Fluid Cavity - Enclosed Surface 1

[lucasmec]

Hello,

I'm using ABAQUS 6.13 for a fluid cavity in Explicit using and axisymmetric model.

It's like a cylinder, so in the Axisymmetric I only define 1 part with half the top, side and half the bot:
Like this:
|
|---------
| |
| |
| Water |
| |
| |
| |
|---------
|
The problem is when I define the surface for the fluid cavity, I only choose the three sides from the cylinder and I dont pick the side from the axisymmetric line... and then ABAQUS says that the surface for the fluid cavity is not enclosed and that the most left elements from the top and bottom have free edges. So it basically doesn't calculate the volume and the cavity is empty.

I already checked the normals and did everything... I searched in old input files and even an old one from Abaqus tutorials (air spring) is making this mistake. Btw, do I need to change the inp file to create fluid elements (in this case FAX2)?

Thank you very much,
Lucas

 

[cooken]

I also find the documentation on fluid cavities a bit odd. Are you sure your analysis is not working as intended? Did you let the analysis run and request CVOL for the reference node to check what the calculated volume was, or is it an assumption based on the warnings and documentation? Reason I ask is that I have been running a 3D model of concentric pipes using a fluid cavity in explicit. My cavity is open at both ends (although I do have plane symmetry BCs), and I get the "not enclosed" warnings, but the actual volume calculated and overall behaviour of the model is as expected.

 

[lucasmec]

You are right! It calculates the volume... but it's not working yet.

Explaining a little bit better, the cylinder has got a pressure applied in the bottom and it can move verticaly. So I want Abaqus/Explicit to understand there is a mass inside and calculate the stress in the cylinder walls for a short period of time. Should I use Hydraulic or Pneumatic? Can I use Hydraulic with Explicit? Ahhhhh!! It keeps saying that I don't have the properties assigned to the hydraulic elements that I generated in the ineer walls (using a skin). I am wasting so much time on this

Help please please!

 

[cooken]

Take your time and work through the messages one at a time. Are you working directly with an inp file or generating it with CAE? I assume the latter since you mention a skin. What elements are you using for the skin, surface membrane? Have you given a density (explicit requires this)? If you upload your inp I can take a look.

 

[lucasmec]

I'm working with python and CAE, but was trying to change the fluid element in the inp file that the programe generates automaticaly...

 

[cooken]

Based on the input file, you created membrane elements that shared nodes with the the solid ones, but the cavity was associated with the solid element surface and not the membrane. The error that I got, though, was that the membrane elements were missing a property (you gave a density but didn't define an elasticity etc..). I don't know if defining the cavity with the membrane elements would be sufficient. I just deleted your membrane elements and it ran without errors. My understanding is that you never actually define fluid elements (FAX2, F2D2 etc..) in an input file, Abaqus does that internally.

Your second big issue is that your boundary conditions are insufficient. There is nothing preventing rigid body motion in the Y-direction, so the whole thing just shuffles along.

Apart from that, you'll want to add the relevant history output variables for the cavity (see below), and I would recommend reducing your output intervals by a couple orders of magnitude, otherwise your odb will just be excessively big. Do you really need to capture what is happening at every 0.000005 seconds?

*Node Output, nset=Set-1
CMASS, CVOL, PCAV


And finally the really curious part - despite seeing a decrease in volume, constant mass in the cavity, the pressure does not change. Not sure why...

 

[cooken]

I changed the cavity reference node from the isolated one defined in the assembly to a node at either the top or bottom of the vessel (node 7 or node 8), and now pressure is being output. Don't know why this works and the isolated one doesn't...

Also, I didn't make it clear above, but in the attached input file I added a boundary condition, and scaled up the applied pressure so be sure to correct those.

 

[cooken]

Oops, I also changed your bulk viscosity.

 

[lucasmec]

Thank you very much! At least now I have some nice variables working fine. In fact, about the BC, I also want to make some simulations where the body is able to move in the y-direction. The only problema now is that the body accelaration in the y-direction only takes into account the mass of the outer material (so it gains too much velocity)... the inertia due to the mass of the water inside is not counting for anything. Maybe there is an option in ABAQUS to enable it. Do you know anything about it?

 

[cooken]

Erm, I can't say I do...I mostly do static or quasi-static analyses so never had to worry about correct inertial forces.

I have used lumped masses before, but not 100% if that would work in this situation, you would need to be real careful about where you placed the node (center of mass) and how you constrain it to the rest of the body. In an input file it looks like this:

*Element, type=MASS
<node number>, <node number>
*MASS
<mass>

 

[AlfredWu]

@cooken
hi cooken
I modeled a fluid cavity in a 2D axisymmetric model, abaqus/standard.
One of the boundary of the fluid cavity is the symmetry axis and the refenrence point is at the symmetric axis too, thus the fluid cavity is not enclosed geometrically.

When I complete the calculation case, it came the following warning messege:

WARNING: "The surface assembly_***** is not completely enclosed. A list of element with free edges on this surface is given as follows:"

but the history output value CVOL (hydrostatic fluid cavity volume) is as expected, which is equel to the whole sphere.

I want to ask that what does the warning message mean and how to remove it.
Thanks very much!

 

[cooken]

Hi Alfred,

Abaqus issues warnings in many situations to flag a potential issue to the analyst. These are like "proceed with caution" messages only and do not necessarily mean there is anything wrong with your model. There is no way to remove the warning as long as you are using an "open" cavity with a symmetry axis or plane, but your results should be unaffected.

 

[AlfredWu]

Hi, cooken
you are right. so I can ignore the warning messege if the results is rational. Thanks very much!
In abaqus 6.13, it doesn't need to edit keywords to create a fluid cavity model, and it seems that the normal direction is automatically defined when pickup the fluid cavity surface and refenrence node to define a fluid cavity interaction in abaqus/CAE.