Comparison of FEA simulations and experimental results for as-built additively manufactured dogbone specimens

Parts built using fused deposition modeling (FDM—an additive manufacturing technology) differ from their design model in terms of their microstructure and material properties. These differences lead to a certain amount of ambiguity regarding the structure, strength, and stiffness of the final FDM part. Increasing use of FDM parts as end use products necessitates accurate simulations and analyses during part design. However, analysis methods such as finite element analysis, are used for analysis of continuum models, and may not accurately represent the non-continuous non-linear FDM parts. Therefore, it is necessary to determine the accuracy and precision of FEA for FDM parts. The goal of this study is to compare FEA simulations of the as-built geometries with the experimental tests of actual FDM parts. Dogbone geometries that include different infill patterns are tested under tensile loading and later simulated using FEA. This study found that FEA results are not always an accurate or reliable means of predicting FDM part behaviors.


Introduction
In the recent years, engineering and manufacturing sectors have shown an increasing interest in additive manufacturing (AM) or 3D printing as a means of manufacturing. From prototypes to functional parts, AM is increasingly being used in the development of new products. With AM, it is possible to develop geometrically complex parts with reduced effort, at the same time AM parts can also be customized for low volume production with economic feasibility.
AM collectively describes several processes including fused deposition modeling (FDM), stereo lithography (SLA), selective laser sintering (SLS), and others to build an object layer-by-layer. This study deals with models developed using FDM, which is based on the principal of material extrusion. The process begins in the software stage, where a CAD model of the object is created. Next, a slicing software mathematically slices the CAD model into layers and stores the information in a G-code format for the printer. The extruder of the 3D printer follows this G-code and builds the model from bottom-up by depositing material along geometry of the part on the printer bed. During deposition, the thermoplastic polymer filament is heated to a semi-molten state and feeding it through the extruder nozzle as shown in Fig. 1. This additive technique enables one to build complex geometries with relative ease, while eliminating the need for assembling complex parts from simple components. The FDM software defines a solid continuous model with an infill pattern with a sufficiently thick perimeter and a porous infill to save weight. With more research, these infill patterns can be used for function specific purposes as well.
The printing parameters significantly influence the part properties. Higher layer resolution, achieved by reducing layer height, produces a finer part finish at the cost of a longer printing time. Similarly, reduced filament extrusion diameters are better able to represent complex and fine patterns. Since the parts are built filament by filament and layer by layer, the microstructure is not identical to the original CAD design, due to the development of voids from imperfect bonding between adjacent filaments. Thus, the FDM parts are non-homogeneous, affecting the strength and other material properties of the part. These material properties are also dependent upon the printing parameters used for to print the part, including significant influences due to the layer orientation and the bonding between adjacent filaments. This leads to an anisotropic behavior of the FDM parts. Due to the nonhomogeneous and anisotropic nature of FDM parts, they deviate from their design in terms of their material properties and microstructure. Figure 2 represents a FDM part from a microstructure perspective. With more and more FDM parts being used as end use products, in performance critical applications, it is necessary to simulate and analyze these parts during design.
Finite element analysis (FEA) is a widely used analysis tool for the engineering analysis of structural, vibrational, and thermal problems. FEA is based on the finite element method (FEM) which is a numerical technique to find approximate solutions to boundary value problems for partial differential equations. In this method, a large body is divided into smaller entities known as finite elements, each represented mathematically by a set of equations. These set of equations representing the finite elements are then aggregated to form an assembly of equations that represents the larger body. Using methods from calculus, an approximate solution can be found [1]. Since FEA discretizes bodies into a continuum of finite elements to solve the problem, FEA is challenged to effectively represent the non-homogeneous FDM bodies. Due to the difficulties in representing the microstructure and constitutive material behavior of FDM parts, FEA may not be able to predict the actual behavior of FDM parts accurately. Thus, an FEA technique that accounts for these differences, between the ideal and actual conditions relating to anisotropy and microstructure, would be able to represent the behavior of FDM parts accurately. This gives rise to a need to link local structural and bonding differences to a global anisotropic material behavior, in order to develop an accurate FEA model [2]. It is therefore necessary to investigate whether FEA of FDM parts predicts their actual behavior.
In a simple FEA approach, an FDM part can be represented as a continuous part, with a linear isotropic material model. This would not be an ideal representation of FDM part behavior since FDM parts are neither homogeneous nor isotropic. Additional model complexity can be incorporated by using an orthotropic material model to take into account the anisotropy of FDM parts. In this study, the isotropic and orthotropic material properties are also derived experimentally to closely represent the FDM part behavior. Similar approaches are found in [3,4]. Furthermore, a composite material model along with a composite laminae setup is used in FEA with the idea that the layered microstructure of FDM parts can be represented as a composite layup. In addition, FDM parts in this study are modeled as they are built, i.e., fiber-by-fiber and layer-by-layer. This would enable us to represent the microstructure of the FDM parts accurately. The goal of this study is to compare the simulations of the FEA approaches mentioned above with actual experimental tests of FDM parts, by determining the ability of FEA simulations of as-built geometries in tensile loading, using experimentally derived material models, to predict actual behaviors of FDM parts.
In this study, suitable dogbone geometry patterns are designed for the comparison of FEA and experimental results. This geometry accommodates different infill patterns such that a typical FDM part with perimeter and an infill pattern can be replicated. These geometries are printed with ABS filament and eventually tested. The printing parameters used for the parts are consistent throughout the study due to a large number of potential parameters affecting the material properties. Therefore, results of the study stand true for parts built with these parameters.  Over the years, AM technology has developed tremendously. With decrease in printing time and increase in the ease of manufacturing complex parts, more and more parts are used as end use products. Similarly, FDM parts are being used in varied sectors like aerospace, automotive, industrial, and medical fields. It is possible to manufacture high end mechanically and thermally durable FDM parts with faster lead times, at the same time the process being feasible for low volume productions. Further information can be found in [5][6][7]. Before comparing the FDM part simulations with actual experiments, it is necessary to understand the effects of printing parameters on the FDM parts. In addition to this, the directions of fibers lead to anisotropy. Anisotropy, along with the microstructure, leads to the difference in behavior of the FDM parts as compared to homogeneous parts manufactured traditionally. It is also important to study the effect of printing parameters on the anisotropy and microstructure of the part. This would enable us to create parts with best possible finish and strength and enables us to keep the parameters consistent throughout the study.
Zieman et al. [17] and Upadhyay et al. [8] discuss the anisotropic properties of FDM parts. These studies derive various material properties by varying the fiber orientation within the test part. Es-Said et al. [9] present a comprehensive analysis of the effect of different layer orientation on the material properties of the part. The authors also go on to discuss the effect of various printing parameters on the quality and strength of the part. Similar studies document the effect of various process parameters on the structure and properties of the FDM parts. Table 1 lists and categorizes the literature according to the process parameters.
The important conclusions regarding the effect of each of the process parameters have been listed below: 1. Layer orientation: Longitudinal fiber orientation (0°) results in the strongest part followed by the "0°/90°," "45°/-45°", and 90°orientation in case of tensile tests [13].
2. Process temperatures (extruder and bed): That higher temperatures lead to a decrease in the percentage of non-filled area in the volume, indicating better bonding [10]. The bond quality is more affected by the extrusion temperature than the envelope temperature. The extruded filaments cannot be maintained at high temperatures long enough to enable complete bonding to occur between filaments. Therefore, finer control over the cooling conditions enables better bonding and eventually leads to better mechanical properties [11]. 3. Air gap: Smaller air gap between adjacent filaments yields stronger parts. With smaller air gap or even a negative air gap (fiber overlap) better bonding between fibers is achieved which leads to stronger parts [13,14]. 4. Layer thickness: A smaller layer thickness increases the quality and the finish of the part.
It is important to understand the material behavior of FDM parts to carry out an accurate FEA. The choice of the material model greatly affects the accuracy of the analysis, since the FDM material (ABS) exhibits isotropic behavior; however, the actual part exhibits anisotropic properties. Various authors have worked on analytically deriving stress values using different material models. This can be the initial analysis that would enable us to conduct a comprehensive FEA. Zou et al. [18] compare two types of material models: isotropic and transversely isotropic. Casavola et al. [19] talk about the mechanical behavior of FDM parts using the classical laminate theory (CLT). Orthotropic properties are derived using experimental procedures and are used to populate the CLT compliance matrix. Stress values are determined using a CLT compliance matrix and later compared with experimental results. The results from the CLT predictions are in accordance with the experimental values of stress for majority of the stress-strain curve; however, CLT results deviate close to 2% strain. Similar studies can be found in [20][21][22][23]. A summary of the literature can be found in Table 2.
Analytical approaches enable us to evaluate stresses only in continuous uniform areas. However, a comprehensive FEA is Some of the literature points out the need to represent the mesostructure of FDM parts to accurately analyze them. Cuan-Urquizo et al. [27] focus on mechanical characterization of lattice structure of FDM parts using simple elastic elements to represent the infill. Villalpando et al. [28] compare an FEA approach to experimental data, using models with parametric internal matrix structures under compressive loading. Rezayat et al. [29] and Garg et al. [30] also use a mesostructure approach to represent FDM parts. Since FDM parts are built in layers, it is hypothesized that a composite laminae approach of analysis would better represent the FDM parts. El-Gizawy et al. [31] present an integrated approach to characterize mechanical properties and internal structure of FDM parts and analyzes these using CLT. Martinez et al. [32] use a composite laminate layup using orthotropic properties in FEA using Abaqus© to predict the behavior of FDM parts. In a similar work, Sayre et al. [33] also present an FEA using two approaches: an isotropic model and a composite FE model. Even though the authors do not compare this with experimental results, the two approaches show considerable differences.
From the literature, it is evident that FEA results for FDM parts have not been consistent. It is evident that a detailed model that takes into account the microstructure and the anisotropy of FDM parts is required for precise and accurate analyses. FDM parts are usually complex with an integral infill pattern, and validating FEA approaches to accurately predict the FDM part behavior is necessary. Section 3 discusses the methodology used in this study; the FEA approaches adopted in this study and its comparison with experimental tests.

Methodology
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.

As-built approach
An FDM part is manufactured in form of closely laid out filaments which give 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 "asbuilt" 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: 1. Some of the filaments intersected adjacent features (filaments), resulting in intersecting errors within the part, rendering the CAD model useless. 2. 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. 3. A large part file was generated which took 9 h to mesh and more than 40 h 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.

Geometry
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 similarly 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: 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 3 and 4 show the HI and CP samples. Examples of all of the sample geometries can be found in Appendix A.

Assumptions
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.

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 130°C. All the specimens were printed using white ABS with an extruder temperature of 230°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 (45°/−45°) 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 (45°/−45°) 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 (0°) direction.

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.

FEA simulations
Each of the specimens was 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 [34]. 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 [35] 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 asbuilt models is divided into a number of layers with each layer 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.

Results
The printed geometries are shown in Fig. 3. The fractured geometries are shown in Fig. 5. The results of the material properties have already been mentioned in Table 3. The experimental stress vs strain values are plotted and used as reference. The stress values calculated for this comparison are stress values across the least cross-sectional area of each of the infill specimens. Similarly, the stress values at the same crosssection from each of the FEA simulations are also plotted. The stress-strain plots have been truncated to show only the elastic region, as a non-linear plastic analysis was not conducted. The FEA stress concentration plots were similar for all the models used with only the magnitude being different; hence, only a single stress plot per sample is shown. Also, the FEA results for a particular sample, results were similar from both ANSYS© and Abaqus©; hence, the ANSYS© results represent the FEA simulation results in the comparison. Separate results are plotted and presented wherever necessary.
The first specimen for discussion is the completely continuous (C) specimen. Figure 5 shows a stress-strain plot of the experimental and FEA results of (C) specimen. We can see a cone of results. The blue line shows the experimental results. We can see that BIM has overpredicted the results, whereas DIM has underpredicted the results. We see a slight improvement in the ODM results as compared to the DIM results. However, CIM results show no improvement over the results from ODM. Even though all the models showed large errors, BIM showed the least erroneous results with about 25% of error between the simulations and experimental results. From the FEA stress plot in Fig. 6, we can see that FEA predicted the highest stress concentrations in the gage section, which is where the actual part fractured. However, whether FEA can predict the zig-zag nature of the fracture is difficult to say without further analysis. Figure 7 shows the stress plot for the CP specimens. The blue line represents the experimental results. In this case, the BIM results, again, overpredicted the results and by a huge margin of about 50%. However, the DIM results, depicted by the yellow line, were very close to the experimental results showing about 3 to 10% errors which are acceptable results considering the fact that a non-homogeneous FDM part is analyzed. It is evident that the ODM stress results (from ANSYS©) were almost completely coincidental with the experimental results for majority of the stress-strain curve. It is important to note in this case that the ODM results from Abaqus© did not coincide but deviated by as much as 20%. Thus, we see a difference between the results from different solvers, with error between the solver results being more the error between simulation and experimental results. The CLM results deviated even more the DIM results. Also, the FEA stress plots showed high stress concentrations in the least cross-sectional areas, which is where they fractured. Figure 8 shows the comparison between the stress contour plot and the fracture pattern. Thus, in case of CP specimens, FEA accurately predicted the magnitude as well as the locations of stresses. The CS specimen results were similar to the CP specimens, i.e., the ODM and the DIM results were within acceptable deviations from the experimental results. However, the BIM model overpredicted by a large margin. Figure 9 shows the stress-strain plots for the experimental and FEA results, and Fig. 10 shows the comparison between the stress contour plot and the fracture pattern. In case of the I specimens, all the FEA models including the BIM underpredicted the results. However, BIM results were accurate with acceptable errors of about 5%. The models using derived properties, however, underpredicted by as much as 50%. The FEA stress plots shows the stress concentrations where the actual fracture occurred. Figure 11 shows a bar graph of stress results from experimental and finite element analyses for all the samples.
To visualize the stress value bars representing the different simulations for each of the specimen geometry, the bars are consistently ordered from left to right: bulk isotropic model, experimental results, derived isotropic model, orthotropic derived model, and the composite lamina model. The HC specimen was similar to the I specimen in the sense that the BIM results were closer than the results from using derived properties. In case of the HI specimen, all the models showed considerable differences in results. In case of both the linear samples, ODM results were the closest even though ODM under predicted by about 20 to 25%. The CHI specimen is the only case in which the CLM results were more accurate than the ODM results. The CLM results were almost completely coincidental throughout the stress-strain curve. FEA also predicted the stress concentration in the gage section which is where the samples fractured. However, whether or not FEA will be able to predict the diagonal nature of the fracture is difficult to state without further analyses. FEA stress plots in case of HI, LS, and LC specimens predicted the location of fracture; however, it was not exhaustive. FEA simulations were unable to predict the fracture in the infill region in case of HI, LS, and LC specimens, which is region that fractured first in experiments. On the contrary, these regions were shown as regions with least stress concentrations. Thus, we see ambiguity with the FEA results for different specimens.
Summarizing the observations, we can say that BIM generally overpredicted the results implying that the part is  Fig. 6 Stress plot for C: left-FEA contour plot, right-actual fractured part stronger than it actually was in physical tests. The BIM results showed deviations of up to 75% with respect to experimental results. However, for HC and I specimens, the BIM results had acceptable errors. BIM results were also more accurate than the rest of the models in case of these two specimens. On the other hand, the derived properties' models (DIM, ODM, and CLM) consistently underpredicted the results. The ODM predicted the results most accurately as compared to the other models. DIM results were within acceptable deviations in case of CP and CS specimens. Other specimens witnessed larger deviations ranging from 15 to 30% with the errors being as high as 50% in case of HC and I specimens. It is important to note that, ODM results proved only a slight improvement over the DIM results, despite increased computational costs. This is due to the fact that the specimens have been analyzed only for uniaxial tensile tests (in x direction). Therefore, even the orthotropic analyses are primarily governed by the elastic modulus in x direction. Recalling the values from Table 3, E x = 1.1 GPa and E = 1 GPa (elastic modulus for the isotropic model), the slight difference in the elastic moduli from the two sample resulted in only a slight improvement of results even when an orthotropic material model was used. However, in case of a more complex, multi-directional loading, the orthotropic model might show considerable improvement as compared to the isotropic model. We also observed difference in results of different solvers in case of certain specimens. The more detailed CLM showed no improvement in the results as compared to the ODM. The only specimen for which the CLM results were better than the ODM results was the CHI specimen. For the rest of the specimens, the ODM results were more accurate than their CLM counterparts. In addition to this, CLM analysis showed large deformations in certain cases (LS and LC) which can be attributed to element meshing errors. Another explanation for CLM showing inferior results can be the type of analysis, since in case of CLM, each layer is considered as a 2D lamina or a planar surface and meshed with an element thickness. In case of ODM analyses, the model is considered as a solid model with orthotropic material properties and assigned a particular material orientation, which is a more accurate representation of the structure. Laminar theory also assumes perfect bonding between each layer of composite; however, this is not the case in actual scenario and can be a reason for the divergence from experimental data. CLM also takes a longer time to complete the analysis as compared to ODM and other models yet fails to predict the results as accurately as ODM. Therefore, using a composite model for analyzing FDM parts under tensile loading is not recommended or not necessary. The stress plots of a particular geometry for the different models were very similar, with only magnitude being the difference. FEA models were accurately able to predict the stress locations in most cases. However, it did not predict all the fracture locations in certain cases like the HI, LC, and LS specimens (FEA failed to show the fracture in the infill regions was).
Thus, we see that FEA results were highly accurate in certain cases, and in other cases, showed large deviations in results as compared to the experimental results. We observe that a given FEA model predicts the same test differently, and hence there is no certainty to propose a correction factor for these errors. The accuracy of the results is different with different geometries. The positive as well as negative deviations from the experimental results renders us to state that FEA is unreliable to predict the analysis of FDM parts in tensile loading. In the next section, we discuss the conclusion and state the scope for future research.

Conclusion
A comparative study of the FEA simulations and experimental tests was performed using specimens with different infill geometries. The use of different infill geometries alters the time between the printing of adjacent fibers in both the intralayer and interlayer situations. Due to changes in the timing between the printing of adjacent layers, we see differences in the bond strengths achieved between adjacent fibers (intralayer bonding) and between fibers in subsequent layers (interlayer bonding). Consequently, FEA models using material properties derived from bulk properties are unreliable predictors of the strength of FDM parts due to anisotropic behaviors in the printed parts. Furthermore, replacing the bulk material models with experimentally derived models of additively manufactured parts did not lead to an appreciable improvement in FEA model performance. In some cases, the experimental models proved to be acceptable, but in other cases, substantial errors were observed. The variable performance appears to be attributable to the particular infill pattern used with respect to the tensile loading. Thus, we conclude that the printed geometry of the part also affects the behavior of the part.
Further experimental efforts with an orthotropic-derived material model (ODM) that better accounts for the differences in fiber orientation by accounting for intralayer versus interlayer bonding strengths between adjacent fibers did produce better and more consistent FEA results, but incurs additional computational costs.
A different material modeling approach employing CLM was also applied, but these models did not better the results as compared to the orthotropic model. Furthermore, the CLM results were generally inferior to the ODM results and CLM analyses produced increasing meshing errors, large deformations and consistently required significantly longer analysis time as compared to the ODM analyses. Therefore, there is no need to resort to a complex composite model while analyzing FDM parts. It can be concluded that, from the four models used, the higher fidelity orthotropic material model (ODM) best represents the non-isotropic FDM parts.
From this study, we conclude that FEA results demonstrate that there are both non-homogeneous, anisotropic, and manufacturing parameters that must be accounted for when developing an FEA simulation. Therefore, FEA is an unreliable predictor of the behavior of the FDM parts without adequate knowledge of the influence of these parameters. For different modeling approaches, FEA models may overpredict or underpredict the behavior of the actual FDM parts. This uncertainty in the result should be sufficient that FEA results of FDM parts may not be adequate for demanding applications.
Further, the results appear to be increasingly unreliable as the number of fibers within the cross-section of the part becomes smaller. This is particularly concerning as the goal of minimizing printing time, part mass, and manufacturing costs often drive part designs to minimize the number of fibers included in a cross-section. Larger cross-sections with many fibers to provide additional intra-and inter-layer bonding locations and thus appear to behave much more like isotropic bulk material specimens. Structures with few fibers in their cross-sections produced the least reliable FEA predictions.
Furthermore, analysis of the predicted failure locations within the samples also was not reliable. Some specimens were accurately predicted, while others were not. In general, it appears that as the infill geometry becomes more complex, and therefore as the fiber patterns become more significant in the analysis that FEA is less able to predict the behaviors of the parts.
Finally, the magnitude of the prediction errors varied not only with material model but also with the infill geometry itself. This pattern clearly suggests that not only are the intra-and inter-layer bonding behaviors, as well as the relationship between fiber size and part cross-sectional area, important to the accurate analysis of FDM parts, but also the actual infill geometries and printing process play a role as well. The digital heritage of FDM parts as opposed to the continuous nature of traditionally manufactured parts proves to be challenging to existing FEA modeling approaches.

Future scope
This research provides a significant contribution by demonstrating that the nonlinear anisotropic material properties as well as the discontinuous nature of FDM parts produces significant reliability considerations for the design of FDM parts. Further experimental work should be conducted to examine these behaviors not only in tensile testing, but in other uni-and multi-axial load conditions, as well as to examine the effect of the additive manufacture process selected for part production. The authors believe that not only the FDM process suffers from intra-and inter-layer bonding effects but also suspect that other additive manufacturing processes will generate similar effects. In addition, these research results suggest that alternatives to FEA modeling of additively manufactured parts should be developed. The data from this research indicates that there are material anisotropic effects, geometric effects, and manufacturing toolpath effects that affect the ultimate material properties of the parts. A model formulation such as that made possible with discrete element methods (DEM) may yield results that have more reliable predictive value. DEM is a numerical approximation method for mechanics of continuous and discontinuous models, which is based on an interacting system of particles [36]. The material is modeled as an assembly of rigid particles and the interaction between each particle is explicitly considered to evaluate the stress-strain results. Steuben et al. [36] discuss a discrete element method to analyze the particle based AM methods. Such a system of discrete rigid particles might be better able to link the material model and the toolpath dependencies associated with an FDM part.
There is a clear need to investigate and develop better technologies to better represent the microstructural and material behavior of FDM (eventually AM) parts. With the increasing use of AM parts for functional applications, research regarding simulating these parts under the actual loading condition is necessary.