yes, I see, I forgot something. It should be:
SNRJ = gf.asm_generic(mimp3b, 1,
"(Gb*Grad(ub):Grad(ub)+Gb/(1-2*nub)*Div(ub)*Div(ub))*Test_t", -1, md,
"t", True, mfpb,
np.zeros(mfpb.nbdof()), "select_output", "t")
otherwise the asm_generic function will include all model dofs which are
not used in the expression.
Best regards
Kostas
On Thu, Jan 27, 2022 at 11:00 PM Lesage,Anne Cecile J <
ajles...@mdanderson.org> wrote:
> Dear Konsta
>
>
>
> I wrote the following lines
>
>
>
> print('mfpf dofs',mfpb.nbdof(),'mfoutb dofs',mfoutb.nbdof())
>
> mass_mat = gf.asm_mass_matrix(mimp3b, mfpb)
>
>
>
>
>
> for step in range(steps):
>
> nit, conv = md.solve('noisy', 'max_iter', 25, 'max_res', 1e-10,
> 'lsolver', 'mumps',
>
> 'lsearch', 'simplest', 'alpha max ratio', 100,
> 'alpha min', 0.2, 'alpha mult', 0.6,
>
> 'alpha threshold res', 1e9)
>
> time_elapsed(timer)
>
> it = step+1
>
> SNRJ = gf.asm_generic(mimp3b, 1,
> "(Gb*Grad(ub):Grad(ub)+Gb/(1-2*nub)*Div(ub)*Div(ub))*Test_t", -1, md,
>
> "t", True, mfpb,
> np.zeros(mfpb.nbdof()))
>
> SNRJ = np.transpose(gf.linsolve_mumps(mass_mat, SNRJ))
>
>
>
> But I get a size error as follows on the transpose line
>
>
>
>
>
> <pre>mfpf dofs 54026 mfoutb dofs 54026
>
> Time elapsed: 9.0 minutes and 40.03 seconds
>
> Traceback (most recent call last):
>
> File "/work/testr25pebrainbsftslhomnrj.py", line 271, in
> <module>
>
> SNRJ = np.transpose(gf.linsolve_mumps(mass_mat, SNRJ))
>
> File "/venv/lib/python3.8/site-packages/getfem/getfem.py",
> line 6447, in linsolve_mumps
>
> return getfem('linsolve', 'mumps', M, b)
>
> RuntimeError: (Getfem::InterfaceError) -- Argument 3 has wrong dimensions:
> expected 54026, found 1339902</pre>
>
>
>
> Thank you
>
> AC
>
>
>
> *From:* Konstantinos Poulios <logar...@googlemail.com>
> *Sent:* Wednesday, January 26, 2022 2:24 AM
> *To:* Lesage,Anne Cecile J <ajles...@mdanderson.org>
> *Cc:* getfem-users@nongnu.org
> *Subject:* Re: [EXT] Re: Computing the linear elastic strain energy
>
>
>
> *WARNING: *This email originated from outside of MD Anderson. Please
> validate the sender's email address before clicking on links or attachments
> as they may not be safe.
>
>
>
> Dear Anne-Cecile,
>
>
>
> Ok, I see. I would not do node-averaging, like most commercial (and not
> only) software do, for exporting smooth scalar fields (von Mises, strain
> energy, etc.). Instead, my favorite approach is the one that you can find in
>
>
> https://git.savannah.nongnu.org/cgit/getfem.git/tree/interface/tests/python/demo_finite_strain_plasticity_3D.py
> <https://urldefense.com/v3/__https:/git.savannah.nongnu.org/cgit/getfem.git/tree/interface/tests/python/demo_finite_strain_plasticity_3D.py__;!!PfbeBCCAmug!wugJEgC0-WoDQzcgHwoZj5gYuTCA8KyuOZ3mE5mEy45wApyQgTuf2h_rRcM-rIzopg$>
>
> for exporting the plastic strain field GAMMA.
>
>
>
> What you need for this method is:
>
>
>
> 1) Before starting your simulation you calculate and store a mass matrix
> for the scalar mesh_fem that you want to get the nodal values for
>
> mass_mat = gf.asm_mass_matrix(mim, mfout)
>
> mfout has to be a scalar fem (1 dof per node).
>
>
>
> 2) After (each step of) your simulation, you assemble the quantity that
> you want to export, in this case strain energy with something like
>
> STRAIN_ENERGY = gf.asm_generic(mim, 1,
> "(Gb*Grad(ub):Grad(ub)+Gb/(1-2*nub)*Div(ub)*Div(ub))*Test_t", -1, md,
> "t", True, mfout,
> np.zeros(mfout.nbdof()))
>
> (check the correctness of the strain energy expression that I took from
> some code you sent earlier)
>
>
>
> 3) Recover nodal values with
>
> STRAIN_ENERGY = np.transpose(gf.linsolve_mumps(mass_mat, STRAIN_ENERGY))
>
> Then the vector STRAIN_ENERGY has the nodal values of the strain energy
> on all dofs of mfout. If you calculate this vector for several simulations
> or simulation steps, you can copy the result into different columns of a
> big matrix as in the paper you are referring to.
>
>
>
> Hope it helps.
>
>
>
> BR
>
> Kostas
>
>
>
> On Tue, Jan 25, 2022 at 8:50 PM Lesage,Anne Cecile J <
> ajles...@mdanderson.org> wrote:
>
> Dear Konstantinos
>
>
>
> The problem with patient specific surgery modeling is that we ignore a lot
> of the surgery scenario
>
> One way to model it with FEM is to precompute an atlas of organ
> deformation with a variety of surgery scenario parameter (here direction of
> gravity, loss of brain buoyancy by csf drainage, shrinkage due to drug,
>
> swelling due to edema, tumor resection, etc …) That is about 1000
> simulations
>
>
>
> Then the idea is to match intraoperative data, the surgeons measure a
> ground truth displacement on a few brain surface points
>
> The idea is to minimize function equation 7 in attached pdf:
>
> the first term is the least square between the ground truth displacement
> and the simulated one see equation
>
> the second term use the elastic strain energy on fem points pondered by
> the distance to the ground truth measurement points
>
> Finally we want to get the optimal alpha pondering vector to match the
> surgery measurement
>
>
>
> Ideally I would like my python script to output after poroelastic
> simulation converge
>
> The simulated displacements on the few measurement points (15)
>
> The pondered energy term
>
> So that I can assemble the function to minimize for the whole atlas
>
>
>
> Thank you
>
> Regards
>
> Anne-Cecile
>
>
>
>
>
> *From:* Konstantinos Poulios <logar...@googlemail.com>
> *Sent:* Tuesday, January 25, 2022 2:40 AM
> *To:* Lesage,Anne Cecile J <ajles...@mdanderson.org>
> *Cc:* getfem-users@nongnu.org
> *Subject:* [EXT] Re: Computing the linear elastic strain energy
>
>
>
> *WARNING: *This email originated from outside of MD Anderson. Please
> validate the sender's email address before clicking on links or attachments
> as they may not be safe.
>
>
>
> Dear Anne-Cecile
>
>
>
> The elastic strain energy density (is a scalar) at each node is easy to
> calculate. However, I have to ask you what you need this quantity for. Your
> reference suggests calculating this quantity on nodes which is probably not
> the best solution. If you calculate the strain energy density at a node
> between different elements, you get different results depending on which
> element you are evaluating the common node from. Then some averaging is
> required to get a value somewhere between all neighboring elements.
> Normally we evaluate strain energy densities at integration points. If you
> tell us what you need this result for I can maybe help with a better
> solution.
>
>
>
> Best regards
>
> K.
>
>
>
> On Mon, Jan 24, 2022 at 9:09 PM Lesage,Anne Cecile J <
> ajles...@mdanderson.org> wrote:
>
> Dear all
>
>
>
> I need to output tat the end of my poroelastic simulation the linear
> elastic strain energy matrix at each node of my mesh
>
> See attached formula
>
> What is an optimal way to compute it from the displacement u?
>
> Epsilon i = 0.5 (grad u + grad ut) right?
>
> And S here is the stress-strain law for isotropic materials?
>
>
>
> Thank you
>
> Anne-Cecile
>
> The information contained in this e-mail message may be privileged,
> confidential, and/or protected from disclosure. This e-mail message may
> contain protected health information (PHI); dissemination of PHI should
> comply with applicable federal and state laws. If you are not the intended
> recipient, or an authorized representative of the intended recipient, any
> further review, disclosure, use, dissemination, distribution, or copying of
> this message or any attachment (or the information contained therein) is
> strictly prohibited. If you think that you have received this e-mail
> message in error, please notify the sender by return e-mail and delete all
> references to it and its contents from your systems.
>
> The information contained in this e-mail message may be privileged,
> confidential, and/or protected from disclosure. This e-mail message may
> contain protected health information (PHI); dissemination of PHI should
> comply with applicable federal and state laws. If you are not the intended
> recipient, or an authorized representative of the intended recipient, any
> further review, disclosure, use, dissemination, distribution, or copying of
> this message or any attachment (or the information contained therein) is
> strictly prohibited. If you think that you have received this e-mail
> message in error, please notify the sender by return e-mail and delete all
> references to it and its contents from your systems.
>
> The information contained in this e-mail message may be privileged,
> confidential, and/or protected from disclosure. This e-mail message may
> contain protected health information (PHI); dissemination of PHI should
> comply with applicable federal and state laws. If you are not the intended
> recipient, or an authorized representative of the intended recipient, any
> further review, disclosure, use, dissemination, distribution, or copying of
> this message or any attachment (or the information contained therein) is
> strictly prohibited. If you think that you have received this e-mail
> message in error, please notify the sender by return e-mail and delete all
> references to it and its contents from your systems.
>
