable mesh densities, is to get the number of nodes to connect, then define the stiffness as stiffnes=stiffnes/number_of_nodes.

I would write a small apdl code for this problem.

Regards,
Alex

 

[torpen]

Hello,

Another possible solution is to create a rigid body between the nodes of the area and a master node. A spring with 3 translational and 3 rotational stiffnesses is then linked between the master node of the rigid body and a clamped node.
You have only 6 dofs as parameters but the area moves like a rigid plane (nodes can't move away).
You can replace the rigid body by a rigid plane (nodes can move away on the area which remains plane).

Modelling depends on the physics of your problem and on what you are interested.
Are you interested in stress field?
Is the result near the frontier or not?

Regards,

Torpen

 

[vidiii]

Dear Torpen,

The problem is related to the clamping of a plate for modal and harmonic analysis and what influence it had on the resonance frequencies of the plate and the dynamic tip deflections of that plate.

Kindest regards,

mab