Discussion Groups

## Simulation Mechanical and Multiphysics

Contributor
Posts: 11
Registered: ‎04-10-2012

# On Nodal Displacement Boundary

776 Views, 7 Replies
07-06-2012 09:47 AM

Hello, guys

This problem has been giving me a had time.  I want to put displacements on several nodes of my model.  Acturally, I can do this in "Static stress with nonlinear material models".  Well, here comes the problem.  In "Static stress with linear material models", there is an option of "Node displacement boundary E..." when I right click an node and select add.  In the dialog of the "Node displacement boundary E..." , besides the displacement type and magnitude, I am asked to input a "stiffness", which makes no sense to me.  How comes the stiffness is needed when we just want to put a displacement on nodes?  What the exact meaning of a stiffness for displacement?

Anyway, I input an arbitrary number, say 10000, in that, and tried to run the analysis.  In the results, that node stays at its original location rather than moves to the location expected.

So what is wrong with this Nodal Displacement Boundary?

I will really appreciate if you have the same experience and would like to share your thoughts?

Thank you.

Contributor
Posts: 18
Registered: ‎07-05-2012

# Re: On Nodal Displacement Boundary

07-06-2012 10:07 AM in reply to: Lonelytown

The node displacement is enforced through a spring linked to another (auxiliary) node, you can think of it as ground, which moves by the prescribed amount.  The greater the stiffness that you need to input in the dialogue, the closer the displacement of the node to which you applied this device is to the motion of the ground.  For zero stiffness the displacement would not be enforced at all.  For infinite stiffness it would be enforced "exactly".

Contributor
Posts: 11
Registered: ‎04-10-2012

# Re: On Nodal Displacement Boundary

07-06-2012 11:29 AM in reply to: Petr.Krysl

Thank you for response.  I can understand the philosophy of this stiffness with your explaination.  But how come I still cannot get the displacement enven after assigned a rather large number in it?

Contributor
Posts: 11
Registered: ‎04-10-2012

# Re: On Nodal Displacement Boundary

07-06-2012 12:27 PM in reply to: Lonelytown

100000000 lb/ft is the number I input.

Member
Posts: 4
Registered: ‎01-24-2012

# Re: On Nodal Displacement Boundary

07-06-2012 12:38 PM in reply to: Lonelytown

Try something much bigger like 1e12, needs to be several orders of magnitude larger than the material stiffness.

Contributor
Posts: 11
Registered: ‎04-10-2012

# Re: On Nodal Displacement Boundary

07-06-2012 12:44 PM in reply to: algor_neil

Thanks. But not working.

Employee
Posts: 492
Registered: ‎03-25-2010

# Re: On Nodal Displacement Boundary

07-06-2012 12:56 PM in reply to: Lonelytown

Just about all loads in linear stress can be adjusted from one load case to another, and prescribe displacements (displaced boundary elements prior to version 2012) is one of those. My guess is that you did not do the following (from the documentation)

• For prescribed displacements to be used in the analysis, you must specify a Multiplier in the Displacement column of the Multipliers tab in the Analysis Parameters dialog box. The value entered is multiplied by the value in the Magnitude field. The product is the displacement applied to the new node of the displacement boundary elements.

P.S. One of the nice things about the wiki documentation is that anyone can add their ideas and explanations. I can see a few improvements myself, so I am going to draft them right now.  :-)

Sincerely,
John Holtz, P.E.
Senior User Experience Designer, Simulation
Autodesk, Inc.

Current version of Mechanical & Multiphysics: 2013 SP1 (2013.01.00.0012 28-Jun-2012)