I am working on a similar thing. The way I have been advised to go about it (pertinent to my problem) is to constrain the surfaces so that all the plane surfaces remain plane at all times. I think this condition applied on all the surfaces takes care of the periodicity of the unit cell. The only problem is applying it!
Symmetric conditions don't seem to work. The only way I can think of is tieing the nodes together to have the same displacement along the axis perpendicular to the surface. CAE doesn't let me do that (atleast I haven't found out how to yet). Going to the input file and putting in the constraint on the nodes is a way but is too tedious, also am not sure about the over constraining of the nodes on the edges of the surface.
You should connect opposite side node values (e.g. displacement). The details depend on your FE code. I know that it is easy to apply PBC in ABAQUS and COMSOL (and it is described in their manuals clearly).
For quasistatic simulations in Ansys, I've used the nodal contraint equations approach to impose periodic boundary conditions. Constraints in ANSYS are implemented using a Lagrange multiplier approach, if I remember correctly. Caveat: There may be simpler approaches that have been provided by Ansys in the last 10 years that I'm not aware of.
Suppose you have a cube in which you want to apply periodic bcs on two opposite faces, for example x+ and x-. You will have to mesh the faces in such a way that both faces have exactly the same mesh geometry. This can be a nontrivial exercise.
Then you will have to loop through the nodes and tie corresponding nodes in x+ and x-, using constraint equations of the form u_i - u_j = 0 where i is a node on x- and j is the corresponding node on x+.
Start with simple geometries to test your approach - 1D, then 2D, then 3D.
Assuming that only the trial solution (displacement) is required to be periodic in the unit cell, then this can be achieved in one of two ways.
Method 1: If only the unique degrees of freedom (DOF) are stored, then the simplest approach is to change the DOF-connectivity of the element connected to the boundary on which periodicity is required to be enforced. In one-dimension, if the mesh consists of 3 linear elements, with nodes 1,2,3,4 (x1 = 0, x2 = 1/3, x3 = 2/3 and x4 = 1 are the nodal coordinates), then there exist only 3 unique DOFs with DOF 1 associated to node 1, DOF 2 associated to node 2, DOF 3 associated to node 3 and DOF 1 (again) associated to node 4. Even though there are four nodes in the mesh, only three unique DOFs exist, and it can be readily seen that the trial function is now value periodic. An illustration that shows the imposition of periodic boundary conditions in 1D appears on page 11 in the paper uploaded here. The same idea extends to two- and three-dimensions.
Method 2: If DOFs of all nodes (four in the above one-dimensional case) are created, then one can first construct the stiffness matrix and force vector for the entire system (assuming no periodicity at this point), and then carry out row-and-column algebraic operations (with subsequent deletions) to realize the reduced systerm of linear equations that is consistent with periodic boundary conditions. So, to take the one-dimensional example, the initial stiffness matrix is 4 x 4 and after the row-and-column operations, a 3 x 3 stiffness matrix is obtained, which is consistent with a periodic finite element bases and would be identical to that obtained via the first approach. Further details on these two equivalent approaches are provided in the aforementioned paper.
Periodic BC's and tieing nodes together
I am working on a similar thing. The way I have been advised to go about it (pertinent to my problem) is to constrain the surfaces so that all the plane surfaces remain plane at all times. I think this condition applied on all the surfaces takes care of the periodicity of the unit cell. The only problem is applying it!
Symmetric conditions don't seem to work. The only way I can think of is tieing the nodes together to have the same displacement along the axis perpendicular to the surface. CAE doesn't let me do that (atleast I haven't found out how to yet). Going to the input file and putting in the constraint on the nodes is a way but is too tedious, also am not sure about the over constraining of the nodes on the edges of the surface.
Anyone has any inputs on this??
Periodic BC
You should connect opposite side node values (e.g. displacement). The details depend on your FE code. I know that it is easy to apply PBC in ABAQUS and COMSOL (and it is described in their manuals clearly).
In reply to Periodic BC by Stephan Rudykh
Re: Periodic BCs in Ansys
For quasistatic simulations in Ansys, I've used the nodal contraint equations approach to impose periodic boundary conditions. Constraints in ANSYS are implemented using a Lagrange multiplier approach, if I remember correctly. Caveat: There may be simpler approaches that have been provided by Ansys in the last 10 years that I'm not aware of.
Suppose you have a cube in which you want to apply periodic bcs on two opposite faces, for example x+ and x-. You will have to mesh the faces in such a way that both faces have exactly the same mesh geometry. This can be a nontrivial exercise.
Then you will have to loop through the nodes and tie corresponding nodes in x+ and x-, using constraint equations of the form u_i - u_j = 0 where i is a node on x- and j is the corresponding node on x+.
Start with simple geometries to test your approach - 1D, then 2D, then 3D.
-- Biswajit
Imposing periodic BCs
Assuming that only the trial solution (displacement) is required to be periodic in the unit cell, then this can be achieved in one of two ways.
Method 1: If only the unique degrees of freedom (DOF) are stored, then the simplest approach is to change the DOF-connectivity of the element connected to the boundary on which periodicity is required to be enforced. In one-dimension, if the mesh consists of 3 linear elements, with nodes 1,2,3,4 (x1 = 0, x2 = 1/3, x3 = 2/3 and x4 = 1 are the nodal coordinates), then there exist only 3 unique DOFs with DOF 1 associated to node 1, DOF 2 associated to node 2, DOF 3 associated to node 3 and DOF 1 (again) associated to node 4. Even though there are four nodes in the mesh, only three unique DOFs exist, and it can be readily seen that the trial function is now value periodic. An illustration that shows the imposition of periodic boundary conditions in 1D appears on page 11 in the paper uploaded here. The same idea extends to two- and three-dimensions.
Method 2: If DOFs of all nodes (four in the above one-dimensional case) are created, then one can first construct the stiffness matrix and force vector for the entire system (assuming no periodicity at this point), and then carry out row-and-column algebraic operations (with subsequent deletions) to realize the reduced systerm of linear equations that is consistent with periodic boundary conditions. So, to take the one-dimensional example, the initial stiffness matrix is 4 x 4 and after the row-and-column operations, a 3 x 3 stiffness matrix is obtained, which is consistent with a periodic finite element bases and would be identical to that obtained via the first approach. Further details on these two equivalent approaches are provided in the aforementioned paper.
Howdy All, Are periodic
Howdy All,
Are periodic Boundary Conditions invoked by constraining all 6 DOFs?
I mean, would it suffice if I just constrain the translational DOFs and not the rotational DOFs of 'corresponding' nodes?
Sourav