Additive Manufacturing Part Level DistortionSensitivity Analysis within Abaqus on a Thinwalled, Tubular StructureRichard A. DeeringThe Kansas City National Security Campus is operated by Honeywell Federal Manufacturing &Technologies, LLC for the United States Department of Energy under Contract No. DENA0002839Abstract: As additive manufacturing (AM) evolves to become a more viable production solution interms of cost, quality, and time, the need for predictive simulation of the process grows as well.After testing several commercial offerings to see how well they could predict deformation ofvarious parts, Abaqus was found to be the most promising option and chosen for a more in depthanalysis. The scope of this particular project was to examine the effects of certain simulationchoices – from basics (mesh, time stepping, element type) to unique AM convergence techniques(full/partial activation, expansion time constant, follow deformation, etc.). Hundreds ofsimulations were run in Abaqus with various permutations and the resulting response on the finaldeformation and stress state was tracked. The results will be presented with charts and images toshowcase the patterns (or lack thereof) produced by isolating each of these modeling choices on athin-walled, tubular structure. The findings and conclusions are of value to anyone using Abaqusto simulate part-level distortion due to AM: for some – the study can provide a model or launchingpoint for other in-depth sensitivity studies, for others – confidence in established procedures, orothers still – insight to the myriad of options available with Abaqus’s AM capabilities.Keywords: Coupled Analysis, Heat Transfer, Postprocessing, Residual Stress, Scripting, ThermalStress, Tube, Visualization, Additive Manufactuing, AM, Thin-Wall, Distortion, DOE, Design ofExperiments, Abaqus/CAE, Element Activation, Expansion Time Constant1. IntroductionAdditive manufacturing (AM) is an evolving technology for fabricating products. Theterm AM is a broad envelope encompassing many specific processes each centered on the idea ofbuilding a part from the bottom up using a series of layers. All of these methods eliminate manyof the constraints of traditional manufacturing methods by allowing for nearly limitless designopportunities. With additive, one can print entire assemblies rather than dozens of piece parts,manufacture organic, complex shapes, or manipulate build parameters to create gradient strengthparts.The specific process of interest for this paper is powder bed fusion (PBF). PBF is acommon industrial process used to additively manufacture metal parts. The process entails1

spreading a layer of metal powder over a bed. Then, a laser (or some other energy source)selectively melts regions of the powder that comprise the part. The regions are essentially crosssections of the part, created and fed into the machine such that there is a cross-section for everypowder layer within the build. This spreading and melting procedure is then repeated until all ofthe cross-sections of the part are printed. The end result is a fully dense, bulk part.A common issue inherent to PBF is that thermal gradients throughout the course of thebuild begin to induce significant residual stress within the manufactured parts. At best, thesestresses tend to warp the parts and can produce out of tolerance product. At worst, these stressescan fracture the part during the build and interfere with the recoater blade crashing the entire build.Typically, reducing excessive distortion requires manual trial and error consisting of repositioningthe part, changing support structure strategies, or modifying machine parameter settings. This is alabor intensive approach which delays schedules and can cost thousands of dollars per build.Avoidance of these failed builds could save a company both time and money while alsoaccelerating the adoption of AM. As AM has gained more widespread traction, a dozen or socommercial simulation suites have begun to come out with specific offerings for AM. Each ofthese codes can fall into two main simulation categories – inherent strain method or transientthermo-mechanical method (TTMM). Both of these methods operate similarly by creating amesh, partitioning the part into layers, then activating elements on a layer-by-layer basis andapplying strain to the active layer. These strains are then resolved to predict the bulk distortion ofthe part. The main difference in the methods is how the applied strains are obtained. In inherentstrain, the strain is predefined and exactly the same for each element making this methoddrastically faster, but potentially sacrificing accuracy. In TTMM, the applied strains are truethermal strains obtained by resolving the scan paths of the machine within a thermal model andfeeding them into the mechanical model. These models are slower, but more closely mimic thephysics.Recently, Abaqus has released simulation capabilities to predict part-level distortionduring additive manufacturing. They developed an entirely new framework to handle the manylaser-mesh intersections. This framework allows the simulation to fully capture the provided scanpath at whatever temporal or physical resolution is desired. It is a full transient thermomechanical model with a sequential, one-way coupling. First, a pure heat transfer simulation isrun. This resolves the temperature history of the part which is then fed into a mechanical model asa predefined field. Then, the mechanical model runs to calculate (and resolve) the thermal strainassociated with the temperature states. The output is a prediction of both deformation and stress.2. PurposeThe purpose of this study is to examine this new simulation methodology and documentthe effects of various simulation choices on the outputs of interest – maximum displacement,maximum stress, maximum temperature, and runtime. This is important to understand howsensitive the solution is and what precautions must be taken during setup to ensure accurate,meaningful results. The study will also highlight useful convergence techniques and whichparameter sets are most robust and accurate.2

The study will consist of running a full factorial DOE changing 6 different aspects thatARE NOT APPLICATION SPECIFIC. The factors chosen are all more closely related tomathematical formulation and solution of the problem rather than constraints/boundary conditionsdictated by the physical system. As such, factors important to accurately represent the real world machine temperature, scan paths, cooling effects, material properties, etc. - while important, werecalibrated once beforehand and then held constant for all of the runs within the study.3. Model SetupThe geometry used for the study is essentially a thin-walled, constant cross-section tube witha bend near the top of the part. It consists of two flat vertical walls and a hemisphere on either endconnecting the two. Then, near the top of the tube, the opening curves at approximately a 45oangle. The change adds a bit more complexity and demonstrates the maximum possible deviationof the wall without requiring supports. The baseplate (12.5mm thick, stainless steel) wasexplicitly modeled. All units were consistent with mmNS unit system. See figure 1 below.Figure 1. Thin-walled geometry3

This geometry was chosen as a representative test piece because the most problematicparts to produce are thin walled structures. These structures are much less rigid and thus distortsignificantly more than bulkier components. Therefore, this class of thin-walled parts offers thebest potential return on investment and is an ideal candidate for simulation. The size was chosensuch that many of the parts could be built on a single build plate with the entire build taking lessthan a day. Many of these parts were manufactured and measured and so a plethora of data existswith which to compare the simulation predictions.Physical parts were manufactured on a Renishaw AM250 machine as well as ConceptLaser M-Lab using 316 stainless steel powder. The machine parameters were constant for allbuilds and were similar to preset strategies. While still attached to the build plate, these parts wereblue-light scanned. This scanning procedure produced an .STL file which was then overlaid ontothe nominal CAD geometry, through GOM Inspect (free), to visualize the deformation due toprinting. See figure 2 below.Figure 2. Baseline model comparison (equivalent scales [-0.4 mm to 0.4 mm])Left: Measured front/back of physical part via blue light scan and GOM InspectRight: Predicted front/back displacement from Abaqus AM simulationThe base simulation model was created entirely within Abaqus/CAE (v2017.HF5) usingthe additive manufacturing plugin. The part was tied to the baseplate during both the heat transferand static runs. This model was then run with defaults to validate some of our baseline boundaryconditions. This serves to ensure the application specific assumptions which will be held constantfor the study are adequate and predict a reasonable deformation profile and magnitude.The following aspects are known to be important in simulation of AM, but were notvaried in the study:1.2.Absorption Coefficient – .68 based on the emissivity of stainless steelMaterial properties – Temperature Dependent 316 Stainless Steel. See figure 3 below.4

Figure 3. Abaqus Material Model3.4.5.6.Scan Strategy – Scan Path and Screed Path, see belowInitial Temperature – 200oC based on early runs, calibrated valueBuild Temperature – 26oC room temperature build, no preheatCooling during builda. Convection - .018 mW/mm-oC to temperature of 26oCb. Radiation - .25 emissivity to temperature of 26oCc. Both values were taken from Abaqus’s suggested parameters, no calibrationMost of the above conditions are easy to come by from either the physical build setup orstandard material properties. The only additional boundary condition is applied to the bottom faceof the build plate. In the heat transfer run, this face has a prescribed temperature of 26 oC; in thestatic run, the face is constrained in all degrees of freedom.One of the factors that has a large impact on displacement is the chosen “initialtemperature” boundary condition. This is the reference temperature that thermal strain iscalculated from. This value can have a large impact on both the magnitude of predicteddisplacement as well as the specific deformation profile. For these runs, a ballpark value was5

chosen by running a simulation using a medium mesh (.2), medium timestep (25), C3D8Ielements, and the default settings from the plugin (partial activation, follow def NO, expansiontime constant 0). The value was incremented by 25o C until the deformation seen was the sameorder of magnitude as observed in the physical part. Studies explicitly looking at this initialtemperature with a couple different geometries have since been performed and a more true valueseems to be 300-375oC (cooling to 80oC build temperature). However the specific initialtemperature value does not change the trends observed within this study. The value simply shiftsthe predicted displacement.The scan path was not able to be obtained directly from the AM machine so a mock scanpath was used. This mock path aimed to mimic the actual scan path as close as possible. It wasgenerated through a series of scripts using Cura (free FDM software). The Cura framework wasused with a modified “extruder” to replicate the same laser spot size and hatch spacing. The layerby-layer rotation angle was also modified to more accurately capture the actual process. A portionof the path can be seen in figure 4.Figure 4. Scan path generation within Cura4. DOE DesignOnce the baseline runs were calibrated and the input decks worked as expected, the DOE runswere generated via python scripts to produce a full-factorial DOE with 6 different factors:1.Follow deformation (2 levels)6

a. determines whether or not the inactivated elements are allowed to moveand follow the predicted deformation of the partb. Tested values – YES, NOMesh density (3 levels)a. Determines the dimensional resolution of the partb. Mesh was controlled by a global seed size. This seed size was picked such thatthe finest mesh had 3 elements through the wall thickness and the coarsest meshhad only 1c. Tested values - .1333, .2, .3 (1.5x factor between seed values)Time step (4 levels)a. Determines the temporal resolution of the part, direct specificationb. Time step was chosen so the finest resolution was approximately the time tobuild 1 physical build layer ( 9sec/layer for the constant cross section, 8secdwell)c. Tested values – 12.5, 25, 50, 100 (2x factor between each time step)Expansion Time Constant (3 levels)a. Determines the amount of time over which induced thermal strains are appliedb. Tested values – 0*time step, 2*time step, 5*time stepActivation Method (2 levels)a. Defines how elements get activatedb. Tested values – Full, PartialElement Type (3 levels)a. Hex (reduced integration and incompatible modes) vs. Tetb. Tested values – C3D8R, C3D8I, C3D4Again, these factors were chosen due to the fact that they are not dictated by the physicalbuilds or machine settings. Each of them are choices the simulation engineer must make for anyAM job run within Abaqus. Understanding how these choices affect the outputs will allow theanalyst to make appropriate choices and inform them of the risks of varying certain parameters.The intent was for each of these runs to be solved on an HPC cluster using 8 CPUs. Dueto runtime concerns, the fine mesh runs were instead run on 128 CPUs. All of the submittals weredone in two job batches to ensure that the heat transfer fully completed before the static initiated.Bash scripts handled the creation of subfolders, running of jobs, monitoring of jobs, transfer ofresults, and deletion of excess files (especially the large heat transfer .odbs).Analysis of output was done via python scripts. The scripts would open the static .odbfile and record the status of the job (Failed/Completed if failed then at what time it failed), themaximum stress and the maximum displacement at the final frame, the temperature at t 5150(arbitrarily chosen time during the constant cross-section portion of the build). It would also takea series of snapshots of each of these quantities. Runtime was pulled from the .msg files. All ofthis data was then exported to a .csv file that could be viewed in Excel or Minitab.7

5. ResultsThe following result plots were produced in Minitab using a subset of the data indicatedin the DOE design. First, resource limitations prevented the running of every finest mesh size soall of those runs have been removed from the analysis. Additionally, the C3D8R runs were allremoved due to the vast majority of the coarse mesh runs failing; these failures occurred early inthe run and the corresponding stress and displacement values are drastically low. Finally, onlyruns with follow deformation NO were used. Follow deformation YES resulted in severaladditional failed runs, which is undesirable. Since follow deformation NO produces less failedsimulations it makes sense to isolate those runs. This is especially helpful considering that havingboth simply obfuscates the overall data by averaging follow deformation YES’s drastically highervalues with the lower values of follow deformation NO. See figure 5 below.Figure 5. Effects for follow deformation NO only (left) vs. Effects when also including followdeformation YES results (right)There are two different plots for each output variable of interest. First, the “main effectsplot” which indicated the effects that each of the individual factors had on the output. The slopeof the lines denotes the severity of the effect; the steeper the line, the larger an impact that factorhad. The second plot is an “interaction plot”. Within these plots, each section represents a certaincombination of factors. The main indicator of an interaction between the two factors listed is nonparallel lines. Parallel lines indicate that the combination is insignificant whereas non-parallellines mean that the specific combination has a significant impact on the result. All of the plots areincluded as is so that the reader can make their own conclusions. After the plots, noteworthytakeaways are compiled along with any observations that may explain the stated behavior.5.1TemperatureHigh-Impact Factors: Mesh size, time step, element type, and activation schemeNon-Impact Factors: Expansion time constantRange: 26.06-28.39oC8

Figure 6. Minitab factorial plots for temperatureTemperature results were as expected. The main effects in order of impact were meshsize, time step, element type, and activation. Expansion time constant was the only factor that hadno impact on temperature; which is to be expected as it is present in only the static analysis.Essentially as the simulation became more refined spatially and temporally, the temperatures rose.The smaller time steps and mesh sizes resulted in higher temperatures as did the smaller elementtype (tets) and sub-sectioning the element through partial activation. However, the total range oftemperature values were 26.06-28.39oC. All of these simulation choices had very minor effects onthe magnitude; essentially in all cases, the activated elements were contracting from their initialtemp (200oC) to room temperature (26oC) in a single time step. Partial activation appeared to bemore sensitive to mesh size than full activation which was mostly driven by the fine mesh andfiner time steps; at the coarse end of the spectrum both activation schemes produced similar9

results. Additionally C3D8I elements were very sensitive to changes in mesh, whereas C3D4elements were not. This is most likely due to the fact that with 2 elements through the thickness,there is now a node in the middle of the wall which takes longer to cool than both of the exteriornodes present with only 1 element through the thickness. With a tet mesh, there already existssome interior nodes even for the largest mesh seed.5.2Maximum StressHigh-Impact Factors: Activation scheme, element type, and mesh densityNon-Impact Factors: Expansion time constantRange: 956- 2815MPaFigure 7. Minitab factorial plots for stress10

With the temperatures from the heat transfer run not varying drastically, one wouldexpect to see similar results for both stress and displacement as the driving force for the staticanalysis is the output of the heat transfer. However, even with such seemingly tiny changes, thepredicted maximum stress varied from 956- 2815MPa. The main effects in order of impact wereactivation scheme, element type, and mesh density. Expansion time constant had no effect whenthe value was 0 or 2, but showed a drastic decrease at 5. This would suggest that 5 is too great avalue which was especially apparent for the higher time steps. Additionally, activation schemeshad a drastic effect on both time step and element type. When choosing full activation, there ismore uncertainty between the results of the tet and hex mesh than the partial activation runs. Asfor time step, the activation scheme chosen dictates the trend of the stress values as the time stepbecomes finer. The stress increases using full activation and decreases when using partialactivation. It is uncertain why this is and could be the reason why overall time step does not havea clear trend in terms of maximum stress predictions.5.3Maximum DisplacementHigh-Impact Factors: Activation scheme, element type, and mesh densityNon-Impact Factors: Expansion time constantRange: .22-.66mm11

Figure 8. Minitab factorial plots for displacementMaximum displacement follow all of the same overall patterns as stress, which is to beexpected. The main effects, again, in order of impact, were activation scheme, element type, andmesh density. The individual values ranged between .22-.66mm. Expansion time constant had noimpact when the value was 0 or 2, but showed an even more drastic decrease at 5 which furthercements the higher values as being undesirable. In addition, the 100 second time stepping showednotably lower values for both meshes which may suggest the temporal resolution is too coarse.The activation scheme chosen dictates the trend of the displacement values as the time stepbecomes finer. The distortion increases using full activation and decreases when using partialactivation which mimics the same behavior shown in the stress. Also, choosing full activationexacerbates the impact of higher value expansion time coefficients. Hex mesh appears to beslightly more resilient to changes in time steps.12

5.4RuntimeHigh-Impact Factors: Time stepping, mesh, and element typeNon-Impact Factors: Expansion time constant, activation schemeRange: 21min – 35hrsFigure 9. Minitab factorial plots for runtimeMost of the runtime results are rather trivial. Runtime is dictated primarily by timestepping, mesh, and element type. This is exactly as one would expect. Each of the simulationsused 8 CPUs and thus the more elements present either with a finer mesh or choosing tets overhexes results in a slower solution time. Likewise, the number of increments that must be solved13

which is dictated by the time step will increase the runtime. The noteworthy insights were of theaspects that did not change the runtime. The activation scheme did not have an impact. Bothpartial and full activation averaged about the same runtime. The same can be said for expansiontime constant. There was no notable gain in runtime by using a larger expansion time coefficient.6. ConclusionOverall, Abaqus is capable of replicating the same deformation profiles seen in physicalbuilds of thin walled specimens. However, the simulation choices that an analyst makes do have adrastic impact on the overall prediction. The choice of allowing follow deformation in particularis crucial. Follow deformation YES does improve convergence in some cases (such as whenusing coarsely meshed reduced integration elements), but usually allows far too much distortion,ultimately making the solution meaningless. It is also more costly in terms of runtime. Meshdensity did not have as large of an effect as predicted, but the predicted displacement doesincrease almost uniformly as mesh density increases (for the 3 seed sizes indicated in the DOE).Time stepping had a non-linear impact on many of the results of interest including displacement.100 seconds ( 6 physical build layers) seemed to be too coarse and 12.5 seconds ( 1 physicalbuild layer) seemed needlessly fine. Somewhere between seemed adequate in terms of accuracyand runtime. It did not show a large dependence on mesh density either; the two are fairlyindependent. Element type is as important in AM as it is in other analysis types. For thin walledstructures incompatible mode hexes were about 2x as expensive in terms of runtime, but alwaysconverged and did not necessitate as fine of a mesh. Activation scheme is dependent on othersimulation choices; full and partial both have merits. Full proved to be more robust, especiallywith a tet mesh, but partial is a closer representation of the physics and doesn’t sacrifice runtime.Expansion time constant did not seem to have an impact in any way until it got too large ( 5x thetime step).Recommended default settings:Follow deformation NOMesh resolution: 1 element through thickness is reasonableElement type C3D8IActivation Scheme PartialTime step 2-4 physical build layersExpansion time constant 2*time step (recommended by Abaqus virtually identical to 0)14

Abstract: As additive manufacturing (AM) evolves to become a more viable production solution in terms of cost, quality, and time, the need for predictive simulation of the process grows as well. . This resolves the temperature history of the part which is then fed into a mechanical model as a predefined field. Then, the mechanical model runs .