add periodic boundary script and example

Author: mkraska

README.md

@@ -191,3 +191,8 @@ This page uses animated gifs. In Firefox, you might want to install the plugin [
   width="200"
   title="Tensile test of an FDM structure perpendicular to the layer plane, generalized plane strain">
 ](RVE/PlaneOrtho1)
+[<img
+  src="RVE/Periodic/se-rot.png"
+  width="200"
+  title="Representative volume element with periodic boundary conditions">
+](RVE/Periodic)

RVE/Periodic/README.md

@@ -0,0 +1,63 @@
+# RVE with periodic boundary conditions
+Tested with CGX/CCX 2.11
+
+This is a generic RVE of a fiber-matrix compound.
+
++ Brick-shaped unit cell
++ Structured mesh
++ Location based assignment of material to elements
++ Periodic boundary conditions applied via helper script `periodic.py`
+
+Todo:
++ Output of the average nominal stress
++ Comfortable specification of load histories
+
+
+| File     | Contents    |
+| :------------- | :------------- |
+| [RVE.fbd](RVE.fbd)     | Pre-processing script for CGX (parametrized with valu commands)     |
+| [post.fbd](post.fbd) | Post-processing script for CGX (stress-strain curve and deformed plot) |
+| [Solve.inp](Solve.inp) | CCX input |
+
+## Preprocessing
+
+```
+> cgx -b RVE.fbd
+> periodic.py all.msh
+```
+
+The RVE represents a matrix material with unidirectional fibers arranged at a rectangular grid. Dimension  `lx` is irrelevant, as the material is uniform
+in x direction. Dimensions `ly` and `lz` represent the fiber grid lengths.
+
+The mesh consists of C3D8I elements and is controlled by a global node distance.
+
+| Parameter | Value | Meaning |
+| :------------- |  :------------- | :------------- |
+| `lx` | 1 | length in x in mm |
+| `ly` | 1 | length in y in mm |
+| `lz` | 1 | length in z in mm |
+| `rad` | 0.2 | fiber radius |
+| `le` | 0.1 | node distance |
+
+Constraints:
+
+* `periodic.py` produces set definitions for control nodes and the equations for periodicity.
+* Components of the average deformation gradient or of the average nominal stress (first Piola-Kirchhoff stress) can be specified as displacements or forces at the control nodes.
+
+<img src="matrix.png" width="400"><img src="fiber.png" width="400">
+
+## Solving
+```
+> ccx Solve
+```
+
+## Postprocessing
+
+Plots of the equivalent stress, the periodicity of the deformation is visible.
+```
+> cgx -b post.fbd
+```
+
+
+<img src="se.png" width="400" title="Displacement in x">
+<img src="se-rot.png" width="400" title="Displacement in y">

RVE/Periodic/RVE.fbd

@@ -0,0 +1,43 @@
+valu lx 1
+valu ly 1
+valu lz 1
+valu le 0.1
+valu rad 0.21
+valu tol 0.00001
+
+# create the cube
+pnt p0 0 0 0
+swep all new tra lx 0 0
+swep all new tra 0 ly 0
+swep all new tra 0 0 lz
+
+# meshing
+div all auto le
+elty all he8i
+mesh all
+send all abq
+
+# create fiber (cylinder along x in the center)
+valu two 2
+valu my / ly two
+valu mz / lz two
+seta nodes n all
+enq nodes fiber rec _ my mz rad
+comp fiber up
+
+# define set for the matrix
+seta matrix se all
+setr matrix e fiber
+
+# write set definitions
+send all abq nam
+
+# images
+view elem
+frame
+plot e fiber r
+hcpy png
+sys mv hcpy_1.png fiber.png
+plot e matrix n
+hcpy png
+sys mv hcpy_2.png matrix.png

RVE/Periodic/Solve.inp

@@ -0,0 +1,27 @@
+*include,input=all.msh
+*include,input=fiber.nam
+*include,input=matrix.nam
+** constraints
+*include,input=periodic.equ
+*boundary
+n0, 1,3
+*material, name=matrix
+*elastic
+2000,0.3,0
+*material, name=fiber
+*elastic
+150000,0.3,0
+*solid section, elset=Ematrix, material=matrix
+*solid section, elset=Efiber, material=fiber
+*STEP, NLGEOM,inc=200
+*STATIC
+*boundary
+nx,1,1,0.2
+nx,2,3
+ny,3,3,0.2
+nz,2,2,0
+*el file
+S
+*node file
+U
+*end step

RVE/Periodic/fiber.png

@@ -0,0 +1,16 @@
+read Solve.frd
+
+ds 2 e 7
+view disp
+view elem
+plot fv all
+rot -x
+rot c -90
+frame
+hcpy png
+sys mv hcpy_1.png se.png
+rot r 20
+rot u 20
+frame
+hcpy png
+sys mv hcpy_2.png se-rot.png