Symmetrical Boundary Conditions on a pressure vessel
Hello there,
I am currently setting up a model of a composite pressure vessel which is build up via a filament winding process. Because of how the pressure vessel is build there is a hole in the dome regions. At one side I do constrain every node around the whole completly in all DOFs (123456). At the other side I am trying to set up appropriate symmetrical boundary conditions, similar to some papers regarding pressure vessels. 
The vessel is perfectly symmetric regarding the xz and the yz plane, my research shows that i need to constrain the perpendicular direction to the xz (or yz) plane and the rotiational DOF parallel to each plane, which I just did as the picture above shows. The vessel is pressurized with a pressure of 200 MPa.
My results visualized via HyperView are not what I expect and I assume that is because my boundary condtions are not correct. The results I expect should show me that the stress maximum is reached in the cylindrical part of my pressure vessel. If I do constrain every DOF at the top end of my vessel I do get that results (but this is mechanical definitly not correct because my vessel is not constrained that way).
I assume i need to somehow constrain every node along its symmetrie plane, but I do not know how I can achieve that with HyperMesh.
Do you guys have any idea how I can change my boundary conditions to be reasonable?
Thanks alot for your advice
Best regards
cluue
Answers
-
In your current modelisation the vessel is not closed, right?
Show us the real structure of vessel. The goal is determining the good simulation model which better prensents the reality.
0 -
I don't understand the boundary conditions you're trying to apply to the vessel other than they should be symmetrical, but this may be a good use of cylindrical coordinate system. I'm assuming it's Optistruct.
Take a look here and see if this works:
https://2020.help.altair.com/2020/hwsolvers/os/topics/solvers/os/cord1c_bulk_r.htmYou can create the system from the Analysis Panel ->systems, then change the type to cylindrical. Make sure to assign the nodes to that new system.
0 -
Q.Nguyen-Dai said:
In your current modelisation the vessel is not closed, right?
Show us the real structure of vessel. The goal is determining the good simulation model which better prensents the reality.
Yes thats right, my vessel is not closed, neither at the top or bottom end.
Here is the real structure of my vessel. All I got is that generic vessel. The domes are perfectly spherical.
0 -
Nick Z said:
I don't understand the boundary conditions you're trying to apply to the vessel other than they should be symmetrical, but this may be a good use of cylindrical coordinate system. I'm assuming it's Optistruct.
Take a look here and see if this works:
https://2020.help.altair.com/2020/hwsolvers/os/topics/solvers/os/cord1c_bulk_r.htmYou can create the system from the Analysis Panel ->systems, then change the type to cylindrical. Make sure to assign the nodes to that new system.
It is actually Abaqus not Optistruct.
So what you are saying is that I should apply all my nodes to a cylindrical coordinate system (respectively make a cylindrical coordinate system my part global system)? If I do so what DOF should I constrain?
0 -
cluue said:
Yes thats right, my vessel is not closed, neither at the top or bottom end.
Here is the real structure of my vessel. All I got is that generic vessel. The domes are perfectly spherical.
In reality, the structure should be closed to support the pressure.
Why you compute the open vessel?
0 -
cluue said:
It is actually Abaqus not Optistruct.
So what you are saying is that I should apply all my nodes to a cylindrical coordinate system (respectively make a cylindrical coordinate system my part global system)? If I do so what DOF should I constrain?
Your model is unrealistic, because of open vessel. So you can not compare the results with theorical results. It not DOF to do, but the modelization should be changed.
0 -
Q.Nguyen-Dai said:
In reality, the structure should be closed to support the pressure.
Why you compute the open vessel?
At my university there was a thesis where they did it this way, because there is no material wound up at that region of the vessel during the manufacturing process.
Also during my research I found papers like this one:
where he is using the boundaries I tried to describe in figure 7 c - but he is getting different results
0 -
cluue said:
At my university there was a thesis where they did it this way, because there is no material wound up at that region of the vessel during the manufacturing process.
Also during my research I found papers like this one:
where he is using the boundaries I tried to describe in figure 7 c - but he is getting different results
Yes, I agree that the vessel is open during the manufacturing process. But how to apply the pressure?
Do you have any special equipment at ends of vessel to close it and apply pressure?
0 -
If you want to do with "open" vessel, here's to try:
- Create a cylindrical syst at end, with Z = Z_global
- Fix DOF 2, 4 & 6 for nodes of ending edge. These nodes should be linked to cylindrical syst.
1 -
Here're the results with SAMCEF solver:
Displacements radial
Displacements Circum
Displacements axial:
VM equivalent stress:
HTH,
1 -
Q.Nguyen-Dai said:
If you want to do with "open" vessel, here's to try:
- Create a cylindrical syst at end, with Z = Z_global
- Fix DOF 2, 4 & 6 for nodes of ending edge. These nodes should be linked to cylindrical syst.
So just to make sure I am doing it the correct way
"These nodes should be linked to cylindrical syst" means I am assigning those to my cylindrical coordinate syst, right?
As soon as i have done that all my boundary conditions I apply afterwards refer to that assigned system correct?
0 -
cluue said:
So just to make sure I am doing it the correct way
"These nodes should be linked to cylindrical syst" means I am assigning those to my cylindrical coordinate syst, right?
As soon as i have done that all my boundary conditions I apply afterwards refer to that assigned system correct?
I don't know how to do that with your FEM solver.
I used Samcef solver, I have to assign the cylindrical syst to this set of nodes. Once assigned, the 1st DoF of node is radial, 2nd is circum,.... That mean that all BC & Loads applied to these nodes within local syst, not global.
Good luck!
0 -
cluue said:
So just to make sure I am doing it the correct way
"These nodes should be linked to cylindrical syst" means I am assigning those to my cylindrical coordinate syst, right?
As soon as i have done that all my boundary conditions I apply afterwards refer to that assigned system correct?
To try: Analysis => systems => assign
1 -
Q.Nguyen-Dai said:
To try: Analysis => systems => assign
yeah i did it that way so that should work if I create my input file I can find codelines which set those nodes to my coordinate system. Im still not getting a symmetrical result which I am still wondering about.
I tried to plot the displacements radial just as you did in your picture below. Doesnt seem to make a lot of sense that the displacement is zero in radial at those blue areas even tho i didnt constrain the radial direction.0 -
cluue said:
yeah i did it that way so that should work if I create my input file I can find codelines which set those nodes to my coordinate system. Im still not getting a symmetrical result which I am still wondering about.
I tried to plot the displacements radial just as you did in your picture below. Doesnt seem to make a lot of sense that the displacement is zero in radial at those blue areas even tho i didnt constrain the radial direction.Please check BC at this node where radial displacement is null.
Check in Hypermesh and in FEM input file.
0 -
Q.Nguyen-Dai said:
Here're the results with SAMCEF solver:
Displacements radial
Displacements Circum
Displacements axial:
VM equivalent stress:
HTH,
Well that works pretty good, atleast I do get the same results as you do know. But I have another issue and I kinda feel like you maybe got the expertise to help me out. I am applying gravity to my vessel, and I need to behave it kinda like a beam (which is constrained at one end) under pressure. But well because i restrained the circumferential direction in my local coordinate system it behaves like i have a support on both ends. Do you think I can model it with the use of a distributed coupling at my not constrained end?
Best regards and thanks alot for your help
0
Altair Employee