The aim of this study is to evaluate and compare approaches to correlate the FDM parts analyzed in FEA with corresponding experimental results. A step by step approach is used in order to evaluate and compare these approaches. Suitable test geometries are printed using an FDM printer. These test specimens are tested on a tensile test bed to obtain the experimental results. The next step is to develop these geometries in CAD using as-built dimensions. The initial approach deals with generating an as-built CAD model of an FDM part which represents the part layer by layer as it is built, to replicate the microstructure, since FDM parts are non-homogeneous and not solid continuous bodies. Once an as-built model is created it is then simulated in a commercial FEA software using different approaches. The different approaches adopted are using isotropic, orthotropic and composite material models. These models are compared with the experimental results. An overview of the methodology, specimen development, comparison metrics and the process of the study is provided in the following subsections.
3.1 As-built Approach
An FDM part is manufactured in form of closely laid out filaments which gives it the fiber and layer microstructure. In order to accurately analyze these parts, it is necessary that they are correctly represented in simulations. The initial approach used in this study to develop a CAD model is to replicate the fiber structure so that we obtain an as-built CAD model. Once the part is printed, its CAD model was redesigned as an ‘as-built’ model using the G-code from slicer. A fiber-by-fiber and layer-by-layer model was created by tracing the G-code in Solidworks©. However, this approach led to meshing errors which are listed as follows:
- Some of the filaments intersected adjacent features (filaments), resulting in intersecting errors within the part, rendering the CAD model useless.
- The part with above errors eliminated caused meshing problems resulting from the misalignment of elements and nodes within the adjacent fibers in the CAD model.
- A large part file was generated which took nine hours to mesh and more than forty hours to analyze.
Therefore, this method to model FDM parts was time prohibitive, even when intersection and alignment issues were corrected for. Therefore, a simpler approach was used to model these parts; in which the 100% infill region was modeled as a solid continuous region, whereas, the regions with infill, were traced as they are built. This approach was used to develop the geometries used in this study.
This study only includes tensile tests for obtaining experimental results, therefore, the test specimen selected was a typical tensile test geometry i.e. the dogbone geometry. It has enlarged ends for gripping the specimen and a narrow middle section known as the gage section to ensure fracture is localized in the gage section only. This geometry was modeled in Solidworks©. The dogbone test specimens are designed similar to the specifications mentioned in ASTM D638. The maximum dimensions of the dogbone specimens (170×35×2 mm) were decided on basis of the print bed dimensions, the test bed dimensions and the grips of test frame. A general FDM part, unless otherwise specified, contains an infill pattern and thick perimeters in order to save material. Therefore, the dogbone geometries were designed to accommodate the infill patterns as well. The gage dimensions of the specimen were (50×20×2 mm) which ensured that enough features of the infill pattern were accommodated in the gage area. The infill patterns were constrained to the gage section so that the specimens would primarily elongate and fracture in the gage area. Therefore, the final test geometry had infill patterns with perimeters in the gage section and 100% elsewhere. Different types of infill patterns were used in study namely:
- Completely Continuous (C, CX, CY, CZ)
- Hexagonal Infill (HI)
- Circular Straight Infill (CS)
- Circular Packed Infill (CP)
- Linear Straight Infill (LS)
- Linear Crosshatch (LC)
- Hilbert Curve (HC)
- Infill-less (I)
- Corresponding Continuous (CC)
The corresponding continuous geometry has a continuous gage section such that it is equivalent in volume in the gage section with the infill pattern. This leads to a gage section with the same rectangular dimensions but with a lesser thickness. In addition to this a completely continuous (C) sample was also created which was used to derive the isotropic material properties in study. In order to derive the orthotropic material properties, the continuous samples were built in three mutually orthogonal directions: X, Y, and Z to obtain three sets of samples: CX, CY, and CZ. Figures 4 and 5 show the HI and CP samples. Rest of the samples can be found in Appendix A.
A number of assumptions that were made in the study have been stated below:
- Over the course of the study, different ABS spools were used for printing the test specimens. It is assumed that the material from the different spools is consistent with the material properties.
- The laboratory operation temperature was consistent throughout the study and therefore, the environment is not considered as a significant factor that affects the printing or testing.
- Any errors in clamping the specimens were considered to be randomly distributed.
3.4 Printer and printing parameters
Once a CAD model is created, it is converted into an STL file format for the slicing software to be prepared for printing. The slicing software creates a G-code file for the printer. The printer used for this study is MakerBot© Replicator 2X. The slicing software used was Slic3r©. However, in case of (C) specimens that were used to derive orthotropic material properties, ‘Simplify 3D©’ was used in order to specify the filament directions.
The printing parameters were kept as consistent as possible throughout the study. The printer’s heated bed temperature for all the specimens was 130º C. All the specimens were printed using white ABS with an extruder temperature of 230º C. The print parameters were finalized after a number of iterations that resulted in the most consistent specimens. The parts were printed without a raft or support. The circular specimens were printed with a layer height of 0.4 mm, whereas the rest of the specimens were printed with a 0.2 mm layer height. The specimens were printed with a 100% diagonal (45º/-45º) infill pattern in the solid region, since the infill pattern in the gage section was already modeled in CAD. The specimens used for deriving the material properties had the same print settings as those of the other geometries. The samples used for deriving the isotropic material properties were printed with a 100% diagonal (45º/-45º) infill pattern as well. In order to derive the orthotropic properties, the continuous sample was built in three mutually orthogonal directions with fibers in the longitudinal (0º) direction.
3.5 Tensile Tests
In order to compare the accuracy of finite element analyses experimental data was necessary. Therefore, tensile tests are conducted on all the samples. The tests were performed on ‘Modular under Microscope Mechanical Test System – μTS’ by Psylotech©. The test specimens were attached using clamping grips. A displacement controlled tensile test was performed at uniform rate of 50 µ/s. The test specifications were similar for all the specimens. The test software recorded the displacement at every time step and the force required to pull the test sample at that corresponding displacement. This data is further post processed to obtain stress and strain using the appropriate gage length dimensions. To ensure repeatability, a sample set of 20 specimens was used for each geometry.
The continuous samples were used to derive the mechanical properties for the study. For deriving the isotropic properties, the (C) sample was subjected to tensile tests. Stress values were calculated using force and cross-sectional area, whereas strain values were calculated using the displacement and the gage length. This stress-stain curve is used to calculate the elastic modulus which is used in simulations. Similarly, in order to derive the orthotropic properties, three sets of different test specimens were built in three mutually orthogonal directions. This enabled us to calculate the elastic moduli in each of the three orthogonal directions.
3.6 FEA Simulations
Each of the specimens were modeled in CAD as as-built models; any changes in dimensions after manufacturing the samples are taken into account. Further, the experimental tensile tests are simulated using these as-built CAD models in a commercial FEA software. Two FEA solvers are used: ANSYS© and Abaqus©. To simulate the tensile tests, a transient structural analysis is conducted on the as-built CAD models. A displacement controlled tensile test is setup wherein the displacement readings from the experiments are used as input displacements with one shoulder end fixed.
Four different FEA models are used; each one being more complex than the previous one to increase the fidelity of FEA model to the actual behavior. In the first model or approach, an isotropic material model is used for FEA. The material properties used are the material properties of homogeneous bulk ABS material . This model will be called the Bulk Isotropic Model (BIM). In the second approach, to increase the fidelity of FEA, derived properties of the continuous FDM samples (C) are used. These samples are used along with an isotropic material model. The elastic modulus is derived experimentally, and Poisson’s ratio is taken from engineering catalogs  due to lack of test equipment. This model is called as Derived Isotropic Model (DIM). Table 3 lists all the derived material properties.
To further take into consideration the anisotropy of FDM parts, an orthotropic material model was also applied. The elastic properties are derived experimentally using CX, CY and CZ samples and used along with an orthotropic material model. This approach is known as the Orthotropic Derived Model (ODM). The fourth approach uses a composite layup to define the finite element model. Since the FDM part is built in layers, a composite laminae approach may be better able to represent the behavior of FDM part. In this type of analysis, the part is divided into a set of plies or laminae, stacked together to form a composite part. This enables us to set fiber orientations in individual fiber lamina, so that the directional fiber layup can be accounted for in the model. This approach is called as Composite Lamina Model (CLM). Each of the as-built models are divided into a number of layers with each layer being as thick as the layer height of the part. The models built with 0.2 mm layer height have a ply thickness of 0.2 mm with 10 layers stacking up to the 2 mm height of the part. Similarly, 0.4 mm layer height parts have a ply thickness of 0.4 mm. The fiber directions are specified as 45º/-45º every alternate layers, just as the actual parts. The CLM is performed only in Abaqus©, since ANSYS© only permits shell models for composite analysis.
Since the infill patterns have intricate features with thin wall structures, a refined mesh is used. Quadratic tetrahedral elements are used in all of the specimens except CS and CP. A similar mesh is replicated in Abaqus©, so that the analysis from the solvers is comparable. Mesh convergence is performed to ensure appropriate suitable mesh density. However, with the CLM, a tetrahedral element mesh is not possible and therefore hexahedral brick elements were used. Normal stresses are calculated and are used as metrics for comparison with experimental and FEA results.