×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

Influence of clamping (ANSYS)

Influence of clamping (ANSYS)

Influence of clamping (ANSYS)

(OP)
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

RE: Influence of clamping (ANSYS)

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).

RE: Influence of clamping (ANSYS)

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

RE: Influence of clamping (ANSYS)

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

RE: Influence of clamping (ANSYS)

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

RE: Influence of clamping (ANSYS)

(OP)
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

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources