apply displacement instead of force

[johnsmith2]

In my model, when I apply the force/pressure, model becomes unstable. I know applied displacement controlled can solve this problem. However, how do I know the value of displacement should I apply. Can I check the reaction force to ensure the displacement that I apply being the same the force/pressure that I should apply? Thanks for ideas.

 

[meshparts]

Hello,

In some cases one can define a spring k with one node on the node where you want to apply the force F. On the other node one can define a displacement u1 such that:

F=k*(u1-u2)

where u2 is the displacement of the force applying node.

This works like a proportional gain.

Regards,
Alex

 

[rb1957]

personally, i'd be worried about a model that "becomes unstable" ... i'd investigate this before trying a work-around; and i don't really understand why a model would be "unstable" with applied forces but "stable" with enforced displacements.

 

[gurmeet2003]

rb1957,

A model may undergo rigid body motion if enough constraints
are not present and a Force load is applied leading to very large displacements. I think this is the unstability discussed in this thread. On the other hand displacement is self limiting by nature.

But I agree with your comment that one should try to investigate and remove the cause of unstablity rather than doing a work around. One could add soft springs to take care of this problem. Or one could add suitable constraints to remove rigid body motion.

Gurmeet

 

[prost]

My experience the model is unstable for a couple of reasons: poor constraint definition (that is, not enough to constrain the rigid body modes) and nonlinear instability caused by too large of a load (this could be a buckling instability if you are running a buckling problem, or a large mesh distortion problem caused by a very big load being applied to a nonlinear material, which causes the material, that is, the mesh, to distort badly). It is difficult to say why you are experiencing these problems without knowing more--I suspect a contraint problem.

If the problem is linear (linear elasticity, that is), it is almost trivial to find the force for a given displacement. Since the problem is linear, input a displacement of 1.0 (unit displacement), calculate the reaction forces, F. Desired reaction force is "R". therefore "R/F" is the desired displacement.

 

[johnsmith2]

thanks for all reply. My problem becomes unstable because of too much force applied. I found that when I try to apply the displacement, instead of force/pressure and keep everything the same (mesh). It can converge. That's why I want displacement-controlled.

For prost,
my material behavior is linear, but I turn on the nonlinear displacement calculation (NIGEO) in abaqus. So, I am not sure the relationship is still linear when enough force is applied.

 

[GregLocock]

Is this a contacts type problem?

Cheers

Greg Locock

Please see FAQ731-376 for tips on how to make the best use of Eng-Tips.

 

[rb1957]

does your code allow you do the equivalant of NASTRAN's GridPointForce balance ?

 

[prost]

As you seeing, there are many different types of nonlinearity; nonlinear material constitutive relationships, nonlinear deformations (such as a end load on a beam causing the beam to wrap around itself), nonlinear kinematics (that is, multi body contact). Each can cause instabilities in the FE solution process. Can you tell me what material you are using--that is, what are using to define the material in the material properties window?

Is there instability problem there when you apply say 100th the force? If not, your analyses appears to be correct, that the force is too large. However, if the force is an input, that is, you have to load this thing with a large force, you might be able with very small load steps to keep the model stable, or in the case of applied displacements, very small displacement increments. Since the problem is nonlinear, you'll have to play around with the inputs until the displacement you input causes the force you need.

I would think all commercial FEA codes have the capability to compute reaction forces someplace in the Results window. Check the FEA help, that might have your answer.

Is it me or is eng-tips squirrely today? 6/20/2007. I am having lots of problems with access.

 

[johnsmith2]

thanks again.

My material is a linear one with stainless steel. It is not a contact roblem. I should be able to check the reaction force in ABAQUS at the displacement that I applied.

prost,
What do you mean by 100th the force? I applied the force in single step. It becomes unstable in the middle of the increment of loading. That's why I think the force is too force for the model. I would rather to apply the displacement controlled.

 

[johnsmith2]

rb1957,

What is NASTRAN's GridPointForce balance? Thanks.

 

[rb1957]

GPF tells you at a node what force each element is reacting.

if this isn't a contact problem, and is linear, i still have doubts as to why an enforceed displacement will work, but an applied force won't. Further, if you've tried a very small force and the model is unstable, it sounds to me like there are issues with either the model or the structure.

give us some more clues, what type of structure is this ? do you think it's a buckling problem ? (would you clue detect this ? ... try running a column to see what happens if you overload it) are you shell elements plates (capable of reacting bending) or membranes ? ditto for you endload elements ?

 

[krishp]

Johnsmith,

first time when you requested for a suggestion also consists the answer, which is a simple approach. Here people seems to be experts and making this a bit complicated, I would say confusing..so just find the "R" value for a X displacement...and thats it..

cheers..
dRiNk TeA

 

[prost]

There are two reasons I suggest applying 100th the force you really want

1) Depending on the numerical algorithm used to solve the FEA, of course, but sometimes a very large force 'F' that causes instabilican be applied over a number of load 'steps' in much smaller increments, say 100 steps, so that each load step is F/100 larger than the previous--ramp up the full force 'F' in 100 equal, increasing steps.
2) If your see an instability at 100th of the force you really want, I still suggest something is wrong with the boundary conditions you have specified.

 

[jmagri]

If the model becomes "unstable" with force application but not with displacement you may need to consider how the model is constrained. A displacement is a constraint on motion. Force application makes imposes no constraint on the possible degrees of freedom of the model.

Also, I like to use pressures instead of forces to avoid having the problem of having a force applied to a very small area (node). This can result in degrees of freedom that the element is not designed to consider.