A validated finite element analysis procedure for porous structures

• An accurate finite element analysis procedure is defined to model lattice structures. • Numerical and experimental results are in good agreement. • Accurate definition of the actual material is necessary to obtain reliable results. • Accurate representation of test conditions is necessary to obtain reliable results. ⁎ Corresponding author. E-mail address: sruiz@tecnun.es (S. Ruiz de Galarre https://doi.org/10.1016/j.matdes.2020.108546 0264-1275/© 2020 The Authors. Published by Elsevier Ltd a b s t r a c t a r t i c l e i n f o


H I G H L I G H T S
• An accurate finite element analysis procedure is defined to model lattice structures. • Numerical and experimental results are in good agreement. • Accurate definition of the actual material is necessary to obtain reliable results. • Accurate representation of test conditions is necessary to obtain reliable results.

G R A P H I C A L A B S T R A C T
a b s t r a c t a r t i c l e i n f o

Introduction
Due to developments in new manufacturing technologies such as additive manufacturing (AM), cellular materials are receiving considerably more attention as they can now be manufactured with a level of control not previously possible. Cellular materials also known as lattice structures are types of porous materials which are typically formed by a periodic or stochastic arrangement of beams/struts forming a threedimensional framework. They can also be made up of surfaces such as honeycombs or triply periodic structures. AM has increased the design freedom, the porosity control and the accuracy of these structures overcoming some limitations found during conventional manufacturing of these materials [1].
The superior specific stiffness and strength of lattice structures [2] make them ideal to design light-weight structures [3], additionally they possess good energy absorption and heat transfer capabilities and thus have many applications in industries such as aerospace, aeronautic and automotive. Their low mass, potentially low modulus and porous nature also make them suited for bone ingrowth applications for the biomedical industry, particularly in the field of orthopaedic implants [4]. Due to the diverse applications of lattice structures, there is significant interest in their mechanical behaviour and therefore numerous numerical and experimental studies have been carried out. The primary benefit of experimental testing is that the results reflect the actual behaviour of the material and are directly translatable to the real-world application. However, the down-side is often a limited design space and a large time and cost associated with manufacturing samples, removing them from the substrate, post-machining and finally testing. Whereas analytical models have the potential to explore a far greater design space in a potentially much cheaper and shorter period of time. Though some analytical models have been developed for unit cells such as bodycentered-cubic (BCC) [5,6], diamond [7], face-centered-cubic (FCC) [8] and rhombic dodecahedron [7,9], the mechanical properties of lattice structures are more commonly estimated by Finite Element Analysis (FEA). However, the FEA methodology used for lattice structures can differ greatly between studies.
Previous studies have analysed the mechanical behaviour of different lattice structures under compression by FEA and have compared it to experimental results, however, different approaches were followed regarding boundary conditions. Some researchers [10][11][12] directly apply a displacement to the top nodes of the structure while fixing the bottom nodes; whilst others introduce two shells in the FEA, representing the platens of the experimental compression test. In the latter works, some researchers consider a frictionless contact between the platens and the lattice [5,6,13,14] whilst others introduce a penalty factor to account for that friction [15][16][17] or even a bonded contact where sliding is not permitted [18]. Due to the computational cost, beam elements are desirable compared to 3D elements when modelling strut-based lattice structures, however there are again different methods followed when using beam elements. Some researchers model the struts with beams of constant cross section [7,10,19], while in other studies, to account for the higher material concentration around the strut junctions or nodes, the diameter is increased at the nodes by~20% [5,6,13] or 40% [20] or as in the case of Luxner et al. [21], the stiffness is increased 1000 times in nodal regions.
The material model is another key parameter that affects FEA results, and again various approaches have been followed. Plasticity is usually included in the material model by a number of methods: by an elastic-perfectly-plastic model (i.e. without accounting for the strain hardening) [22], by considering the strain hardening with a bilinear-elastic-plastic model [18], by directly using the material stress-strain data [13] or by using other models such as the Johnson-Cook model to evaluate damage [12,23]. To determine the material model, some studies use mechanical property data provided by the machine manufacturer or test tensile specimens from the bulk AM material [12][13][14]17,24,25], whilst other studies manufacture and test individual representative struts [6,16]. The advantage of the latter, is that the material model describes the behaviour of the strut including possible imperfections such as diameter deviations, surface roughness or internal micro-porosity. Some studies also physically model these types of imperfections [11,26] as well as other imperfections such as the fracture behaviour of struts [18] and strut 'waviness' [17]. In studies which have tested individual micro-struts [6,16,27] they have found modulus and strength values below that of the bulk material. However, it has not been shown yet how the material properties change as strut diameter increases or at what point it approaches that of the bulk material.
In most studies, FEA results are compared to experimental values, however the FEA methodology followed differs significantly amongst studies and often a systematic approach to developing the model is not described. It must also be noted that strut-based porous structures are often classified by their deformation mechanics. The structure is said to be 'bend-dominated' if struts bend or buckle during compressive loading; alternatively for certain porous structures it is possible for some struts to carry an axial tensile load during compression and these structures are classified as 'stretch-dominated.' It remains unclear how deformation mechanics and different types of cellular geometries will affect the convergence and accuracy of FE simulations. The main purpose of this work is to determine and provide a procedure to perform FEA of a periodic lattice structure under compression with accurate and reliable results when compared to physical mechanical testing at minimum computational cost. This will initially be done on bend-dominated structures, with the view that it can be applied to stretch-dominated structures, stochastic structures and graded structures. The following steps were performed: • Determine element size/type and the minimum # of unit cells required for both beam and 3D models to achieve convergence of mechanical properties.

Numerical modelling
As the method used to model compression tests by FEA has a significant influence on the results, prior to simulating the experimental tests, a sensitivity analysis of different methodologies was performed. All quasi-static simulations were performed using ABAQUS 2019/Standard software package (Dassault Systems). Two methods were used to model the lattice structures. For the first, an in-house code developed in MATLAB was used to model the struts with 3-node Timoshenko quadratic beam elements (B32). For the second, the lattice structures were designed in PTC CREO 5.0 (PTC Inc.) and meshed in ABAQUS with 3D quadratic tetrahedral elements (C3D10). A modified Face-Centred-Cubic (FCC) structure (all horizontal beams were removed) was used for the FE model development and validation (Fig. 1). Prior to simulation, a mesh size sensitivity analysis was carried out on both beam and tetrahedral elements. Following this, a convergence study was performed to determine the minimum number of unit cells required in each direction to obtain consistent elastic modulus and yield strength results. The results of the convergence study are presented in Section 3.1.
The FEA model is seen in Fig. 1, for all simulations two rigid shells models were placed at the top and bottom of the lattice structure, each having a reference point at their centre. The reference point of the lower shell was completely fixed, while the reference point of the upper plate was set to progressively deform the lattice structure until it yields (with strains ranging from 3% to 10% depending on the structure). For the solid FE models, symmetry is considered and only one quarter of the structure is studied, constraining the normal displacement of the symmetric faces (Fig. 1). The contact properties between the shells and the lattice structure were set to "hard" in the normal direction and frictionless in the tangential direction (except in 2.1.2). The bilinear elasto-plastic model shown in Table 2 and described in Section 2.2.5 was implemented in all the analyses (except in 2.1.3). Due to the small deformations self-contact between struts was not considered.
To calculate the elastic modulus and yield strength for each structure, the engineering stress-strain curves were derived from the FEA results. Stress was calculated by dividing the reaction force at the reference point of the top shell by the apparent cross-sectional area of the structure, whilst strain was determined by dividing the displacement of the top shell by the initial length of the structure. A regression analysis was performed in the linear region of the stress-strain curve to obtain the elastic modulus. Due to the lack of a distinct peak stress value, the yield strength was measured at a strain offset of 0.2%.

Lattice structure modelling sensitivity analysis
Due to computational cost, some studies use beam elements to model lattices. In most of these studies an increase of the strut diameter close to the nodes is applied to account for the material concentration and to avoid the lack of contact between struts, whilst in others a constant strut cross section is used. To analyse the sensitivity of the results to these approaches, three cases were studied for the FCC structure: struts with constant cross section and struts with an increased diameter in the node regions of 20% and 40% (Fig. 1). The length of the region where the diameter was increased was set to be equal to the strut radius. FCC structures of varying unit cell sizes and strut diameters were studied (Table 1). Identical structures were also modelled with 3D elements to compare the two modelling approaches. Note that length (l) in Table 1 is the length between two nodes and not the total length of the strut nor the unit cell length (Fig. 1).

Boundary conditions sensitivity analysis
To determine the mechanical properties of lattice structures from experimental compression tests, platens are usually lubricated to reduce the effect of friction on lateral deformation. This tangential friction is modelled in FEA with different values in the literature. To analyse its sensitivity on the results, five scenarios were studied: frictionless, friction coefficients equal to 0.1, 0.2 and 0.3 and bonded contact, i.e. no sliding permitted. These contact properties were applied to structure 10 (Table 1) meshed with solid 3D elements. When implementing friction in FEA simulations of lattice structures, the "barrel"-ing effect is observed due to the shear forces at the contact region. Consequently, this will have an influence on the results depending on the height of the structures and therefore the influence of the number of unit cells was studied again. To avoid a huge amount of 3D elements, the width of the FCC structure was set to 12 mm, i.e. 8 unit cells which is the minimum number recommended by Gibson and Ashby [28,29]. Then the number of unit cells in the height of the structure was investigated again, to ensure the stiffness and yield strength converged at minimal computational cost, for each of the five friction boundary conditions.

Material model sensitivity analysis
The material model has a significant influence on the results in FEA simulations. As discussed in Section 2.2.5, single struts of increasing diameter were tested in tension and stress-strain curves were obtained. Due to little variation between curves of different diameters, an average stress-strain curve of all the struts was produced. From this curve, two bilinear elasto-plastic models were derived (Section 3.3). In the first one (A) the yield strength is the intersection between the slopes of the initial stiffness and plastic hardening modulus. In the second one (B), the yield strength was set at an offset of 0.2% of the stress strain curve. These two models together with the actual stress-strain curve were used to model the material of structure 14 (Table 1) and the results were compared. Additionally, the same structure was modelled with the elasto-plastic model B derived from the stress-strain curves of strut 1 and 4 ( Table 2). These struts were chosen because they had the greatest yield strength and stiffness deviation from the average model.

FEA of the experimental structures
After the sensitivity analysis of the different variables and methodologies, FEA was performed on the FCC structures that were manufactured and tested experimentally. Strut diameter was taken from the physically manufactured specimens, as discussed in 2.2.3. The width/length of the designed structure was the same as the fabricated structures, while only 5 unit cells were modelled in the height to reduce the number of elements as discussed later in Section 3.2. The structures were meshed with quadratic tetrahedral elements. The average bilinear elasto-plastic model B described later in Section 3.3 was used to define the material for all the structures. A penalty factor equal to 0.1 was set in the tangential direction to account for the friction between the structures and the platens. To further investigate the accuracy of the developed FE methodology on other structures; modified octet-truss (OCT) specimens with all horizontal beams removed, were also simulated following the same procedure as above and were compared against experimentally tested specimens.

Specimen design and build file generation
Modified FCC porous specimens were designed in MATLAB (MathWorks Inc.). The structure was defined in a 7 column CSV (comma separated values) format, where each row reflects a single strut. The first 3 columns are the starting x, y & z co-ordinates of the strut, the following 3 columns are the end x, y & z co-ordinates of the strut and the final column is the diameter of the strut. Cuboid specimens were designed with one of two different unit cell sizes: either a 1.5 mm or 2.5 mm unit cell size. The test specimen size was 15 × 15 × 22.5 mm (10 × 10 × 15 unit cells) and 20 × 20 × 30 mm (8 × 8 × 12 unit cells) for the 1.5 mm and 2.5 mm unit cell size variants respectively. Ensuring there was a minimum of at least 8 unit cells in the length/width as per the recommendations of Gibson & Ashby [28,29] and a height of at least 1.5× the length/width (as per ISO 13314:2011). Modified OCT porous specimens, to further test the accuracy of the developed FE methodology, were also designed with a 1.5 mm unit size cell and specimen size of 15 × 15 × 22.5 mm (10 × 10 × 15 unit cells). To understand the material properties of the struts in the FCC and OCT specimens, 80 mm long single struts were designed at the same angle as are present in these structures (45°to the build plate) to be used for tensile testing.
An in-house developed piece of software was used to create slice data and thus generate build files (Fig. 2). For every strut, the software calculates the intersections between the strut and the slice layers. At each intersection a circle or ellipse is generated (based on the angle of the strut) at the specified size. Following Boolean union-ing of these contours on a layer-by-layer basis, the resulting geometries are placed into the file format required by the additive manufacturing system. Traditionally, the area enclosed by these contours are filled in with 'hatch' scans, however in this research, the diameter of the contour scan was set equal to the spot size of the laser (70 μm), this was to ensure it was possible to build small micro-struts and that there was no need for interpolative calculations to generate additional border or hatch scans, strut thickness was then controlled purely by the laser parameters. This method has been described and utilised previously in [30,31]. Laser parameters were assigned on a part-by-part basis. Previous work has established a relationship between strut diameter and laser parameter utilising the above method [31] and consequently for each unit cell size, specimens were built with 5 different strut diameters/laser parameters. Strut diameters were nominally in the range of 170-450 μm to produce relative densities of~2-20%, as described in Table 4. Single struts for tensile testing were built with all of the laser parameters used for the FCC and OCT structures.

Materials and manufacturing
A Renishaw AM250 metal powder bed fusion system was used to manufacture all specimens. The workings of the AM250 and the manufacturing process has been described in detail previously [30,31]. Specimens were manufactured from Stainless Steel 316 L powder (Carpenter Additive Ltd.) having a spherical shape with a particle size range of 10-45 μm (D 50 : 27 μm) and built onto mild steel substrates. The lattice structures were removed by electro discharge machining, ground parallel and cleaned ultrasonically in ethanol whilst the single struts were removed by pliers.

Morphological analysis
Overall structure relative density per unique specimen was measured by dry weighing in atmospheric conditions with n = 5 (i.e. repeated on 5 identical samples). Relative density was calculated by dividing actual weight by the theoretical weight of the macro volume using a density of 8.1 g/cm 3 . Overall dimensions of the structure were taken by a Vernier calliper. Each structure as well as the struts manufactured for tensile testing were imaged using a scanning electron microscope (Hitachi S-3400 N) and consequently strut thickness was measured utilising ImageJ in 20 locations and averaged.

Quasi static compression testing
Quasi-Static compression testing was performed on the lattices to ISO 13314:2011 using a material testing machine (Instron 8872) equipped with a 5 kN load-cell. Specimens were compressed at a constant rate of 2 mm/min. For a given unit cell size and strut diameter, a preliminary sample was compressed to 50% strain to estimate the plateau strength. The estimated plateau strength was the mean of the stresses between 20% and 30% strain (Fig. 3). To determine the elastic modulus and yield strength for a given unit cell size and strut diameter, samples (n = 5) were loaded to 50% strain with a hysteresis loop between 70% and 20% of the estimated plateau strength (Fig. 3) to account for the localized plasticity in porous materials which reduces the slope of the initial loading curve [28]. Displacement between the platens was measured at 30 Hz by two LVDTs (RDP D6/05000A) to reduce test-machine compliance errors. Strain was the average LVDT displacement divided by the specimen's initial height and stress (σ) was the measured load divided by the specimen's initial cross-sectional area (calculated from the initial length & width of the specimen). Stress-Strain curves were produced for each test; elastic modulus (E) was the linear regression of the hysteresis loop whilst the yield strength (σ y ) is determined as compressive stress at a plastic compressive strain of 1.0% relative to the elastic modulus (Fig. 3).

Single strut tensile testing
Tensile testing was performed using a materials testing machine (Instron 5570). The gauge length of the strut was 40 mm and was gripped over a 15 mm length either side (Fig. 4). The grips were additively manufactured and struts were sandwiched between one grip featuring a 90°'v-groove' and one flat grip. Grips with different depths of vgrooves were made to hold the struts of different diameters. Seven different strut diameters (ranging from 170 to 410 μm) were tested and for each diameter two specimens were tested. Displacement between the grips was measured at 30 Hz by two LVDTs (RDP D6/05000A) to get a more accurate measure of strain by reducing test-machine compliance errors (Fig. 4). The small diameter of the struts makes using a clip-on extensometer prohibitively difficult; the LVDTs were validated against a camera system with the benefit of being far faster in terms of data post-processing. Strain was the average LVDT displacement divided by the specimen's initial gauge length and stress (σ) was the measured load divided by the specimen's initial cross-sectional area (calculated from the strut diameter measured from SEM images). Stress-Strain curves were produced for each test; elastic modulus (E) was the linear regression of the initial loading curve whilst the yield strength (σ y ) is determined as compressive stress at a plastic compressive strain of 0.2% relative to the elastic modulus (Fig. 4).

Lattice structure modelling
For the FCC structure, six quadratic beam elements were found to be appropriate to model each strut, while for the solid mesh, element size ranging from 80 μm to 120 μm (depending on the strut diameter) resulted in the convergence of stiffness and yield strength. When modelling with beam elements, a structure of 14x14x14 unit cells saw convergence of the elastic modulus and yield strength (the difference with a structure of 16x16x16 was b1%). In contrast, for the 3D mesh, structures of 6x6x3 were found to be sufficient, especially when considering the computational cost (the difference with the 8x8x4 structure was b2.5%). It should be mentioned that increasing the height varies the results b1% and therefore the height was set to 3 unit cells to minimize the number of elements used. Also, if structures with large heightlength ratios were analysed, buckling effects would appear due to the slenderness of the structures affecting the mechanical properties. Element size and number of unit cells sensitivity analyses for the beam and solid mesh are illustrated in Fig. 5.
The elastic modulus and yield strength of the FCC structures displayed in Table 1 are illustrated in Fig. 6. When modelling the structure with beam elements, increasing the diameter in the nodal regions, results in an increase of both the elastic modulus and yield strength. When increasing the diameter 20% in the nodal regions, the elastic modulus and yield strength increases by 12.85% (3.27%) and 11.64% (3.18%) respectively, and 19.01% (4.90%) and 12.29% (3.51%) when increasing the diameter up to 40%. Fig. 7 shows the errors between the beam model with constant cross section and the 3D model. As it can be observed for small d/l ratios (or small relative densities) the errors in elastic modulus converge to 14% and therefore for d/l values below 0.06, the beam model approximation is acceptable. However, for larger d/l ratios the errors increase almost linearly making the difference between the beam model and 3D elements significant. A similar trend is observed with the beam models with a 20% and 40% diameter increase in the node regions, with errors converging to 6% and 2% respectively at small d/l ratios and increasing as the d/l ratio goes up. It is also seen that the error depends solely on the d/l ratio (i.e. relative density) rather than the unit cell size.   unit cells in the height is enough to reach convergence, however, when applying a friction coefficient of 0.3, 10-11 unit cells are required to reach convergence. For a bonded contact, the structure was modelled up to 13 unit cells in the height, but convergence was not achieved. Fig. 8 (right) illustrates the difference in the elastic modulus based on the different boundary conditions. When a frictionless contact is applied, the elastic modulus of the structure is 267.34 MPa, and as the friction coefficient is increased to 0.3, the elastic modulus rises to 327. 35 MPa, an increase of 22.5%. This difference would be even greater for the bonded contact.

Material model
The average diameter, elastic modulus, yield strength and ultimate strength values for each of the single struts are shown in Table 2.
As expected, due to irregularities in the manufacturing process such as internal porosity, diameter variation or semi-fused powder (Fig. 9), as well as due to the test conditions, variations in mechanical properties were observed for each strut diameter ( Table 2). The modulus of the struts varied between 68.9 and 98.8 GPa. These values are around 60% lower than the bulk material and within the range found in other studies [6,16].
As mentioned earlier, an average stress-strain curve was produced and consequently two bilinear elasto-plastic models were derived and shown in Table 3. These two models together with the stress-strain curve are illustrated in Fig. 10.
The effect of the material model on the FCC FEA results are seen in Fig. 11 (left). Results are very similar when defining the material either with the average stress-strain-curve of the struts or with elasto-plastic model B, where the structure's yield strength differs by 3.8%. However, when elasto-plastic model A is used, this difference increases to 15.6%. Strut 1 and 4, which have the greatest yield strength and stiffness deviation with respect to the average model, were also used to generate elasto-plastic models as per elasto-plastic model B generated from the average strut stress-strain curve. The difference in stiffness and yield strength between the material model of strut 1 and average material model is 5.8% and 5.2% respectively. This difference results in a variation of the lattice structure stiffness of 8.4% and yield strength of 4.9%. When using the material model of strut 4, which has a stiffness and yield strength difference of 13.2% and 1.8% with respect to the average material model, the lattice structure stiffness and yield strength consequently differ by 10.5% and 4.4%.

Compression test results
It was found that for a given laser parameter, strut thickness in the porous structure was slightly larger than when manufacturing single struts. The measured values are shown in Table 4. This is likely due to residual heat being present when manufacturing a porous structure where struts are in close proximity to each other rather than single struts placed far apart. When observing the manufactured lattice structures under SEM (Fig. 12), there is a clear difference in surface morphology between the upward facing surfaces (upskin) of the struts versus the downward facing surfaces (downskin). There also appears to be some mild thinning of some struts near intersections/nodes as well as distortion of nodes and strut 'waviness' is more apparent on thin long struts.
Regardless of unit cell size or strut thickness all porous structures displayed a ductile failure and similar failure modes/failure planes (Fig. 13).
The experimental results of the elastic modulus and yield strength for both structures are represented in Table 5 and illustrated in Fig. 14 for the FCC structure. Regardless of structure and unit cell size, both apparent modulus and yield strength vary by a power-law with respect to relative density as per Gibson and Ashby [29,32].  Table 6 illustrates the elastic modulus and yield strength of both the experimental compression tests and the FEA results. For the FCC, the average error between the experimental and FEA results for the elastic modulus and yield strength was 10.99% (6.91%) and 17.77% (15.26%), respectively. The maximum difference between the FEA and  the experiments for the elastic modulus and yield strength are 21.5% (FCC 8) and 42.2% (FCC 5), respectively. The FEA was also able to mimic the failure mechanics and yielding behaviour of the modified FCC structure (Fig. 13c).

FEA vs experiments
To further determine the accuracy of the FE approach, the OCT structure was numerically simulated as well as manufactured and tested experimentally. The average error between the FEA and experiments for the OCT structure was 8.50% (6.67%) and 17.02% (2.44%) for the elastic modulus and yield strength, respectively.

Discussion
This work has explored the various methodologies and variables necessary to build FEA models of lattice structures and has compared them to experimental compression testing for two different structures. The study highlights how modelling the appropriate number of unit cells, altering the boundary conditions or material model can drastically affect the outputs of the simulation. A systematic study of these variables is necessary to have confidence in the results and reliability of the simulation. The methodology presented in this work (Fig. 15) should provide a foundation to build future models for other lattice structures comprising non-stochastic or periodic unit cells as well as more complex structures such as functionally graded materials.
When working with lattice structures with large d/l ratios, a solid mesh is suggested. In this study it was found that for d/l ratios N0.1, the mechanical properties can differ by N20% between the solid 3D mesh and beam models. This difference seems to increase linearly with the d/l ratio. Whilst, these findings were obtained for the modified FCC unit cell, it should be seen whether the same is true for other unit cells. Although many lattice FEA studies consider a frictionless contact between the platens and samples [5,6,13,14], a barrelling effect was observed experimentally in the tested samples, indicating that friction was present. Whilst, other studies account for this friction in their models with friction coefficients equal to 0.2 [33,34], 0.9 [17] or even bonded contacts [11,18]. In this work it was observed that the difference in modulus between considering a frictionless contact and a friction coefficient of 0.2 is 16.5%, and 22.5% if considering a friction coefficient of 0.3. Altering the applied boundary condition will also change how many unit cells are necessary in the height to ensure convergence of the mechanical properties. In this work, the convergence for the bonded contact boundary condition was not achieved (a height of 13 unit cells was studied), but the trend indicates that the difference in the elastic modulus between a frictionless contact and a bonded contact is~50%.
It was found that defining the material model in FEA simulations with the bilinear elasto-plastic model B derived from the strut tensile tests was accurate. The procedure highlights that using the bulk material properties would not be accurate unless the actual strut geometry,  imperfections and deviations were modelled. Using the mechanical properties from tensile testing of an individual strut and modelling the struts at a constant diameter is simpler and consequently includes the imperfections in the model. Over the range of diameters tested in this study for stainless steel, the mechanical properties of the struts did not differ greatly with increasing strut diameter. When comparing FEA results using the average strut material model versus the mechanical properties from the strut with the greatest difference in properties (Strut 4), only resulted in differences in lattice structure modulus of 13.2%. Therefore, for stainless steel and for the range of strut diameters tested in this study, using an average material model rather that a structure/strut specific model can be considered as a good approximation. For both the FEA simulations and the experimental testing the relationship between modulus, yield strength and relative density followed models described by Gibson and Ashby [29,32] seen in Eqs. (1) and (2). Stress/Strength (σ) and modulus (E) increase with density (ρ) by a power law. This relationship was found to be true for AM structures by a number of authors [2,13,23,24,30,31] and can be seen in Fig. 14.
where σ 0 , ρ 0 and E 0 are the properties of the base material (i.e. solid stainless steel) and C, m and n are constants found experimentally. It is important to note these equations are only accurate to a relative density of 0.3 [29].When comparing the experimental results to the final FEA simulations differences in the moduli were on average (s.d.) 10.99% (6.91%) and 8.50% (6.67%) for the FCC and OCT structures respectively. There are however, a number of sources of error still likely present. As mentioned earlier, a barrelling effect was observed in the tested structures and therefore a friction coefficient of 0.1 was applied in the FEA. This value is likely close to reality when applying lubrication to the platens but needs further validation. Small errors when measuring the strut diameter would affect the 3D structure designed in PTC CREO. These errors would have more impact on the 1.5 unit cells as the variation in the relative density would be greater than in the 2.5 unit cells. Larger differences of on average~17% for each structure were seen in yield strength when comparing the experimental results to the FEA. Apart from the afore-mentioned sources of errors, it was observed that also using the elasto-plastic material model instead of the actual stress-strain curve of the material results in an increase of the yield strength in the FEA of around 4%. Yield strength can be overpredicted in FEA due to the idealised cylindrical shape of the struts. It is also clear from the SEM images that a number of structural irregularities are present such as strut waviness, non-idealised strut intersections/nodes, differences in surface morphology between upward and downward faces surfaces and crack initiation sites. There is also a limitation on measuring strut thickness from SEM images and not μCT scans as it assumes the cross-section is a perfect circle. At a 45°build angle and as multiple individual struts were measured with a low standard deviation it can be assumed the struts were quite cylindrical but it is possible with different diameters and build angles this may not always be the case. To combat this, μCT scanning of individual struts and lattice structures can better inform the shape and size of the struts. Finally, there is likely residual stress and a level of self-stress in the structure that is not accounted for in the FEA, possibly stress-relieving the specimens could reduce the errors found. The mismatch found in this work between the predicted FEA results and the experiments are acceptable and generally lower than found in literature. Table 7 displays the elastic modulus differences obtained in other works following various FE methodologies. Fig. 11. Stress-strain curves for the FCC structure comparing the elasto-plastic models with the actual stress-strain curve (left); and elasto-plastic model B derived from the average strut, strut 1 and strut 4, which deviate the most from the average strut stress-strain curve (right). The first four works displayed in Table 7 considered strut irregularities when modelling the lattice structure. In the recent work carried out by Lei et al. [33] all the structures were scanned by μCT to implement the actual irregularities in the FEA model, however the struts were modelled with beam elements and the structure had a small d/l ratio. In our work, it was found that modelling the lattice structure with beam elements instead of tetrahedral elements underestimates the apparent elastic modulus of the lattice structure for large d/l ratios and thus it is possible their methodology would produce larger errors for structures with greater d/l ratios. The error obtained by Kadkhodapour et al. [12] was 10% for a diamond unit cell and 63% for a cubic unit cell. Although strut irregularities are known to happen during the manufacturing process, in their work irregularities were not added to the model nor in the geometry nor in the material model. In the work by Smith et al. [5] the difference found in the elastic modulus was only 15%, in the range of this study. In Smith et al.'s work the material properties of stainless-steel were used and a reverse engineering method was used to find the effective diameter of the struts. In this reverse engineering method, the strut diameter was   varied until both the experiment and FE stress-strain curves coincided. This approach is performed for every model and strut diameter and has the drawback of experimental data being required.
The procedure described in this study, which gives accurate results, better represents reality by utilising the actual diameter and material properties measured from the struts. In this work two bending-dominated structures were studied and although one can expect similar results with other unit cell types, this should be studied in more detail before extrapolating the results. For instance, the results for stretch-dominated, stochastic or graded structures may differ due to the different deformation mechanisms. However, a similar procedure to the one described in this work can likely be followed to study these structures. In contrast, for triply periodic and surface based porous structures, more work should be performed in the future to define an accurate FEA procedure, particularly in defining the material model (as this study derived the material model from tensile testing of struts) and the minimum area to model. Future work should also look at studying the behaviour of the studied structures in other directions and under different load conditions such as shear or bending.

Conclusion
In this study a procedure to build and validate a finite-element model for additively manufactured metal lattice structures has been described. The results of the simulation were compared to experimental compression testing for a modified FCC and OCT lattice and showed good agreement (the average errors for the modulus and yield strength were 9-11% and 18% respectively) over a range of strut diameters (relative densities) and unit cell sizes whilst trying to minimize computational cost. It was also found that structure geometry can inform what modelling approach to use. When working with lattice structures with large d/l ratios, a solid mesh is suggested. For d/l ratios N0.1, the mechanical properties can differ by N20% between the solid 3D mesh and beam models. This difference seems to increase linearly with the d/l ratio. However, for small d/l ratios the beam model approximation can be appropriate. This study has also shown how boundary conditions can affect the minimum size of the structure that has to be modelled in order to achieve convergence. Finally, the study highlights how finite-element models of lattice structures are heavily dependent on the material model and boundary conditions and that accurate representation of the actual material and test conditions are necessary to obtain reliable results that can be used with confidence.

Declaration of competing interest
The authors declare that they have no known competing financial interests or personal relationships that could have appeared to influence the work reported in this paper.