Hello Kostas,
your approach works perfectly for me.
I checked me code and it seems like there was a little typing error. So
what I did at first works too. But your approach seems to be faster. (Some
warnings occure in my code.)
I have one last question at the moment. This question concerns the line
md.add_nonlinear_term(mim, "Th*0.5*kappa*sqr(log(Det(F)))+"
Th*0.5*mu*(pow(Det(F),-2/3)*Norm_sqr(F)-3)")
Where did you get that expression from? Is there any literatur, where I
can find such expressions? Or can you give me an approach to deriving that
expression?
Best regards,
Moritz Jena
Von: Konstantinos Poulios <[email protected]>
An: Moritz Jena <[email protected]>
Kopie: getfem-users <[email protected]>
Datum: 03.07.2019 23:20
Betreff: Re: Re: [Getfem-users] Antwort: Re: 2D nonlinear plane
stress
Dear Jena,
Without having run your code I would say that your definition of the 3D
deformation gradient looks correct. Another way of converting from 2x2 to
3x3 is
"(Id(3)+[[1,0,0],[0,1,0]]*Grad_u*[[1,0,0],[0,1,0]]')"
but it should be equivalent to your approach.
Could you attach a screenshot of the "strange" solution that you get?
BR
Kostas
On Wed, Jul 3, 2019 at 9:49 AM Moritz Jena <[email protected]>
wrote:
Hello Kostas and all GetFEM-Users,
I finally managed to try your approach for my plane stress problem.
But unfortunately I got a problem with it.
When defining the 3D deformation gradient, I have to add a [2x2] - matrix
to a [3x3]- matrix. To work around this problem I tried to rewrite the
displacement gradient to a [3x3] - matrix.
So instead of
md.add_macro("F", "Id(3)+Grad_u+epsZ*[0,0,0;0,0,0;0,0,1]")
it tried
md.add_macro("F",
"Id(3)+[Grad_u(1,1),Grad_u(1,2),0;Grad_u(2,1),Grad_u(2,2),0;0,0,0]+epsz*[0,0,0;0,0,0;0,0,1]")
To test the approach, I created a little test-script with a simple beam
and a force. The calculation works with this work around, but the
deformation seems something strange. I think I did a mistake by accessing
the matrix-elements of the displacement gradient, but I'm not sure about
it.
Can you, or anyone else, help me with my problem?
import getfem as gf
import numpy as np
# Parameter
l = 100
h = 10
b = 1.5
size = 1
E = 203000
nu = 0.3
Lambda = (E*nu)/(1-pow(nu,2))
mu = E/(1+nu)
lawname = 'SaintVenant Kirchhoff'
# Create mesh
m = gf.Mesh('cartesian', np.arange(0, l+size , size), np.arange(0, h+size,
size))
#MeshFem
mfu = gf.MeshFem(m,2)
mfd = gf.MeshFem(m,1)
mf1 = gf.MeshFem(m,1)
#assign FEM
mfu.set_fem(gf.Fem('FEM_QK(2,2)'))
mfd.set_fem(gf.Fem('FEM_QK(2,2)'))
mf1.set_fem(gf.Fem('FEM_QK(2,1)'))
#IM_methode
mim = gf.MeshIm(m, gf.Integ('IM_GAUSS_PARALLELEPIPED(2,6)'))
# Some Infos
print("nbcvs = %d | nbpts = %d | qdim = %d | nbdofs = %d" % (m.nbcvs(),
m.nbpts(), mfu.qdim(), mfu.nbdof()))
#regions
P = m.pts();
pidleft = np.compress((abs(P[0,:])<1e-6),range(0,m.nbpts()))
pidrigth = np.compress((abs(P[0,:])>l-1e-6),range(0, m.nbpts()))
left = m.outer_faces_with_direction([-1, 0], 0.5)
rigth = m.outer_faces_with_direction([1,0], 0.5)
fleft = m.faces_from_pid(pidleft)
frigth = m.faces_from_pid(pidrigth)
m.set_region(1, fleft)
m.set_region(2, frigth)
#Model
md = gf.Model('real')
md.add_fem_variable('u', mfu)
md.add_initialized_data('lambda', Lambda)
md.add_initialized_data('mu', mu)
md.add_fem_variable("epsz", mf1)
md.add_initialized_data('kappa', 68000)
md.add_initialized_data('Th', 0.2)
#material
md.add_macro("F",
"Id(3)+[Grad_u(1,1),Grad_u(1,2),0;Grad_u(2,1),Grad_u(2,2),0;0,0,0]+epsz*[0,0,0;0,0,0;0,0,1]")
md.add_nonlinear_term(mim,
"Th*0.5*kappa*sqr(log(Det(F)))+Th*0.5*mu*(pow(Det(F),2/3)*Norm_sqr(F)-3)")
# fixed support left side
md.add_initialized_data('DirichletData1', [0,0])
md.add_Dirichlet_condition_with_multipliers(mim, 'u', mfu, 1,
'DirichletData1')
# force on rigth side
md.add_initialized_data('VolumicData', [0,0])
md.add_source_term_brick(mim, 'u', 'VolumicData')
md.add_Dirichlet_condition_with_multipliers(mim, 'u', mfu, 2,
'VolumicData')
# force array
F = np.array([[0,-4], [0,-10], [0,-15], [0,-25], [0,-35], [0,-50]])
nbstep = F.shape[0]
#iterative calc
for step in range(0, nbstep):
print(step)
md.set_variable('VolumicData', [F[step, 0],F[step,1]])
md.solve('noisy', 'max_iter', 50)
U = md.variable('u')
s1 = gf.Slice(('boundary',), mfu, 4)
s1.export_to_vtk('test_%d.vtk' % step, 'ascii', mfu, U ,
'Displacement')
Von: Konstantinos Poulios <[email protected]>
An: Yves Renard <[email protected]>
Kopie: Moritz Jena <[email protected]>, getfem-users <
[email protected]>
Datum: 05.02.2019 10:05
Betreff: Re: [Getfem-users] Antwort: Re: 2D nonlinear plane stress
Dear Moritz Jena,
To define a hyperelastic material law for a plane stress problem, the
easiest way is to add one extra variable representing the out of plane
strain. If mf1 is a scalar fem and mf2 is a vector fem with 2 components,
then you can simply do:
md = gf.Model("real")
md.add_fem_variable("u", mf2) # displacements variable
md.add_fem_variable("epsZ", mf1) # out of plane strain variable
md.add_initialized_data(’kappa’, kappa) # initial bulk modulus
md.add_initialized_data(’mu’, mu) # initial shear modulus
md.add_initialized_data(’Th’, Th) # plate thickness
md.add_macro("F", "Id(3)+Grad_u+epsZ*[0,0,0;0,0,0;0,0,1]") # 3D
deformation gradient
md.add_nonlinear_term(mim, "Th*0.5*kappa*sqr(log(Det(F)))+"
Th*0.5*mu*(pow(Det(F),-2/3)*Norm_sqr(F)-3)")
Best regards
Kostas
On Wed, Jan 16, 2019 at 9:40 PM Yves Renard <[email protected]>
wrote:
Dear Jena,
For an hyperelastic law, the weak form of the static elastic problem can
be written in the weak form language
"Def F := Id(meshdim)+Grad_u; (F * S) : Grad_test_u"
for u the displacement, F the deformation gradient and S has to contains
the expression of the second Piola-Kirchhoff stress tensor (you can of
course express it in term of PK1 also). For instance for a St Venant
Kirchhoff law, you can write
"Def F := Id(meshdim)+Grad_u; Def E := 0.5*(F'*F-Id(meshdim)); (F *
(lambda*Trace(E)+2*mu*E)) : Grad_test_u"
where E will be the Green Lagrange deformation tensor and lambda, mu the
Lamé coefficients.
This gives you some examples of construction of hyperelastic laws. The
weak form language gives you access to some standard operators (Trace, Det
...) see
http://getfem.org/userdoc/model_nonlinear_elasticity.html#high-level-generic-assembly-versions
So, if you have the expression of your law in plane stress, it should not
be very difficult to implement it. But of course you need the expression
of the law in plane stress. On the construction itself of plane stress
hyperelastic law, now, I don't know a good reference, unfortunately.
Best regards,
Yves
----- Original Message -----
From: "Moritz Jena" <[email protected]>
To: "yves renard" <[email protected]>
Cc: "getfem-users" <[email protected]>
Sent: Wednesday, January 16, 2019 2:17:01 PM
Subject: Antwort: Re: [Getfem-users] 2D nonlinear plane stress
Hello Yves,
thank you for your answer.
I'm afraid I'm not into the topic weak form language and I'm not sure
where to start with this problem.
I looked at the chapter in the documentation, however I don't know how to
describe a plane stress material model with it.
I also studied the examples, that come with the MATLAB-Interface. There
are a few examples, how to declare a material model with this weak form
expressions. But I still don't know, how to build this expressions.
Can you give me a approach for this problem or where I can find
expressions for such a problem? Is there any literature that you can
recommend?
Best regards,
Moritz
Von: Yves Renard <[email protected]>
An: Moritz Jena <[email protected]>
Kopie: getfem-users <[email protected]>
Datum: 09.01.2019 17:17
Betreff: Re: [Getfem-users] 2D nonlinear plane stress
Dear Moritz Jena,
No, unfortunately, plane stress versions of Hyperelastic laws has not been
implemented yet.
I would not be so difficult, but as to be made. If you need one in
particular and have the expression, it is no so difficult to describe it
with the weak form language.
Best regards,
Yves
----- Original Message -----
From: "Moritz Jena" <[email protected]>
To: "getfem-users" <[email protected]>
Sent: Tuesday, January 8, 2019 4:11:48 PM
Subject: [Getfem-users] 2D nonlinear plane stress
Dear GetFEM-Users,
I use the MATLAB-Interface of GetFEM to create a program that
automatically solves different models of the same problem.
The problem is three-dimensional, but can be reduced by plain stress
approximation. (to reduce computing time).
I want to define a nonlinear material with the brick
gf_model_set(model M, 'add nonlinear elasticity brick',
[...])
For this nonlinear command it is specified in the description, that in 2D
always plain strain is used.
So my question is: Is there a way to define a nonlinear material with the
plain stress approximation? Or is it planned to install such an option in
a future release?
I hope you can help me with my problem.
Best regards,
Moritz Jena
