Hello @Disla
Thank you for sharing this. So just to confirm, you tried both models and both give the same discrepancy from analytical results?
The Neo Hookean model is not awfully off and the formula in the paper is what you are looking into, correct?
I have recently applied some of my learnings on Hyperplastic models to a bouncing ball.
It looks nice, and I have only seen ANSYS references on youtube where the deformation of the ball can be seen so clear with itās first vibrating mode exited.
Just want to share it. Hope you like it.
NOTE: Be careful and use SafeSearch if you look for ābouncing ballsā on Google. 
6 Likes
Mind sharing the input deck?
I currently have the file below, but the case diverges as soon as I use hyper elastic instead of elastic.
The zero concentrated loads are to be replaced by forces from the fluid solver.
Would appreciate any help.
ĀæWhat system of units are you using?
Then your inp units are read as:
**ELASTIC
**300000.0 [Pa], 0.3
*HYPERELASTIC,NEO HOOKE
C10= 0.2449 [Pa], D1= 0.25 [1/Pa] !!!
*DENSITY
1200.0 [Kg/m3]
C10 value is typically something between 0.5-1.0 [MPa] !!!
My ball was:
C10=0.2 [MPa] = 200000 [Pa]
D1=0.002 [1/Mpa] = 2E-09 [1/Pa]
Be careful when searching for constants out there, especially for Ogden. Each commercial software uses different formulation.
Be sure your constants have derived from the same Strain energy potential definition (Abaqus).
The smallest D1 the more incompressible up to the point ccx considers a minimum value to warranty convergence.
Iām very new too hyper-elasticity but there are very interesting applications out there. Iām now trying to reproduce this paper:
A study of balloon type, system constraint and artery constitutive model used in ļ¬nite element simulation of stent deployment .
Alessandro Schiavone
Loughborough University
Liguo Zhao
Loughborough University
Super cool stuff. You can find some Abaqus constants there as reference.
1 Like
For those who might be interested, informative pictures of the 3 typical stent applications can be found here
Stents - What to Expect When Getting a Stent | NHLBI, NIH
2 Likes
100%! You will need to be careful with the constants and read the different manuals to understand the formulations. I believe the 3 major commercial packages (Abaqus, Ansys, and MSC Marc) have different formulations each.
@Disla, you are right. I forgot to convert the constant values to meter based after switching the geometry size. I now have:
C10 = 244898, D1 = 2.5e-7
1 Like
Hello, but here the phrase was taken out of context, āthere is a misprint in the work, and solutions for Mooney-Rivlin rectangular beam are given for H=W=0.2, and the Neo-Hookean beam has dimensions H=W=0.1.ā The misprint referees to the results, not to the definition of the energy function, and only to Mooney-Rivlin material. Please, next time, put the whole text of the message, not only convenient part.
Hi @Disla
Hope you are well
I set up the Calculix case but, this time, with an intention of coupling it with a fluid solver for FSI.
however, seems like there is some error in this case that I am not able to spot.
Would really appreciate if you could take a quick look.
It is a tube with length 0.15m and inner diameter of 0.015m
E = 1.44 MPa and poisson = 0.47
I donāt know how to set up an FSI sorry, but I can see different things in your file.
*HYPERELASTIC,NEO HOOKE
244898, 25e-7
-This do not correspond with E = 1.44 MPa and poisson = 0.47. Double check D1.
-I would make sure my model works under a predictable load condition before coupling an FSI. ĀæWhich range of Cload do you expect?. Have you applied that value to see if your model solves?
-ĀæAre you using the same unit system in both analisys?
-Your model seems constrained only in z direction.mmmh. Rigid body displacements (And rotation!)
-Keep in mind shells expand and the node number will change.
-Why dynamics? .Have you succeeded with a couple of nonlinerstatic?.
Apart from that it seems to works after adding some more constrains.
Hi @Disla
Thank you for taking the time out to look at my case.
You are right; the D1 value is uspposed to be 2.5e-7.
So, I am not sure what the actual CLOAD would be but from the little time that the FSI case ran, I got an average force of about 0.0008 N but close to diverging, it increases to 0.019N then 38N. Should I apply that force in all three directions for the interface nodes to check?
Yes sir. Units are same on both sides (meters)
Yes. I can constraint all three directions to see if that plays out well.
As per the website of preCICE, Configure the CalculiX adapter | preCICE - The Coupling Library, the coupling works for DYNAMIC, FREQUENCY or MODAL DYNAMIC
What load did you apply and what additional constraints did you add?
And what software are you using to run the cases? and post-process? Your videos look nice (much better than CGX)
I have constrained both ends with a kinematic coupling and later frequency analysis to check. There are no loads. Thatās the first mode. I was curious of the frequencies involved in your model.
If I where you (ā¦and I knew how to do it 
) I would start with a rigid clamped pipe. Both problems coupled but āremovingā the possibility of failure of the structural problem. Letās see what pressures or loads you get and if they make any sense.
You will also get an idea of the required time scale. Introduce the complexity slowly.
Iām using ccx on Mecway. Prepomax has a nice GUI too.
*INCLUDE, INPUT=all.msh
*INCLUDE, INPUT=inlet.nam
*INCLUDE, INPUT=outlet.nam
*INCLUDE, INPUT=interface.nam
*MATERIAL, Name=EL
*HYPERELASTIC,NEO HOOKE
244898, 2.5e-7
**0.2449, 0.25
**ELASTIC
** 1440000.0, 0.47
*DENSITY
970.0
*SHELL SECTION, Elset=Eall, Material=EL, OFFSET=-0.5
0.0007
*STEP, NLGEOM
**INC=1000000
*DYNAMIC,DIRECT
0.0001,0.01
*RESTART,WRITE,FREQUENCY=1
*BOUNDARY
Ninlet,1,3,0
Noutlet,1,3,0
*CLOAD
Ninterface,1,0.0008
Ninterface,2,0.0008
Ninterface,3,0.0008
*NODE FILE
U
*EL FILE
S, E
*END STEP
I ran this now. Both sides are constrained and the solid case runs to completion. This would be considered rigid clamping correct?
Nice!!
No. Both lips, Ninlet and Noutlet, are still free to rotate. You have constrained DOF from 1 to 3 and shellās nodes have up to 6 DOFs. Last three for rotations. But if it converged, you can keep going with it. One problem less.
Look closely to the animated result to see if thatās what you were expecting.
So, I fixed it for all 6 DOF but it diverged.
*BOUNDARY
Ninlet,1,6,0
Noutlet,1,6,0
Yep I know 
.
Too stiff or maybe the fact that curved shells have some issues when constraining rotational degrees of freedom out of plane. Mecway has been able to reduce that problem a lot.
If your goal is to fully solve the FSI, I would keep going. Thatās something you can work on it later with different approaches (already exposed in the forum, like for example selecting two rows of nodes instead of just the lip).