apply displacement instead of force
apply displacement instead of force
(OP)
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.





RE: apply displacement instead of force
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
RE: apply displacement instead of force
RE: apply displacement instead of force
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
RE: apply displacement instead of force
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.
RE: apply displacement instead of force
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.
RE: apply displacement instead of force
Cheers
Greg Locock
Please see FAQ731-376: Eng-Tips.com Forum Policies for tips on how to make the best use of Eng-Tips.
RE: apply displacement instead of force
RE: apply displacement instead of force
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.
RE: apply displacement instead of force
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.
RE: apply displacement instead of force
What is NASTRAN's GridPointForce balance? Thanks.
RE: apply displacement instead of force
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 ?
RE: apply displacement instead of force
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
RE: apply displacement instead of force
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.
RE: apply displacement instead of force
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.