Finite Element Analysis

Finite Element Analysis is a computational method by which the internal strains of any body can be evaluated in a piecewise fashion to provide useful stress and deflection information. Commercially available FEA programs provide an easier interface by which to do the computations. ABAQUS and ANSYS are available on any CAEN computer. Before working through this tutorial (of sorts) you will need a reasonable understanding of ABAQUS. You may also want to talk with Professor El-Tawil, an expert on FEA and teacher of CEE 510.

Analysis Methods

An advantage of finite element analysis is that you can test your structure in just about any mode imaginable - granted, more creative models require a lot more work. I made the assumption that due to symmetrical loading all forces would act equal and opposite along the centerile of the canoe. Therefore, I could restrain this edge and not worry about having an unstable structure. This model is described in detail below. Note: After further evaluation, it turns out that this model us unrealistically conservative in computing deflections. See the report above for better techniques.

The best way to test model, however, would be through the use of fluid elements. You could model both the canoe and the water and just plop the canoe in. This requires an advanced knowledge of ABAQUS and extensive use of input files. Other loading patterns to consider include gravity loads while being transported or set on stands and the application of bending moments on the longitudinal axis. In each of these cases, the entire canoe could be considered.

Creating the Part

Begin with the canoe model in Rhino 3D. Delete any extraneous curves and surfaces leaving only the hull form polysurface. Draw a rectangular surface at the waterline and use this as a cutting surface to split the canoe into two polysurfaces. This will allow you to hydrostatically load only the portion of the canoe actually percieved to be below the water. Draw another surface perpendicular to the first along the centerline of the canoe. Use this surface to trim half of the canoe away. Delete the extra surfaces and export the two polysurfaces in *.iges format. Be carefull not to include extremely small surfaces in the canoe polysurface. This will be very hard to mesh in ABAQUS.

Open ABAQUS and load the part module. Import the *.iges file that you created for the split canoe. If ABAQUS finds any inconsistencies in your part, it will notify you and offer some help in seeking a remedy. Even if all problems cannot be resolved, you may still be able to perform an analysis. Carefully consider the validity of these results.

Next, open the property module. Try to make some reasonable assumptions about the Elastic Moduls and poisson's ratio of lightweight concrete. Since we're using an extremely lightweight experemental material, there will be very little evidence to support your arguement. ACI approximates Ec=57000*sqrt(f`c) -> f`c and Ec in psi. If you do a compression test you may be able to compute poisson's ratio as the ratio of transverse strain to longitudial strain. Compression testing, however, isn't really realevant to ferrocement because of the importance of the mesh layers.

Meshing

Meshing can be an art form. There are a wide variety of element types available in ABAQUS. For the canoe application, shell elements are most appropriate. These elemtents work well in 3D space and generally have fewer limitations than plate elements. When assigning the section type, you should pick a shell thickness roughly equivalent to the desired canoe thickness. This will assume plane strain (basically the whole thickness deforms as one but behaves as with its full size) behavior through the thickness. You can also choose between 4-node (linear order) and 8-node (quadratic order) nodes. Both element types should converge to the same answer for this application. 8-node elements provide additiona degrees of freedom by which each element may deform. These can be more computationally rigorous than the 4-node elements. I would recommend using 4-node elements with a finer mesh.

Assigning the mesh size is another art form. Meshes with more elements don't always produce better results. It's best to perform several computations and attempt to find a convergence pattern. More elements will also result in increased time necessary for computation. ABAQUS functions make meshing pretty easy. You may want to mesh one section at a time, however, so that the computer does not become overlaoded.

Loading

Because we've already cut the form along the waterline, adding a hydrostatic load is quite easy. In the load manager, choose to create a pressure. Select the side from which the water will act and then choose hydrostatic under the direction drop box. You'll also need to define the water pressure at depth and the location of the free surface. Loadings for the paddlers can be input as point loads or pressures anywhere in the canoe. Restrain the canoe along the entire centerline under the assumption that all force are acting equal and opposite on the other imaginary side.

Results

ABAQUS will present quite comprehensive results. It may take some time to feel your way around the layout. Using the Field Ouput option you can display bending stresses, defections, and internal forces. For whatever reason the connection to the UNIX server (on which ABAQUS is run) does not allow you to print from a PC. I recommend using cntrl-print screen to take a screen shot and then editing it paint.

The following picture was an early attempt to model the canoe. It is restrained at each end and loaded in the center. The units were not consistent accross the input fields so the distortion was severe. Also note that the front deforms through itself. Interaction conditions may be set so that these surfaces cannot move through one another.