Fluid Cavity - Enclosed Surface
Fluid Cavity - Enclosed Surface
(OP)
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
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





RE: Fluid Cavity - Enclosed Surface
RE: Fluid Cavity - Enclosed Surface
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!
RE: Fluid Cavity - Enclosed Surface
RE: Fluid Cavity - Enclosed Surface
RE: Fluid Cavity - Enclosed Surface
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...
RE: Fluid Cavity - Enclosed Surface
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.
RE: Fluid Cavity - Enclosed Surface
RE: Fluid Cavity - Enclosed Surface
RE: Fluid Cavity - Enclosed Surface
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>
RE: Fluid Cavity - Enclosed Surface
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!
RE: Fluid Cavity - Enclosed Surface
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.
RE: Fluid Cavity - Enclosed Surface
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.