FEM Shear of a Composite Block

Introduction
In this tutorial we analyze the shear deformation of a composite block consisting of a stiff core embedded in a soft matrix. It demonstrates the use of BooleanFragments and CompoundFilter to create solids for the block and the matrix from two concentric cubes. This work-flow ensures that separate MeshRegions, Materials and Boundary Conditions can be defined for the block and the surrounding matrix. The CalculiX results clearly show the effect of the stiff core on the response of the composite block.

Geometry
First we create two concentric cubes, one size 10mm and the other size 5mm. This is done in the workbench "Part". By default the cube is placed at the origin [0, 0, 0], so the smaller cube needs to be scaled down and shifted by changing the settings in the Data tab of the property panel. To make the core visible, the Transparency of the outer block is set to 50 in the View tab of the property panel. The result is shown below.



Mesh and Mesh Regions
From workbench FEM we create an Analysis container. This will contain all definitions required for the CalculiX analysis and its results. Note that this Analysis container needs to be activated (right-click and select "Activate analysis") whenever re-loading the file or after switching back from other analyses. To start the meshing process, highlight the CompoundFilter in the Object Tree and activate the meshing dialog "Mesh > FEM mesh from shape by Gmsh". Leave the dialog by clicking OK.

A Mesh object is now created in the Object Tree. Highlight this object and create a Mesh Region object via "Mesh > FEM mesh region". Open the dialog box for this Mesh Region by double clicking and tick the radio button for Solid. Next click the "Add Reference" button and select the Cube_Matrix object in the Graphical Window. This should add a reference to "Box:Solid1" in the object list of the Mesh Region. Finally specify the maximum element size for this region (5mm in the current analysis). Leave the dialog by clicking OK.



Next make the Cube_Matrix object invisible by highlighting it and pressing the space bar. In a similar way make the Cube_Core visible. Now create a new Mesh object as above and select the Cube_Core object in the Graphical Window. This time the reference list should show "Box001:Solid1", as below. This time we chose a maximum element size of 1mm



Material Assignment
Material is assigned to Mesh Regions via a SolidMaterial object. In this tutorial we assign two materials; one for the Matrix and one for the Core.

Start by making the Cube_Matrix visible as in the above section. Then create a SolidMaterial object via menu option "Model > FEM material for solid". Open the dialog and tick the radio button for Solid, press "Add Reference" and select the Cube_Matrix from the Graphical Window. The reference list should now show "Box:Solid1", as before. We assign ABS material to this region, with a Young's modules approximately 1% that of steel.



Next make Cube_Matrix invisible and Cube_Matrix visible. Repeat the above procedure for Cube_Core. This time we assign CalculiX-Steel, which is much stiffer than the ABS material for the Matrix.



Sliding Support
To create a "Simple Shear" condition for the composite block the deformations at the boundaries need to be unconstrained. To achieve this, the block is placed on a sliding support. This leaves three degrees of freedom in the plane of the support (2 translations and a rotation) and those will be constrained later. (Note: as the plane prevents warping of the face, it still induces a minor constraint, which could be eliminated by a different choice of boundary conditions). To create a sliding boundary condition add a FemConstraintDisplacement object (Model > Mechanical Constraints > Constraint displacement). With the dialog box open first select the face to which the boundary conditions is to be applied and then click the Add button. As the block is allowed to slide in the x-y plane, only the "Fixed" radio button for "Displacement z" is selected and the other radio buttons are all left as "Free".



Fixed Nodes
To prevent rigid body motion in the plane of sliding, three independent degrees of freedom need to be eliminated. To achieve this, one vertex in the plane of sliding is constrained in x and y direction (eliminating 2 degrees of freedom) and one vertex is fixed in the x direction (eliminating the last degree of freedom). For this purpose two additional FemConstraintDisplacement objects are created and the result is shown below.



Shear Forces
The final step in the Analysis definition is the application of loads. To create a Simple Shear condition, a set of shear loads is applied as shown below. Each load is chosen as 1000 N and considering the directions of application, force and moment equilibrium is achieved for all translation and rotional degrees of freedom. In FC this requires addition of four FemConstraintForce objects (Model > Mechanical Constraints > Constraint force) - one for each face. With the dialog box open first press the Add Reference button and then select the face to which the boundary condition is to be applied (Note: this is a different sequence than with FemConstraintDisplacement). By default, this creates a set of forces perpendicular to the face (i.e. a normal force). To change this to a shear force, press the direction button and select a cube edge that runs in the desired direction. If the resulting force points in opposite direction of what is required, then select the radio button for "Reverse direction".



CalculiX Analysis
Now all mesh regions, material and boundary conditions have been defined we are ready to analyse the deformation of the block with CalculiX. Activate the Analysis by right clicking "Activate analysis", open the CalculiX dialog by double clicking the CalculiXccxTools object and select a directory for the temporary files created by both FC and CCX. Write CCX Input file and check for any warning or error messages.



After that the analysis can be started by pressing the RunCalculiX button. If all goes well, the CCX output window should show the following messages.



CalculiX Results
Upon completion of the analysis double click the CalculiX_static_results object and select the "Abs displacement" option. The maximum displacement of ~ 0.08mm will show up in the relevant output box. As the maximum displacement is relatively small to the dimensions of the block (<1% of the block size), the displacements need to be scaled. This can be done under the heading "Displacement" by ticking the "Show" radio button and scaling the displacement by a factor of -say- 20. The maximum displacement will now be exaggerated to approximately 20% of the box size. Upon closing the dialog window, the deformed mesh can be made visible again by highlighting the Result_mesh object and pressing the space bar.





Internal Boundary Conditions (Under Development)
Under Development