ANSYS: Bending originated by Pipe Internal Pressure 2

[Enr1que]

Dear all,

I am trying to model the bending due to the internal pressure on a curved pipe. When using Elastic Curved Pipe elements (Pipe18) with Elastic Straight Pipe (Pipe16) this effect does not appear... Is there any Real Constant or Keyoption which I should be using? My model is quite complex and not modelling with pipe elements would be a huge effort...
Thank you in advance.

 

[Drej]

Hmmm...

These elements are pretty good at capturing the overall behaviour of a system, even at relatively large strains. However:

1) Are you sure that this effect should occur? Have you tried to compare with a simple shell model to confirm this? Internal pressure on a simple pipe element may probably result in only a uniform expansion of the pipe I would guess (boundary conditions may be the key here). What do your results tell you?

2) Pipe elements are a relatively simple approximation to the real thing - particularly the internal/external pressure loading applied.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[cbrn]

Hi,
yes, in addition please consider that you won't "see" any effect of this kind unless you activate Powergraphics and use "3D visualization of elements" in the Size-And-Shape options. However, remember that any derived result will be an "extrapolation" to the element's "skin" of quantities determined at the axis (the only thing that counts for a 1D-formulation element).

Regards

 

[Enr1que]

Dear Drej,

Thank you very much for your answer. I am pretty sure this effect occurs (simple party blowers work on this principle)

Find attached two small "test bench" models: one with shell elements, the other one with pipe elements:

*****************************************************
/PREP7
/TITLE, PIPE elements
PipeDiameter = 0.02
Thickness = 0.002
ElbowRadius = 0.02
Lenght = 0.1

MP,ex, 1, 210e9
MP,nuxy,1, 0.3
ET,1,pipe18
R, 1,PipeDiameter,Thickness,ElbowRadius
ET,2,pipe16
R,2,PipeDiameter,Thickness
N,1,0,0,0
N,2,ElbowRadius,ElbowRadius,0
N,3,0,ElbowRadius,0
TYPE,1
REAL,1
E,1,2,3
N,4,ElbowRadius,ElbowRadius+Lenght,0
TYPE,2
REAL,2
E,2,4
allsel,all
SFE,all,1,pres,1, 1000000
D,1,all,all
FINISH

/SOLU
solve
FINISH
/POST1
/ESHAPE,1
PLNSOL,u,x

*****************************************************
/PREP7
/TITLE, SHELL elements
Radio = 0.02
D = 0.02
t= 0.0015
k,1,0.1,0,0
k,2,0,0,0
clocal,11,cylin,0,Radio,0
k,3,Radio,0,0
l,2,3
csys,0
k,4,Radio,0.2,0
l,3,4
allsel,all
wprota,,,90
k,101,0,0,Radio
numstr,line,11
circle,2,D/2,1,101
lsel,all
adrag,11,12,13,14,,,1,2
MP,ex, 1, 210e9
MP,nuxy, 1, 0.3
ET,1,shell181
R,1,t
mshkey,1
amesh,all
nsel,s,loc,x,0
d,all,all
allsel,all
sfe,all,1,pres,1,10000
finish
/solu
solve
finish
/post1
/EDGE,1,1,45
plnsol,u,x
*****************************************************

I have tryed to modify some keyoptions on the pipe element model, but didn't get any result, and building the whole model with shells is something that I want (need) to avoid.

Best regards.

 

[cbrn]

Hi,
honestly, when facing the same kind of "real-life" problems, where I work we use the pipe model ONLY to determine reaction forces on foundations, overall deformation effects including thermal expansion, and things like that. The membrane stress determined with PIPE16 is realistic only in case of continuous straight pipe.
For any determination of local effects, we immediately shift to local shell submodels or even to local solid submodels (e.g. bifurcations, etc...).
Please note that you almost never need to model the full pipe system with shells: only where you know local / secondary stresses arise.

Regards

 

[Drej]

I've run the pipe and shell models you gave and confirmed the bending effect you see in the shell model. I also confirmed what you said regarding the pipe model being unable to capture this effect - I did this by generating my own pipe model with a finer mesh and non-linear geometry. Still nothing.

I also checked and compared the reactions between both models and they are miles apart. Therefore, I'm afraid to say that my original fears were correct - the simple pipe elements are just unable to capture this behaviour.

This is an interesting problem, but unfortunately it appears that the only way to capture the correct behaviour is to generate a shell/solid model.

Best of luck.


------------
See faq569-1083 for details on how to make best use of Eng-Tips.com

 

[Enr1que]

Thank you very much for all your answers.

Our conclusion is:
ANSYS Elastic Curved Pipe elements (Pipe18) cannot capture bending originated by the pipe internal pressure.

Best regards.