ANSYS Hull Strength Analysis Support - Multi-node constraints

[Iain Young]

Hi all,

Currently have a ship hull which I have modelled in SpaceClaim and meshed in mechanical.

In Mechanical, I am trying to constrain all of the nodes at fore and aft ends of the hull (see photo attached) in order to carry out stress/strain analyses.

These nodes will be constrained at midships and at the neutral axis.

However, I am struggling to work out how to do this.

Can anyone give me any help in how to carry out a this multinode constraint?

Thanks in advance.

 

[Ad Hoc]

Welcome to the forum Iain

Those regions you show in red shade, these would be conditions of symmetry.
That means the displacements - at the nodes - will be constrained in the z axis in translation, and then in the x and y axis in rotation.

...These nodes will be constrained at midships and at the neutral axis....

You don't need nodal constraints at the neutral axis!

But with 2 boundary conditions of symmetry, the model will be free to "float" away, as it has insufficient constraints, and as such, your stiffness matrix will be singular. In other words, you'll get endless rigid body motion.
Simple solution, place one node, far away from where you are investigating and add the constraint to ensure the matrix is no longer singular, in this case the y -axis.

 

[Iain Young]

Thank you for the welcome, but more importantly, thanks for the response.

I will attempt to constrain the nodes using the displacement constraint and use your tip for the endless body motion problem.

Could you elaborate on why you don't need to constrain the nodes to the neutral axis?

To confirm: I am doing this to analyse the structural strength of the hull when applying the still water and wave loads (and eventually topside weights) in a similar manner to this paper - JMSE | Free Full-Text | Structural Analysis of a Barge Midship Section Considering the Still Water and Wave Load Effects (mdpi.com)

 

[Ad Hoc]

Hi Iain,

...Could you elaborate on why you don't need to constrain the nodes to the neutral axis?...

Consider a simple I-beam, that is simply supported.
If you apply a UDL...it will deflect bend and experience stress as a result.

If you were to "hold" the part of the web - that is coincident - with the neutral axis, what do you think will happen?
It wont move, it is restrained.

So...if it is restrained, how can the beam bending into the natural curve/shape that is would otherwise do, if unrestrained at the NA?

 

[Iain Young]

Understood.

I've managed to do all the constraint set-up correctly, but as you said, I am getting the endless rigid body motion.

So in terms of adding the constraint in to prevent the endless rigid body motion, how would this be applied on ANSYS?

Is it a Nodal Displacement for the end nodes at each end attached to the 'far away point' constrained in the y-axis?

 

[Ad Hoc]

Hi Iain,

Ok, so I assume you have now set up your FEM like so:

The central; section, is the area under investigation. The extend parts, either side, are "copies" of the central section and simply mirrored.
Thus, you end up with 3 identical sections.

The regions shaded blue, these are the boundary conditions of symmetry, noted above.
This being the displacements - at the nodes - will be constrained in the z axis (longitudinal) in translation, and then in the x (transverse) and y (vertical) axis in rotation.

So, as noted before, that means the FEM is only constrained in translation in the z-axis. But it is contained in rotation in the x, y axis.
However, sometimes, depending upon the accuracy of the model and the type of solver you select and how your loads are applied, adding just 1 more constraint is insufficient - because a force boundary condition may also be insufficient. Therefore you will need to add 2 more constraints in translation.
So the FEM will now be fixed in 3 axis of translation. This will then allow the matrix to be solved as it is no longer singular.

So, how do you do that?...well, you have restrained the model in the z-axis, longitudinal....so, now you need to restrain the model in the y and z axis. But to do so, without influencing the results in the region you are investigating.

At the ends of the mirrored sections, the area you are not worried about, you have the location of the neutral axis - this is perhaps where you misunderstood this concept.
On the centreline of the NA, select one, only one node, at one end and one at the other end, noted by the arrows.

Select one to be restrained in the y axis, and the other in the z axis.
This then gives the FEM 3 nodes that are constrained, and thus, the model, under an applied load will not experience rigid body motion.

So, why is this?
The physical meaning of this, is that the structure, is free to undergo unlimited rigid body motion unless some support constraints are imposed to keep the body or structure in equilibrium under the loads. Hence, some boundary or support conditions must be applied before being solved. Because, If the structure has insufficient constraints to prevent rigid body motion, there are then an infinite number of solutions to the model (equations) that exist; each having the same deformation, but a different location in space.

Hope this makes sense now?

 

[Iain Young]

This makes sense, but I'm honestly struggling with the constraint set-up on ANSYS in order to achieve the model.

Do you use this software? If so, could you share what kind of constraints are needed?

Furthermore, for expanding the model, I'm presuming that I would need to go back into SpaceClaim to mirror both ends, then re-mesh, then apply the constraints and run the simulation?

 

[Ad Hoc]

I us two softwares, one is Ansys, but i haven't used it in years.
Simply because i keep going back to the one I have been using for almost 30years. It is much easier to use, so I have forgotten most Ansys commands/procedures.

For constraints, you go to the constraints tool box, and there are listed a range from Horizontal (applied to a line) to Midpoint (mid point of a line) etc etc.
There is where and how to apply them.

As for mirroring/copying, ive forgotten the 'easiest' way, perhaps this'll help:

 

[Iain Young]

I us two softwares, one is Ansys, but i haven't used it in years.
Simply because i keep going back to the one I have been using for almost 30years. It is much easier to use, so I have forgotten most Ansys commands/procedures.

For constraints, you go to the constraints tool box, and there are listed a range from Horizontal (applied to a line) to Midpoint (mid point of a line) etc etc.
There is where and how to apply them.

As for mirroring/copying, ive forgotten the 'easiest' way, perhaps this'll help:

So I've managed to get the constraints sorted and now my ship model is appropriately behaving - you're advice on the NA constraints was very helpful.

However, as you can see, the stiffeners on the transverse web plates are piercing through the deck plating which shouldn't be happening.

Have you any advice on how to fix this?

 

[Ad Hoc]

Hi Iain,

Looks like several issues going on at once here.

1. Before you run the model, you need to make sure you have "merged" all the nodes.
This means that somewhere within the programme, when you lets say created a panel that has 4 x 4 elements on it, and on the boundary you create a FB that is at right angles to the panel, with the same number of elements, the "intersection" of the FB and panel elements there will be coincident nodes. A duplication if you like. Until you 'merge' the nodes, - make them one node, not two at each space - then the programme treats them as separate entities, not one continuous entity. Thus, you need to ensure that nodes that are in the exact same space - in geometry - are merged to be the same node, no matter which element it is attached to.

Here, these nodes - which are coincident - with the FB and deck plate, must be joined, merged, together. If they are not, this occurs:

2. Looks like in your modelling, you have not aligned the feature i noted above:

The angle bar that is modelled, its base does not appear to be aligned with elements on the shell plate.
So the nodes that are on the angle bar, on this edge, shown by the blue line:

But be coincident (same space) as those on the black line, of the shell plate.
Since there is nothing joining them together.

One final comment, it does look like your aspect ratio of the shell plating on the side is borderline - iffy!!. Looks a tad high to me, which can lead to erroneous results:

The AR should not be greater than 5.

You can also see the misaligned elements again:

The angle bar must line up - to be same joint - as the shell panel element, or vice versa.
So, in this case, the angle bar is independent of the side shell, and so no load will pass through it.

Hope this helps.

FEA is not a simple click click and click, as everyone seems to think. It is a tiger that will either control and consume you, or, you control it.
To control it, you need to learn and understand how the programme works and why it works.

Good luck...

 

[Iain Young]

Hi Iain,

Looks like several issues going on at once here.

1. Before you run the model, you need to make sure you have "merged" all the nodes.
This means that somewhere within the programme, when you lets say created a panel that has 4 x 4 elements on it, and on the boundary you create a FB that is at right angles to the panel, with the same number of elements, the "intersection" of the FB and panel elements there will be coincident nodes. A duplication if you like. Until you 'merge' the nodes, - make them one node, not two at each space - then the programme treats them as separate entities, not one continuous entity. Thus, you need to ensure that nodes that are in the exact same space - in geometry - are merged to be the same node, no matter which element it is attached to.

Here, these nodes - which are coincident - with the FB and deck plate, must be joined, merged, together. If they are not, this occurs:
View attachment 183871

2. Looks like in your modelling, you have not aligned the feature i noted above:
View attachment 183867

The angle bar that is modelled, its base does not appear to be aligned with elements on the shell plate.
So the nodes that are on the angle bar, on this edge, shown by the blue line:
View attachment 183868
But be coincident (same space) as those on the black line, of the shell plate.
Since there is nothing joining them together.

One final comment, it does look like your aspect ratio of the shell plating on the side is borderline - iffy!!. Looks a tad high to me, which can lead to erroneous results:
View attachment 183869

The AR should not be greater than 5.

You can also see the misaligned elements again:
View attachment 183870

The angle bar must line up - to be same joint - as the shell panel element, or vice versa.
So, in this case, the angle bar is independent of the side shell, and so no load will pass through it.

Hope this helps.

FEA is not a simple click click and click, as everyone seems to think. It is a tiger that will either control and consume you, or, you control it.
To control it, you need to learn and understand how the programme works and why it works.

Good luck...

Understood. Thanks once again for your help.

 

[Ad Hoc]

No prob's....good luck.
Any more Qs...fire away.