Re: [Getfem-users] Elastic interface

[Yves Renard]

Dear Jean-François,

The "interpolate tranformation" tool is a generic tool but it can indeed be 
time consuming because for each Gauss point on the boundary, a search of the 
corresponding element on the other mesh is done. Although this search is 
optimized (rtree structures), it can be of course far more expensive than a 
standard assembly (however, in 2D it is done on a 1D interface so that it 
should be relatively fast).

However, in your case, the simpler way should be to do the job with a single 
mesh defining two different regions. You can define two different fields on the 
two regions by restricting the same "mesh_fem" to the dof of the corresponding 
region (with the partial_mesh_fem object, for instance, or with a filtered 
variable of the model object).
Then, you have to define two integration methods, one on each region to add the 
two different elasticity terms. Then, you can use the generic assembly without 
"interpolate transformation" to add your elasticity term on the interface (you 
have to define a mesh region by selecting the faces corresponding to your 
interface on only one side of the interface).

Another possibility is indeed to use a level-set and the mesh_fem_level_set 
object which describe a finite element space cut by the level-set. However, 
there is no tool for the moment to deal directly with the jump at the interface 
in the generic assembly (I agree that this would be interesting in many 
situations). So that, the easier way is again two define two different fields 
and use the level-set tools of getfem to define cut integrations methods 
(mesh_im_level_set) still using the generic assembly to add your elasticity 
term on the interface (using a integration method on the level-set, also 
provided by mesh_im_level_set). All is available on the python/matlab/scilab 
interface. You have some examples in the interface test programs:

interface/tests/python/demo_fictitious_domains.py
interface/tests/matlab/demo_fictitious_domains.m
interface/tests/matlab/demo_fictitious_domains_laplacian.m
interface/tests/matlab/demo_structural_optimization.m

Best regards,

Yves.


----- Original Message -----
From: "Jean-François Barthélémy" <address@hidden>
To: address@hidden
Sent: Sunday, December 28, 2014 12:15:47 PM
Subject: [Getfem-users] Elastic interface

Dear Getfem users, 

I am trying to find an easy and efficient way to take into account an elastic 
linear interface between two different materials in Getfem (using the python 
interface and/or in C++). The problem is defined on a uniform elastic matrix 
containing an elastic inclusion (with different moduli from that of the matrix) 
such that the matrix/inclusion interface is ruled by a relationship of the form 
T=K.[u] where T is the stress vector acting on the interface, K is the 
interface stiffness and [u] is the displacement jump (simple bilateral 
contact). Some finite element codes address this problem by allowing to build 
"joint elements". 

I have already succeeded in solving this problem but in a very inefficient way 
I think. I have indeed defined two differents meshes, one for the matrix and 
one for the inclusion. Although occupying the same geometrical domain, the 
interface boundaries are different from one mesh to the other (pairs of points 
at the same place but one in the matric mesh and the other one in the 
inclusion). I then defined two MeshFems, two variables (umat and uinc), two 
integration methods,... and the contribution of the interface to the global 
elastic stiffness "(umat-uinc).K.(Test_umat-Test_uinc)" by using the 
"interpolate transformation" to project fields expressed on one mesh to the 
other one (kind of mortar method on consistent boundaries). It works fine on a 
small mesh in 2D but is too time consuming on large meshes or in 3D. 

Is there a better way to do it either by using one or two meshes in which the 
interface correspond to element edges or, even better, by resorting to a 
levelset to define the interface independently of the mesh and xfem ? 

In the case of a levelset, how is it possible to build the discontinuous field 
of elastic moduli (the elements crossed by the levelset contain two different 
materials but how to correctly define all the degrees of freedom including 
those related to the Heaviside function) ? And finally how can I define the 
interface contribution to the stiffness ie integral_{interface} [ 
(umat-uinc).K.(Test_umat-Test_uinc) ] dS, possibly in a high-level generic 
assembly procedure in Python since I don't know how to access to discontinuity 
terms in the high-level language ? 

I haven't really found solutions to my questions in the examples (either 
related to mortar, cracks, contacts...) but I may have missed something. 

Thank you very much in advance for any help or piece of code. 

Best regards, 
Jean-François Barthélémy 


_______________________________________________
Getfem-users mailing list
address@hidden
https://mail.gna.org/listinfo/getfem-users