Milton,
Ive tried quite a few things.
I have tried both full and reduced integration elements (C3D8H and C3D8HR)
for the tube when i modelled it as hyperelastic.
I have a good idea of the modulus of the material at low strains.. so i also
tried to model the tube as linear (C3D8 and C3D8H) and made the materials
slightly compressible, possions ratio of 0.46 because i thought my problem
might have something to do with volumetric locking.
The stent elements are C3D8I. But for a bit now i have just been forcing
displacements on the stent. So i dont think that they are all that important
to me at the moment.
So my steps work as follows:
Crimp. STENT is reduced to just below inner diameter of wall (Displacement
constraint (R-4.2, T0, Z0))
Contact: Activate the contact and activate the WALL BC (R-, T0, Z0)
Expand: Make the STENT a bit bigger in diameter (Displacement constraint
(R-3.95, T0, Z0))
Pull: finally im trying to move the stent out and see what friction forces
are set up (Displacement constraint R-3.95, T0, Z5)
Its almost like the outside surface of my wall doesnt want to deform.. when
the stent comes into contact i am getting no uniform distribution of
stress.. just right under the strut. i checked my units and all is ok there
Im using surface to surface contact, Finite sliding, Node centered, and
single configuration. Im not using any adjustment of the slave nodes or
surfaces because i think that occurs at the start of the analysis before i
crimp and the surfaces are not close then. i suppose i could remodel the
stent to be in its crimped state and then expand it and try to do some slave
node adjustment before the analysis.
While the stent is expanding i have no friction turned on. The contact is
default, hard contact with the surfaces allowed to separate. im using
contact damping of 0.25 and a clearane of 0.01.. im not 100% sure about the
damping settings. but the damping factor was calculated as per the manual..
and it is helping with convergence.
I have shown a closeup below with and without the stent, looking in along
the stent strut. you can see that all the deformation is on the inside
surface of the wall and that there is only very localised stresses. In the
case shown the tube material is linear with a poissons ratio of 0.46. The
elements are R3D8H. I dont understand how i can be getting hourglassing as
the manual says that it only affects reduced integration elements!
Loading Image...
Post by Milton DeherreraOK, I see it now... Looks even stranger, and you might be getting
hourglassing in the tube (hard to tell without a closeup)... Can you tell
me what properties you're using for the tube and for the stent? You may
also consider using shell elements (s4r) for the tube, but I'll leave that
up to you.
Post by T_C_Milton, Just to add that in the image that the stent is removed to show the
distortion of the wall
I am getting no real problems with the stent.
Post by Milton Deherrera1. You seem to be getting severe hourglassing in the stent, which is not
a good thing.
2. If you're not interested in the stent, you can model it as rigid by
using r3d3 or r3d4 elements to represent the stent's outer surface. In
this
case you would need to make the stent the master, because when you have
rigid to deformable contact, the rigid body has to be the master. You can
"deform" the rigid stent by specifying a radial motion in cylindrical
coordinates.
3. If you do model the stent as a deformable body, you will need to
either mesh it with c3d8i or refine the mesh, otherwise you'll continue to
get hourglassing.
4. Make sure your material properties are in consistent units; when
modeling metal to elastomer contact, I have seen people get in trouble more
than once by using MPa for the metal and kPa for the hyperelastic
coefficients.
Good luck!
On Thu, Oct 8, 2009 at 5:19 PM, T_C_
Post by T_C_Thanks again milton. I appreciate all your suggestions!
The stent isnt my main concern at all really at the moment.
I was actually thinking of modelling the stent as rigid but i think
its
Post by Milton DeherreraPost by T_C_better to keep the stent as the slave and making it rigid means i
cannot
Post by Milton DeherreraPost by T_C_do
that.
Im more concerned with the behaviour of the wall.
Im still getting weird and very localised distortions around the stent
strut. I have tried making the wall elements C3D8H as i thought that
it
Post by Milton DeherreraPost by T_C_might reduce the distortion but it still seems to be happening.. Ive posted
a picture below. its scaled but you can see that the inner wall is
taking
Post by Milton DeherreraPost by T_C_all the deformation and that its very localised. and that there is
almost
Post by Milton DeherreraPost by T_C_no
deformation or stress on the outer wall (you can just barely make out
deformation on the outside wall). it should obviously get bigger in diameter
all around the stented area. The ends of the tube are held in the Z
and
T
Post by Milton DeherreraPost by T_C_directions. Would making the wall elements C3D8I help?
http://www.nabble.com/file/p25813810/Document1.jpg
Post by Milton DeherreraIf you're limited to 3 or 4 elements across the depth, you should
use
Post by Milton DeherreraPost by T_C_Post by Milton Deherrerac3d8i
elements, otherwise you won't capture the bending in the struts very
well,
Post by Milton Deherreraparticularly with 3 elements.
On Wed, Oct 7, 2009 at 4:18 PM, T_C_
<timmyc2005%40gmail.com><timmyc2005%40gmail.com>>
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_Thanks for the comments.
Im using 4 elements through the wall. and three across the strut.
The
Im
be
Post by Milton DeherreraPost by T_C_nice
Post by Milton DeherreraPost by T_C_obviously if my results were within 20% of what they should be!
I have solved the problem somewhat. i was using different BCs on
the
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_stent
for different steps.
on cylindrical coords my first constraint to crimp was
R - 5
T - 0
Z - 0
then my BC after contact was turned on was
R - -
T- 0
Z - 0
i thought that this would allow the system to balance and that by
not
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_specifying any movement in the R direction that the stent would be
influenced by the wall.. the outward force of the stent and the
inward
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_force
of the silicone rubber would balance.
I figured out that the stent was returning to its uncrimped
diameter
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_though
so by just using one BC and modifying it after each step it worked
pretty
Post by Milton DeherreraPost by T_C_ok.. my distortion problem is much much less.
Post by Milton DeherreraMy suggestion would be to do this using ABAQUS/Explicit with mass
scaling,
Post by Milton Deherreraparticularly the crimping part of your analysis. Also, you should
be
the
Post by Milton DeherreraPost by T_C_<timmyc2005%40gmail.com><timmyc2005%40gmail.com>>
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_Hi,
Im trying to do a contact analysis in abaqus standard v6.7.
Im simulating a stent being crimped and then expanded inside a
silicone
Post by Milton DeherreraPost by T_C_rubber artery model. (its a bit like one tube inside another but
the
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_inside
tube is a bit complex in geometery)
Im then displacing the stent in the axial direction and looking
at
Post by Milton DeherreraPost by T_C_the
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_frictional forces set up using a history output request.
All the above is done with displacement constraints. there are
no
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_loads
Post by Milton DeherreraPost by T_C_on
the model.
The stent is nitinol and meshed with C3D8R elements.
The wall is Hyperelastic and meshed with C3D8RH elements.
Unfortunately when i expand the stent im getting excessive
distortion
Post by Milton DeherreraPost by T_C_of
Post by Milton DeherreraPost by T_C_the
mesh. I have tried enhanced hourglass stiffness and specifying a
(ridiculously) high hourglass stiffness in the element type
window
reduce
Post by Milton DeherreraPost by T_C_the
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_distortion somewhat it made the results useless.
Im not sure what kinematic split and second order accuracy do or
if
Post by Milton DeherreraPost by T_C_when
Post by Milton DeherreraPost by T_C_the
Post by Milton DeherreraPost by T_C_body is rotating. thats not really the case in my model.
There is an option in the element type window of distortion
control
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_but
Post by Milton DeherreraPost by T_C_that
doesnt work with hybrid elements it seems.
Any ideas or suggestions appreciated!
--
http://www.nabble.com/Stent%2C-rubber-contact-tp25783901p25783901.html
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_Sent from the Abaqus Users mailing list archive at Nabble.com.
[Non-text portions of this message have been removed]
--
http://www.nabble.com/Stent%2C-rubber-contact-tp25783901p25796087.html
Post by Milton DeherreraPost by T_C_Post by Milton DeherreraPost by T_C_Sent from the Abaqus Users mailing list archive at Nabble.com.
[Non-text portions of this message have been removed]
--
http://www.nabble.com/Stent%2C-rubber-contact-tp25783901p25813810.html
Sent from the Abaqus Users mailing list archive at Nabble.com.
[Non-text portions of this message have been removed]
--
http://www.nabble.com/Stent%2C-rubber-contact-tp25783901p25826078.html
Sent from the Abaqus Users mailing list archive at Nabble.com.
[Non-text portions of this message have been removed]
--
View this message in context: http://www.nabble.com/Stent%2C-rubber-contact-tp25783901p25834174.html
Sent from the Abaqus Users mailing list archive at Nabble.com.
