Constraint definition problem

[dabu76]

i have problem with defining constraint.
I am working on steel panel stiffened with beams (movable deck on ship).
Entire part is defined with shell elements and only force is gravitation. Panel is lying
on four points simulating deck lifter vehicle which moves panel in various positions.
Now, i want to know what deformations and twisting panel is experiencing during lifting on these four points. For that i must have constraint that moving in -z direction (gravitation vector) is prohibited and moving in +z direction is free in constrained point (panel is freely lying on lifter). That is because in practice panel is in some cases deformed in that way that one edge is lifted up.
I think plain rope is example of this constraint. it prevents moving in one direction (away) but opposite direction is free.
How to simulate this type of translation constraint?

 

[nschlueter]

Can you post a picture of the model?

 

[headrush]

Cool. What kind of boat are you building?


While I haven't thought this through like you have, Isuspect you are overthinking the problem. You have gravity (which is never prohibited, except in space) and you have the constraints which represent the support forces. You could uses forces instead of contraints, but unless the forces are perfectly balanced with the gravitational force, you will get rigid body motion and it won't solve.


Don't forget, in situations where there is inherent load balance instability you can use soft springs to stabilize the model(which may or may not be applicable in this case).
Edited by: headrush

 

[Mloew]

Most FE solvers have a special type of element called a Gap. It is a non-linear spring element that essentially allows for different stiffnesses in compression and tension. In this case, the tension stiffness is the spring constant (or curve) of the rope and then zero in compression (can't push on a rope). I'm not sure Mechanica has this type of element in released versions yet.


This can be simulated in linear solvers by eliminating (or modifying the stiffnesses) of the springs that show a compression force. This is an iterative process (though one that can be automated by using Behavioral Modeling) and can be time consuming.


I hope this helps.

 

[KurtStark]

I would define it with contact. There you have the option that the contact may seperate during the analysis.

 

[ghgarzon]

I completely agree with Kurt; you may have to add points on those regions where contact is to take place so as to force the creation of more elements around those contact regions. Be prepared for long time runs.

 

[miya]

Hey dabu76,


A contact analysis might be a little expensive since you are only looking for deformations of the panel.


Also, since you mention it is a "panel stiffened with beams" using shell elements and beam elements, you cannot do a contact analysis: Mechanica only allows contact regions between solid elements.


Since you mention "Panel is lying on four points simulating deck lifter vehicle", this implies the area of constraint is small compared to the overall size of the panel.


Try using point constraints and constraining only in the z direction. You cannot have a constraint which is fixed in the negative direction and free in the positive direction. Your constraint will be fixed in both directions, but since the constraint is applied at a point, you will leave the rotational degrees of freedom "free", so the panel will be able to rotate about the point constraint, which should give you good enough results for overall deformed shape.


Of course the stress results will not be valid in the area of the constraint since you will have a singularity, but as mentioned, the displacement results should be good.


If you only constrain in the z direction, you will also have to take care of the rigid body modes (you will have 3). Either use symmetry if applicable, or use a 3-point-constraint-scheme, to eliminate the rigid body modes.


Hope that helps,
Ray.
---
Ray Miya