Design for AM

Abstract

Many industries approach AM as a direct replacement for conventional manufacturing technologies. This approach, however, does not fully utilize the unique possibilities that additive processes offer.

4.1 The General Thought Process of DfAM

Many industries approach AM as a direct replacement for conventional manufacturing technologies. This approach, however, does not fully utilize the unique possibilities that additive processes offer. For example, a production component designed for 3-axis computer numerically controlled (CNC) machining that is manufactured through additive processes will, generally, be more expensive to produce with AM. Additionally, parts generated through 3D printing may still require conventional machining-based post-processing in order to meet surface quality and engineering tolerance specifications. Thus, AM should be approached as a complimentary form of manufacturing through which novel products/forms of products can be generated. In general, it should only be considered as a viable production technology if the value it adds to the product is high enough to overcome the high costs of its relatively slow speed.

Much like the design requirements of established manufacturing technologies, the optimal fabrication capability of AM is dependent on the implemented design. It is through this design for additive manufacturing (DfAM) that parts of increasing geometrical complexity can be generated without the financial constraints found within conventional manufacturing. This enables the use of complex re-entrant geometries, lattice structures and otherwise difficult to produce geometries resulting from topology optimization.

AM also enables several design features that would otherwise be impossible or very expensive to achieve with conventional manufacturing. Through the layer-upon-layer process of AM, it is possible to produce internal voids without complex tooling or dividing the component into several parts. This enables, for example, internal conformal cooling channels to be added to molds to increase productivity and part quality. Additionally, AM has allowed for the generation of objects having multiple parts/components without the requirements of post-fabrication assembly.

Additive manufacturing, because of its layer-upon-layer process is, by nature, a slow manufacturing process. This relatively slow speed, especially when compared to conventional manufacturing technologies such as injection molding and casting, means it is also an expensive technology. For this reason, it is important to only use AM for production when it adds enough value to overcome the high cost of producing the part.

The overall thought process that can be useful in redesigning parts for AM includes:

• 1. Reduce part to only those features that serve functionality.

  With a conventional technology, such as CNC machining, we try to minimize the amount of cutting required for the part and, therefore, try to remove as little material as possible from the billet we start with. AM is precisely the opposite, because any material that does not serve a real engineering function is just material that has to be processed by the AM system and therefore costs time and money. Anything that breaks the ‘even-thickness rule’ is just unnecessary material that increases cost, causes more residual stress and therefore more supports and heat treatment.

• 2. If, after reducing the part to only those features that serve a real function, some of those features are disconnected, then decide how those features can be joined together.

• 3. Now consider the most appropriate print orientation depending on what is important to you. Print orientation will have an impact on part surface finish, mechanical performance, and the amount of post-processing that will be required. In the majority of cases, this decision will be a compromise in which some characteristics are improved, while others deteriorate.

• 4. Run it through support generation software to see results.

  • Consider replacing temporary supports with permanent walls. Support material can be thought of as a temporary wall that will be removed after the part is printed. So why not consider replacing the temporary wall with a permanent one that then becomes a feature of the part.

  • Consider changing the angles of features requiring support. If a feature is horizontal, it will require support material beneath it. But, if you can change its angle, chamfer or gusset the bottom horizontal face at 45 degrees then the need for support material can be avoided.

• 5. Reiterate.

As an example, let us look at the step-by-step design thought process that can be employed in the redesign of a 100 mm × 100 mm × 100 mm steel manifold.

Eliminate evrything that does not serve a purpose

The first step of the design process starts with eliminating everything in the manifold that does not serve a real function. In the case of a manifold, the only thing that performs a real function are the pipes, so the goal of the first step is to eliminate all the material that is not a direct part of the pipe network. The goal is the simplest possible representation of the ‘block’ manifold (Fig. 4.1) with just the actual channels for the transport of hydraulic fluid.

Fig. 4.1

Simplified ‘block’ design manifold with only the required in and out channels (Courtesy of Olaf Diegel [1])

Once the block design has been simplified, the next step is to remove all the excess material of the cube to leave just the pipes that form the manifold channels. The majority of CAD software packages have some built-in functionality, often called a ‘shell’ function that makes this step relatively easy. In this example, we select all six outer faces of the cube to be removed, and apply the ‘shell’ function (Fig. 4.2), leaving only the internal channel structure with, in this case, a thickness of 2 mm.

Fig. 4.2

Manifold design after shell operation on block design (Courtesy of Olaf Diegel [1])

Decide on print orientation

One of the early decisions that needs to be made when designing for AM is the print orientation, as this will affect all other design decisions thereafter. This is because print orientation will have an impact on almost every aspect of the part. When designing for additive manufacturing, one should always design around the specific orientation in which the part will be printed because part orientation will determine the direction of anisotropy, mechanical properties, surface finish, roundness of holes, support material, etc.

When we run the manifold example through software used to generate support structures we see that support is generated between all the horizontal pipes (Fig. 4.3). In one of the orientations below, where the large diameter pipe is horizontal, we can see that support has also been generated inside the large diameter pipe.

Fig. 4.3

Support material required by shelled-block design in 2 different print orientations (Courtesy of Olaf Diegel [1])

It is important to remember that, in DfAM, there is no absolute that says one orientation is better, or worse, than the other. Instead, it must be a conscious exercise to examine what the effects of a particular print orientation are on a part. In our example, both print orientations will necessitate the removal of this support material after printing, as well as some surface treatment to improve the surface finish of the areas where the support material makes contact with the real part. This post-processing increases the amount of labour required to finish the part, extends the delivery time on the part, and increases cost.

One could possibly make the argument that, in the print orientation where the large diameter pipe is horizontal, it will be harder to remove the support from inside the pipe than from all the outside surfaces. So, unless there were some other advantage to having the large diameter pipe printed horizontally, the better print orientation might be the one where it is in the vertical position. However, without fully understanding the context in which the manifold will be used, one cannot guarantee that this is, in fact, the best orientation.

Eliminating support material

Support material is, essentially, a sacrificial temporary material, that serves a certain purpose during the print process, but is then removed after the print is finished. In many cases, a design option that is worth considering is to replace the support material beneath each of the horizontal channels with a permanent wall to eliminate the need for support material altogether. The idea is that the added wall becomes the support material and becomes a permanent feature of the part.

In the case of the manifold example, we can replace all of the support material with permanent walls, thus eliminating the need for support material entirely. The bottom walls are chamfered at 45°, as that is the angle we have set beyond which to use support material, and we can add elliptical, diamond, or teardrop-shaped holes in the walls to further reduce weight, yet without requiring support material in the holes. As can be seen below (Fig. 4.4), the only needed support material is a very small amount required to weld the part to the build platform.

Fig. 4.4

Support material required by optimised for metal AM design (Courtesy of Olaf Diegel [1])

In the case of the above manifold, the weight of the original 100 mm × 100 mm × 100 mm block design, in steel, would be 7.4 kg. In contrast, the optimised for metal AM design weighs only 600 g. That represents a greater than 94% weight saving, and a proportional reduction in print time and cost.

The above example demonstrates how some simple design decisions can greatly reduce the amount of support material required, and therefore, the post-processing, which means a better product at a lower cost. Remember, however, that in many cases of printing metal AM parts, some support material is unavoidable, but that the designers thought process should constantly be looking for ways to minimise it.

4.2 The Economics of DfAM

This section investigates economic arguments related to AM, namely how design-controllable factors of this manufacturing and the results of DfAM affected costs relate to operations, material, and processing.

Though the strategies implemented within this chapter apply equally to all AM technologies, a focus is made with respect to metal PBF AM because it is one of the technologies in which cost and time factors are the most significant. This section will evaluate the current economic relationships relative to operations within AM. An analysis regarding the current fabrication related costs is conducted to act as a better framework for discussions relating to design-based 3D printed part optimization. To further illustrate these ideologies, a case study is conducted through which the described DfAM techniques are demonstrated in the generation of previously discussed manifold part. The preferred design option for this example was fabricated with an EOS M290 selective laser melting system, in 316L stainless steel, to demonstrate that it could, indeed, be printed with minimal support material and post-processing.

4.2.1 Machine Costs

Printing parts in which DfAM has not been considered are susceptible to high costs. This is due to the expensive nature of industrial AM systems paired with comparatively slow part production rates. A metal production sized AM system, typically, costs between US$500,000 to over US$1,500,000.

A typical operational time (80%) for a metal AM machine results in approximately 7000 h of annual use. A desirable return on investment used by industry recoup the cost of a rapidly evolving technology infrastructure investment is, for example, 2 years. Whilst this may vary relative to individual companies, it will suffice as a benchmark for this work. Additional associated costs might include potential loan-based interest rates (e.g. 5%), installation labour and power consumption (both being relatively minor expenses in comparison to machine time). This simplified cost model is summarized in the Equation below and some examples for the hourly running costs of differently priced AM systems are shown below in Table 4.1.

$$ \begin{aligned} & {\text{Machine}}\;{\text{hourly}}\;{\text{running}}\;{\text{costs}} = ({\text{Machine}}\;{\text{purchase}}\;{\text{cost}} + {\text{interest}})/ \\ & \;\;({\text{payback}}\;{\text{period}}*\% \;{\text{running}}\;{\text{time}}*{\text{yearly}}\;{\text{hours}}) \\ \end{aligned} $$

Table 4.1 Machine hourly running costs for 2-year payback period and 80% utilization

The above equation illustrates a simplified costing model from which hourly operational machine costs between US$500,000 to US$1,200,000 have been generated. From this range of potential costs (US$37–90/h) an average of US$65/h was used for the examples in this chapter. This is, in some cases, a potentially optimistic value as certain user specific expenses (e.g. overheads) have not been accounted for. Currently, metal AM technologies are associated with long operational times (e.g. dozens of hours to produce a part to, not uncommonly, greater than 100 h) demonstrating an operational cost vs. time vulnerability within the technology. These operational costs are, however, not dissimilar to other conventional high-end manufacturing technologies such as industrial CNC and injection molding machines. However, geometrically simple parts can be produced much faster with these conventional technologies than they can with AM.

4.2.2 Material Costs

Metal AM powders can range from US$70/kg (e.g. steel or aluminium) to US$300/kg (e.g. cobalt chrome or titanium) which is significantly more costly than the same material alloys used for traditional manufacturing. Costs for AM polymer materials are also substantially more expensive, between 10 times to up to well over 100 times, than their conventional manufacturing counterparts.

Powder-based metal AM also requires the use of additional support material for overhanging part geometries, to anchor the part to the build platform and to help with heat dissipation. This support material, together with losses from partially sintered powder, yields an estimated 8–10% loss/wastage of material. Thus, an argument can be made relating to the reduction in wasted material (relative to subtractive manufacturing) and therefore cost reduction in production. Currently these material costs are often negligible relative to the machine-time costs. However, the likely future increases in AM production speeds will result in an increased role of material costs in metal AM cost-based viability in the future.

4.2.3 Post-processing Costs

AM typically requires pre- and post-processing to yield a desirable part. This includes operations relating to the heat treatment of parts, support material removal and surface modification. The table below shows the estimated cost proportions of these tasks with values derived from a 2017 Wohlers Report service provider survey [2] (Table 4.2).

Table 4.2 Breakdown of pre and post-processing time versus print time

This data indicated that approximately 45% of metal AM expenditure is related to the pre- and post-processing required for part production. This value demonstrates the significant economic impact of parts which have not been designed to minimize these processes.

Time-consuming operations within AM are not solely limited to part geometry and post-processing. Such operations relate to the time taken to, for example, the spreading of material for a layer (recoater time) and the implementation of controlled environmental conditions. The requirements for purging (typically the removal of oxygen through inert gas addition) and the heating of the printing region are machine and material dependant. The recoater time is user dependant given the implemented part print orientation which will typically affect the required number of layers/recoating operations. However, if two parts, one well designed and one poorly designed, have the same overall height, then the recoater time will be the same for both, and is not affected by how good or poor the design is.

4.2.4 Time Factors That Are Affected by Design

Similar to the golden rule of injection moulding, where even wall thickness is always recommended, large masses of material, typically, offer little functional advantage. In fact, large material masses can be detrimental as those are the areas that are likely to contain residual stress which can cause distortion of the part. Moreover, in AM, large areas with solid material also greatly extend print times. There are many techniques for removing large masses of material, including the ‘shell’ technique described below. Others include filling solid parts with honey-comb, lattices, or even porous material. From a time-based perspective, it is best to print a part in the orientation in which it has the lowest vertical height as this will generally have the fewest layers, and therefore the fastest print time. However, because print orientation also plays a major role on part mechanical properties, geometric accuracy, surface finish, and support material, this decision can often be a compromise between print time and these other aspects.

Design factors that reduce laser operating time

Within most AM, printing time is directly related to the quantity of material which needs to be solidified. This is particularly true of powder-based techniques which employ a processing (sintering/melting) beam (laser or electron) to scan across a region of power to generate a fused layer/slice of a model/part. This scanning operation can be characterised as either a contour or hatching operation (Fig. 4.5).

Fig. 4.5

Example form highlighting the typical implementation of laser scanning for contourlines and hatch patterns (Courtesy of Olaf Diegel [1])

The contour operation relates to the processing of the slice edge (which will become the part outer surface) and the hatching operation relates to the pattern employed to process the internal material of the part and can occur in various forms (e.g. meander, stripe or chess-board). A good analogue for the laser scanning process would be to draw a shape outline with a pencil (this being the contour operation) and then proceed to ‘colour in’ the internal area of the shape by running the pencil back and forth (hatching) many times.

As such it is desirable to implement techniques capable of reducing the quantity of material requiring laser scanning. Techniques of solid material substitution with shells, honeycombs or lattices result in faster manufacturing as they avoid unnecessary processing of material.

Design factors that affect print time and cost

The Table 4.3 further highlights the various stages within an AM process which are affected by part design and in which part design can, therefore, influence the cost of the part.

Table 4.3 Factors within AM processes through which DfAM can yield economic improvements

4.2.5 Economics Case Study: Metal AM Manufactured Hydraulic Manifold

Within AM, metal-based techniques yield the greatest opportunity to optimise the design for products otherwise designed for traditionally manufacturing. One example of which are manifold like objects, as per the example discussed in the previous section. These parts are typically generated by the drilling of channels within a large metal block to form a network of interconnecting pipes. Of note is the requirement to drill separate holes through the block to act as internal connecting channels, some of which are then required to be appropriately blocked (plugged) post machining. The Fig. 4.6 below illustrates the previously discussed block manifold example for which a print layer is depicted to highlight the inferred AM material/material processing requirements.

Fig. 4.6

A block manifold and an illustration of the laser scanning process to melt a single layer of the part (Courtesy of Olaf Diegel [1])

The scanning hatch pattern for the example layer slice will require a relatively long beam scanning distance. For a manifold having dimensions 100 mm × 100 mm, and a hatch spacing set to 0.1 mm, a scanning hatch distance of approximately 100 m is required per square layer. For the purposes of this example, a beam travel speed of 330 mm/s and the previously derived machine operating cost of US$65/h will be utilized. This results in a layer hatching time of 100/0.33 = 303.03″ s = 5.05″ min. At $65/h this equates to US$5.47 in operational time.

The first fundamental step related to DfAM encourages a reduction in material requiring processing. The use of a hollowing (“shell”) based technique upon the generated model allows for the retention of the established surface morphology as well as the specification of a desirable uniform wall thickness. The results of this modification are depicted in the Fig. 4.7 below.

Fig. 4.7

A shelled block manifold and an illustration of the laser scanning process to melt a single layer of the part (Courtesy of Olaf Diegel [1])

This simple alteration to the model results in a greatly reduced material processing (laser scanning) requirement, therefore reducing overall print time and cost. Utilising a ‘shell thickness’ of 2 mm and the previously described hatch settings yields a total hatch distance of 4.5 m (a > 95% reduction over the solid block). This will take approximately 13.6 s to hatch and result in a layer cost of US$0.24 (saving US$5.23 per layer). It is worth noting that within powder-based AM the generated cavity will be filled with un-melted powder. For applications in which this is not desirable, this powder can be removed via the inclusion of an opening/hole through which this excess material can be drained. It is worth noting, also, that support material is still likely to occur for the horizontal geometries within the shelled structure. The removal of these would be relatively complex or impossible.

Given the parts requirements, the outer surface (external box form) can be further removed yielding a part having solely the desirable functional form of the manifold thereby further reducing print time and the associated costs. Within this example, limited functional reduction in support material will be achieved via the variation of printing orientation for the manifold. Whilst the support material required for the part can be reduced by implementing an angular alteration (relative to the desired materials operational range) to the various extrusions of the manifold, this would not yield a functionally desirable result. Additionally, within metal AM support material is fundamental in anchoring the part to the build platform as well as aid in the controlled dissipation of thermal energy. As such it is required to minimise the potential thermally generated distortions which could occur to the part during fabrication. As such this example made use of designed permanent supporting structures which when added to the part both avoid automatically generated support as well as acted to reinforce the channels.

Great care must also be taken to ensure no/limited support material occurs within the manifold channels as this will result in flow distortion. The maximum diameter from which AM will no longer require support material will vary relative to the material and machine utilised. Within this example, the utilised material (Stainless Steel 316L) and EOS M290 Printer allowed for a minimum inner diameter of 8 mm for the manifold channels without requiring any additional support structures. The resultant manifold design including the implemented permanent support structures is demonstrated in the Fig. 4.8 alongside a version which depicts the limited automatically generated support material.

Fig. 4.8

Resultant manifold design having permanent support structures and model depicting software derived support material (blue) (Courtesy of Olaf Diegel [1])

With regards to the aforementioned steps required in DfAM; step 1 related to the implemented hollowing/shell technique and removal of all the non-essential material, step 2 was not required as the design geometries were already connected, step 3 identified the potential regions and requirements for support material relative to printing orientation, and step 4 included the reduction in support material via inclusion of permanent support structures and software-based design validation. The resultant manifold developed through this process is shown below (Fig. 4.9). This required no further surface machining and the channels were manufactured free of support material, the part only needing removal from the printer build plate for use.

Fig. 4.9

A designed for AM block manifold with reduced print time and support removal time (Courtesy of Olaf Diegel [1])

A costing comparison of the various stages of the part redesign (solid block, shelled block and optimized DfAM) was conducted through simulating these parts within Autodesk’s Netfabb Ultimate 2018 software for an EOS M290 machine. The print material was set to 316L stainless steel and a layer thickness of 50 µm utilised. The simulations identified major reductions in time and cost namely; an approximate ~90% reduction in time, ~90% reduction in machine cost, ~92.5% reduction in weight and material cost. Additionally, external AM bureau quotes were requested and an 87% reduction in purchasing cost was identified. The results of these costing comparisons are shown below (Table 4.4). This case study acts as an example of how AM, and more specifically the DfAM can dramatically improve production cost and part size/weight.

Table 4.4 Manifold design print times and cost

This chapter demonstrates that machine cost and print time is one of the main factors that affects AM part production and the most significant controllable factor is the avoidance of large masses of material. These require extended hatching times, and the avoidance of support material aids in minimizing post-processing. It quantifiably demonstrates that a simple strategy of replacing large masses of material with even wall thickness shells can have a substantial impact on hatching times and therefore machine time and cost.

This chapter establishes the importance of DfAM from an economic point of view. The difference in cost between a part that has been designed for AM compared to that of a conventional part made with AM is so significant illustrating DfAM to be an essential part of successfully implementing AM. Moreover, if one includes the less quantifiable added value elements such as reduced weight, improved functionality, reduced time to market, reduced waste material etc., then the argument for the absolute necessity of DfAM is not hard to make.

4.3 Polymer Design Guidelines

A previous assessment of part geometry is recommended so as to evaluate whether additive manufacturing will bring benefits to our part or not, based on a first quick assessment we will be able to decide if AM, conventional manufacturing methods or both of them are required.

Some of the keypoints that must be analysed are:

• Part weight/volume assessment.

• Production costs (using traditional methods) AM technique that will be necessary.

• Part nestability (build density).

• Functional surfaces and part requirements (geometrical and dimensional tolerances to be achieved).

Although costs involved in the Additive manufacturing production chain vary depending on the technology, average values can be stablished as: (i) material (15%), (ii) human resources (30%), (iii) machine (55%), and (iv) post processes (if required).

Therefore, many variables take part in the process that will affect part production costs.

Part weight/volume

Given the material optimization that additive manufacturing processes permits due to the design freedom, this is not only an opportunity for the part to be optimized in terms of weight but also an opportunity to reduce the production costs in the AM processes. The more parts we manage to put inside the build envelopment the cheaper the production costs will be.

Hence the design for additive manufacturing is a key factor for the part and process optimization. Normally a part which is conceived for traditional methods will not be economically feasible for AM if the design is not adapted.

Production costs analysis

As in all the additive manufacturing technologies happens, there is a fix cost which comes from the machine preparation and build preparation, the cost will not vary if only one part is produced or plenty of parts are nested inside the build envelopment, therefore the unitary cost will vary depending on the amount of parts that are allocated in the build envelopment. Some calculations can be done so as to assess the feasibility of additively manufacture a certain geometry. A relationship between unitary costs and number of parts per build is found in Fig. 4.10.

Fig. 4.10

(Source Skin Project—AIDIMME)

Unitary costs versus number of parts in build envelopment

As a summary, although there might be different approaches depending on the part complexity and each situation, there are a few questions that we must formulate so as to decide whether re-desing for additive manufacturing will be required or not:

• Production: number of parts that will be manufactured. Given a certain 3D model that it was conceived for standard methods as milling, CNC and so on, the re-design for additive manufacturing will require human resources. Hence if just one copy will be produced through AM, the entire re-design HR will be charged to this copy, whereas if the number of parts demanded is bigger, re-design costs will be distributed between them all.

• Know the environment of the part and the working conditions: prior to a redesign process, it is quite important to understand how the part works, the interaction with other parts in the assembly and the working conditions (loads and restrictions). Some of these restrictions might limit our design.

• Know the dimensional and geometrical tolerances: AM technologies are not as accurate as traditional methods, thus areas of the geometry where fine adjustments or very specific geometrical and dimensional tolerances are demanded, will require to be post processed. A good understanding of these limitations will allow us to focus our design thinking not only in the part construction, but also in the post processing steps, clamping areas, and so on.

• Know the raw material: we can find that in some occasions, parts are being manufactured in materials that are not necessary just because the production ratios make inefficient processes as injection moulding. (These methods require high productions in order to amortize the mould costs. Therefore, it is highly recommended to analyze the material to be used for the part construction, sometimes a part which was initially conceived in metal-based materials, can be produced in polymeric materials by additive manufacturing.

• Know the surface finishes: due to the layer by layer method of the AM processes, parts produced by these techniques present an important surface roughness that sometimes is detrimental in the final parts, just because the mechanical properties are slightly affected or because the part appearance is compromised. Thus, surface finish must be defined so as to determine which kind of postprocessing tasks will be applied and of course it will affect the DfAM.

• Determine the AM process: once the previous key factors have been analysed, AM technique must be defined. Design rules vary quite a lot from one technology to another, thus depending on the AM process that is selected, re-design approach will be different.

4.3.1 Designing for Material Extrusion (MEX)

Material extrusion is the AM process with the most anisotropy. The bond between the layers can substantially weaken parts in the vertical direction, so this is the process in which choosing the most appropriate print orientation can have the biggest impact.

Material extrusion accuracy and tolerances

There is a great difference in accuracy and tolerance between different material extrusion systems. This is particularly the case when comparing desktop systems to industrial systems. Accuracy and tolerance can also vary depending on geometric features and print orientation. The only sure way to know the accuracy and tolerance of any particular system is to print a test reference part and to measure it.

The numbers given in Table 4.5 are for industrial quality material extrusion systems. They represent a general tolerance and accuracy for material extrusion technologies.

Table 4.5 General tolerance and accuracy for material extrusion technologies

Layer thickness

Layer thickness is one of the first decisions that has to be made when using material extrusion. In general, the thinner the layer, the better the surface quality, particularly on rounded parts, as the stair-step effect will be much less visible. Remember, however, that the thinner the layer, the longer the part will take to print.

If a part is composed mainly of planar geometric features in the vertical direction, then printing it with thicker layers will not necessarily produce a substantially worse surface finishes that if it is printed with thin layers, but it will print much faster. If the part is made up of mainly curved surfaces, then thinner layers may be preferable in order to achieve the smoothest possible curved surfaces.

Support material

Some material extrusion systems print with soluble support material while others do not. If the supports need to be removed manually, rather than being dissolved away, then access should be allowed so the supports can be broken away. Also, with small and delicate features, care should be taken that they are not accidentally broken when the support is removed.

Another decision that has to be made is what type of support material structure options to use. Almost every different maker of material extrusion printer offers different options for this. But some of the common types of support strategies include supports shown in Fig. 4.11.

Fig. 4.11

Types of support strategies (Courtesy of Olaf Diegel [1])

Fill style

Most material extrusion systems allow the user to choose if the part should be printed as a solid part, or as a ‘sparse’ part in which the interior void is filled with a scaffold structure. Some systems may also give the user the option to specify how thick the outer shell wall should be. Some systems also allow the user to select the infill percentage, or how dense the internal scaffold structure should be (Fig. 4.12).

Fig. 4.12

Examples of different interior infill percentage options (Courtesy of Olaf Diegel [1])

Other considerations

A characteristic of the material extrusion process is a “stair-stepping” effect on gently inclined or curved surfaces of parts. This can be reduced by various post-processing techniques (such as acetone vapour smoothing for ABS parts), but this will have an impact on part accuracy, geometrical stability and sometimes material properties.

Material extrusion can, depending on the particular AM system being used, leave a small air gap between the laid down filament for certain wall thicknesses. This is because the software has to make a decision on whether to deposit an extra strand of material in the wall. For example, if the strand of polymer exiting the printer nozzle is 0.4 mm wide, but the wall thickness is 0.9 mm, the software must make a decision as to whether or not to add an extra strand of polymer between the two first tracks, or to leave a 0.1 mm gap. This very much depends on the machine brand and model, so it is best to do some tests and to find which wall thicknesses are not ideal for each brand of machine.

Holes in a Material Extrusion part are usually printed undersized. If tight tolerances are required, it is best to drill the holes to the required diameter.

Because of the sometimes weaker bond between contour lines and infill (or hatch) lines (Fig. 4.13), self-tapping screws can occasionally strip away the contour material in the screw bosses. A drop of cyanoacrylate (super glue), allowed to wick between the contour and fill material can improve this.

Fig. 4.13

Reinforcing the joint between contour and hatch lines (Courtesy of Olaf Diegel [1])

The following pages contain general design guidelines for the material extrusion process.

Vertical wall thickness
Process variable	Wall thickness (t)
Layer thickness	Minimum	Recommended minimum
0.18 mm (0.0071 in.)	0.36 mm (0.014 in.)	0.72 mm (0.028 in.)
0.25 mm (0.0098 in.)	0.50 mm (0.02 in.)	1.00 mm (0.039 in.)
0.33 mm (0.013 in.)	0.66 mm (0.026 in.)	1.32 mm (0.052 in.)
Comments Avoid unsupported large flat surface areas. Warping may occur with extended lengths of unsupported walls (i.e., no ribs or intersecting walls). In this case, avoid using the minimum wall thickness Avoid sharp transitions. Fillets at the points where walls join are recommended In general, an even wall thickness is recommended on all walls, both vertical and horizontal
Horizontal walls
With material extrusion technologies, horizontal walls can, theoretically be as thin as a single layer of material. In practice, however, to produce a horizontal wall with some strength and consistency, at least 4 layers of material are recommended Again, it is best practice to keep all walls of your product at the same thickness

Support material overhang angles
Maximum overhang angle (a)
45° This is a safe default number. But the angle can vary greatly from printer brand to printer brand, and depends on the material used and desired surface quality
Comments Overhang angles less than 45° (measured from horizontal) require support material, which is normally added automatically by the system software. Be aware that some systems measure the support angle from the horizontal, while others measure from the vertical Excessive supports that need to be broken away manually will increase post-processing time. Soluble support structures require much less manual labour, but they still waste material and time Horizontal holes (e.g., cooling channel profiles) can often be modified into teardrop or ovals shapes to minimize the need for internal supports that are hard to remove

Clearances between moving parts with soluble supports
Process variable	Minimum clearance
Layer thickness	horizontal (h)	vertical (v)
0.18 mm (0.0071 in.)	0.36 mm (0.014 in.)	0.18 mm (0.0071 in.)
0.25 mm (0.0098 in.)	0.50 mm (0.02 in.)	0.25 mm (0.0098 in.)
0.33 mm (0.013 in.)	0.66 mm (0.026 in.)	0.33 mm (0.013 in.)
Comments Large areas of close proximity will slow down the removal of support material. Clearance between parts built separately and assembled later must be at least equal to the general build tolerance of the system

Clearance between moving parts with break-away support material
Process Variable:	Minimum clearance:
Layer thickness	horizontal (h)	vertical (v)
0.18 mm (0.0071 in.)	0.36 mm (0.014 in.)	Adequate access to facilitate supports removal
0.25 mm (0.0098 in.)	0.50 mm (0.02 in.)
0.33 mm (0.013 in.)	0.66 mm (0.026 in.)
Comments The main challenge with printing moving parts on a printer without soluble support is in the difficulty of removing the support material from between the moving parts Large areas of close proximity will slow down the removal of support material. Clearance between parts built separately and assembled later must be at least equal to the general build tolerance of the system

Vertical circular holes
Required diameter (d)	CAD model diameter
5.0 mm (0.197 in.)	5.2 mm (0.205 in.)
10.0 mm (0.394 in.)	10.2 mm (0.402 in.)
15.0 mm (0.591 in.)	15.2 mm (0.598 in.)
20.0 mm (0.787 in.)	20.2 mm (0.795 in.)
Comments Holes are generally built undersized, typically by around 0.2 mm (0.0079 in.) across the diameter (Note this value needs to be verified for each machine/material combination being used). This can be remedied approximately by adjusting the CAD model using the values above, or more precisely by drilling out the hole after the part has been built If using self-tapping screws, the column of contour material that surrounds the hole can sometimes be stripped out by the screw. A drop of super-glue, allowed to wick in between the contour and fill material, can alleviate this problem

Circular pins
Minimum diameter for vertical pins (v)	Minimum diameter for horizontal pins (h)
2.0 mm (0.079 in.)	2.0 mm (0.079 in.)
Comments Pins with small diameters, vertical ones in particular, are prone to breaking off if only supported at one end Always fillet the pin where it joins the wall. Even 0.5 mm is enough to substantially strengthen the pin

4.3.2 Designing for Polymer Powder Bed Fusion (PBF-LB/P)

What differentiates polymer powder bed fusion processes, be they laser-based or multijet fusion-based, from the majority of other AM processes is that they do not require support material. The part being constructed does not require supports because the unfused powder surrounding the part provides sufficient support. It can therefore be argued that this gives the designer greater freedom than most other AM system.

Parts created using polymer powder bed fusion usually have some degree of vertical anisotropy, particularly for small features that are less than about 25 mm² in surface area in the vertical direction. Engineers must design around this by, for example, ensuring that highly stressed features are built horizontally rather than vertically.

Powder bed fusion accuracy and tolerances

There is a difference in the accuracy and tolerance between different manufacturers systems. They also vary depending on geometric features and print orientation. The only sure way to determine the accuracy and tolerance of any particular system is to print a test reference part and measure it. The numbers given in Table 4.6 are for industrial quality powder bed fusion systems.

Table 4.6 Tolerance and accuracy for powder bed fusion

Layer thickness

A common layer thickness for powder bed fusion is 0.1 mm, but some systems allow for thinner layer thicknesses. Compared to other AM technologies, however, the stair-stepping effect is less visible on polymer powder bed fusion technologies. It is only on very gently curving surfaces of a relatively large surface area that it is visible.

Avoiding large masses of material

Designers need to be careful in trying to avoid uneven thicknesses of plastic in their parts and to avoid large masses of material. These can cause distortion in the part and will add substantially to the time and cost it takes to make the part. The same applies with multijet fusion because, for large masses of material, much more fusing agent needs to be deposited by the print head, which can substantially increase the cost of the part.

The following pages contain guidelines on how to design features to be built using polymer powder bed fusion.

Wall thickness
Minimum wall thickness (t)	Recommended minimum wall thickness (t)
0.6~0.8 mm (0.031 in.)	1.0 mm (0.039 in.)
Comments Though it is, on occasion, possible to print walls thinner than 0.6 mm, their success is highly dependent on the rest of the part geometry, print orientation, etc Thin walls with a large surface area are likely to warp during the cooling process. If large surface area thin walls are required, consider adding ribs to stiffen the walls Thicker walls and any large volumes of material will result in excess heat retention in the part and hence shrinkage, resulting in geometric deformation. Therefore, a maximum wall thickness of 1.5~3 mm is also recommended. If walls must be thicker than this, consider shelling them. This will both help to reduce distortion and greatly speed up print times In general, an even wall thickness is recommended on all walls, both vertical and horizontal

Clearance between moving parts
Minimum horizontal clearance (h)	Minimum vertical clearance (v)
0.5 mm (0.02 in.)	0.5 mm (0.02 in.)
Comments The required gap between moving parts is highly dependent on the surface area of the faces that are in close proximity. If faces in close proximity have surface areas of only a few mm2, then gaps as small as 0.2 mm between the faces are possible. The 0.5 mm gap stated above is one that will work in most situations and on most different manufacturers systems Large areas of close proximity will slow down the removal of excess powder. Clearance between parts built separately and assembled later should be at least equal to the general build tolerance of the system

Circular profile through holes
Process variable	Minimum diameter
Wall thickness	vertical hole (v)	horizontal hole (h)
1 mm (0.039 in.)	0.5 mm (0.019 in.)	1.3 mm (0.051 in.)
4 mm (0.157 in.)	0.8 mm (0.031 in.)	1.75 mm (0.069 in.)
8 mm (0.314 in.)	1.5 mm (0.059 in.)	2.0 mm (0.079 in.)
Comments Small round holes, typically below 1.5 mm are related closely to wall thickness. As the wall thickness increases, powder becomes increasingly difficult to clear from small holes. As the wall thickness decreases, smaller through holes become feasible

Square profile through holes
Process variable	Minimum diameter
Wall thickness	vertical hole (v)	horizontal hole (h)
1 mm (0.039 in.)	0.5 mm (0.019 in.)	0.8 mm (0.031 in.)
4 mm (0.157 in.)	0.8 mm (0.031 in.)	1.2 mm (0.047 in.)
8 mm (0.314 in.)	1.5 mm (0.059 in.)	1.3 mm (0.051 in.)
Comments Small square holes typically below 1.5 mm are related closely to wall thickness. As the wall thickness increases, powder becomes increasingly difficult to clear from small holes. As the wall thickness decreases, smaller through holes become feasible

Circular pins
Minimum diameter for vertical pins (v)	Minimum diameter for horizontal pins (h)
0.8 mm (0.031 in.)	0.8 mm (0.031 in.)
Comments Pins with small diameters are prone to breaking off if only supported at one end Always fillet the edge where a pin joins a face

Hole proximity to wall edge
Design variable	Minimum distance to edge
Hole diameter	vertical hole (v)	horizontal hole (h)
2.5 mm (0.098 in.)	0.8 mm (0.031 in.)	0.8 mm (0.031 in.)
5.0 mm (0.197 in.)	0.9 mm (0.035 in.)	0.95 mm (0.037 in.)
10.0 mm (0.394 in.)	1.05 mm (0.041 in.)	1.0 mm (0.039 in.)
Comments Larger holes require slightly greater distances to the edges of walls

4.3.3 Designing for Vat Photopolymerisation (VPP)

Although many of the previously covered polymer design rules apply equally to vat photopolymerisation, there are certain guidelines that are specific to resin-based processes.

Resolution

Vat photopolymerisation resolution in the XY-direction is dependent on the laser spot size and can range from 50 to 200 µm. The smallest feature size can therefore not be smaller than the laser spot size.

Resolution in the Z-direction varies from 10 to 200 µm depending on the choices of layer thickness allowed by the machine. As with other AM technologies, choosing a very fine vertical resolution is a trade-off between speed and quality. For a part that has few curves or fine details, there will be little visual difference between a print at 25 µm and one at 100 µm.

Print orientation

When orienting a part for vat photopolymerisation, particularly on a bottom-up SLA machine that cures the part from the bottom and pulls it out of the vat of resin, the biggest concern is vertical cross-sectional area. The forces involved with a print sticking to the bottom of the tank are directly proportional to the 2D cross-sectional area of the print. Because of this, a part with large cross-sectional areas, is often best printed at an angle to the plate. Minimizing the cross-sectional area along the Z-axis is the best way to orient parts for vat photopolymerisation prints. Reducing the number of horizontal areas relative to the print orientation, hollowing out components and reducing the cross-sectional area are all steps that can be taken to optimize a design for vat photopolymerisation.

Support material

Vat photopolymerisation does require support material for overhanging features. This is because the uncured resin is not viscous enough to support features on its own. This support material must be removed in post-processing. On most vat photopolymerisation systems the process of adding support material to the part is largely automated but, with experience, the user can manually edit the supports to avoid having supports in areas where surface finish is critical.

Overhangs

Overhangs generally pose very little issue with vat photopolymerisation, unless the model is being printed without adequate support structures. Printing without supports can lead to warping of the print, but if printing without supports is necessary, any unsupported overhangs should be kept to less than 1.0 mm in length and at least 20° from horizontal.

Isotropy

Vat photopolymerisation is one of the AM processes where the parts are relatively low isotropic. This is because the layers chemically bond to one another as they print, resulting in near identical physical properties in the X, Y, and Z-direction.

Hollowing parts and resin removal

Vat photopolymerisation machines can print solid, dense models but, if the print is not intended to be a functional part, shelling the model to be hollow can significantly reduce the amount of material needed as well as reduce the print time. It is recommended that the walls of the hollowed part be at least 2 mm thick to reduce the risk of failure during printing. If printing a hollow part, drainage holes must be added to allow the uncured resin to be removed from the part. Drain holes should be at least 3.5 mm in diameter, and at least one hole must be included per hollow section, although two holes can make the resin much easier to remove.

Details

Embossed details (including text) include any features on the model that are raised slightly above the surfaces around them. These must be at least 0.1 mm in height above the surface of the print to ensure the details will be visible.

Engraved details (including text) include any features which are recessed into the model. These details are at risk of fusing with the rest of the model while printing if they are too small, so these details must be at least 0.4 mm wide and at least 0.4 mm deep.

Horizontal bridges

Bridges between two points on a model can be successfully printed, but one must keep in mind that wider bridges must be kept shorter (usually under 20 mm) than thin bridges. Wider bridges have a greater cross-sectional area of contact which increases the chance of print failure during delamination from the bottom window.

Clearances for connecting parts

If parts are being made that need to connect together, it is always best have a certain tolerance between the parts that fit together. For vat photopolymerisation, these tolerances are typically:

• 0.2 mm clearance for assembly connections.

• 0.1 mm clearance will give a good push or snug fit.

If interlocked moving parts are being printed, then the tolerance should be 0.5 mm between the moving parts. The following pages contain guidelines on how to design features to be built using vat photopolymerization.

Wall thickness
Minimum wall thickness for supported walls (t)	Minimum wall thickness for unsupported walls (t)
0.4 mm (0.016 in.)	0.6 mm (0.023 in.)
Comments Supported walls are walls that are connected to other structures on at least two sides, so they have very little chance of warping. These should be designed at a minimum of 0.4 mm thick. Note that if the supported wall has a large surface area, a larger thickness may be required Unsupported walls are walls that are connected to the rest of the print on less than two sides, and are at a very high chance for warping or detaching from the print. These walls must be at least 0.6 mm thick Always fillet the corners where one wall meets another wall to reduce stress concentrations along the joint In general, an even wall thickness is recommended on all walls, both vertical and horizontal

Circular holes
Minimum diameter h & v
0.5 mm (0.019 in.)
Comments Holes with a diameter less than 0.5 mm in the X, Y, and Z axes may close off during printing

4.4 Metal Design Guidelines

4.4.1 General Design for Metal PBF

Metal AM technologies can be broken down into the technology categories in the Fig. 4.14 below.

Fig. 4.14

Hierarchy of metal AM technologies (Courtesy of Olaf Diegel [1])

In this chapter we will give recommendation for powder bed fusion technologies based on lasers and electron beams, which are the most widely spread technologies for producing metal parts.

Metal powder bed fusion is an AM process in which thermal energy selectively fuses regions of a powder bed. Materials used include stainless steel, tool steel, aluminium, titanium alloys, nickel-based alloys, cobalt chrome, and precious metals such as gold. The part being constructed normally requires supports (sometimes called anchors) to be added, built from the same material as the part. These supports are removed manually after the build process.

If we compare metal PBF AM parts to conventionally produced metal parts, AM parts, with no post-processing other than support material removal and shot-peening, would perform as follows (Table 4.7):

Table 4.7 Performance of AM parts compared to conventionionally produced parts

With suitable post-processing, however, AM parts can, in some cases, approach the mechanical properties of forged or wrought parts.

The PBF-LB/M AM process

The powder bed fusion process begins by spreading a thin layer of powder onto the build plate, and an energy source is then used to scan the powder and fuse it together where required. The process is then repeated for subsequent layers (Fig. 4.15).

Fig. 4.15

The overall metal AM build process (Courtesy of Olaf Diegel [1])

As metal AM is an expensive process (see the chapter on the economics of AM for details), and parts can require substantial post-processing, you need to have a good reason to make a metal AM part. In general, parts that are not specifically designed for metal AM are not worth doing with AM. There are exceptions to this, like spare parts for example, but, in general, the geometry of the part should be complex enough that it cannot easily be made through traditional manufacturing.

Topology optimisation

Because of the high costs associated with metal AM, topology optimisation is an excellent technique to apply to metal parts. Because one of the benefits of AM is its ability to make very complex geometries, topology optimisation, which can often create cell-like biologically inspired structures, offers the ability to make much lighter components than with conventional manufacturing. Please refer to the chapter on topology optimisation for further information on how to apply this technique to additive manufacturing.

Lattice structures

Lattices are another excellent way of producing light-weight parts, but extremely strong, parts that can also reduce the time and cost it takes to make metal AM parts. A lattice is a cellular structure made of repeated unit cells to form a larger volume. There are many options for the shape and size of such lattice cells, and for the pattern in which they are is repeated. Lattices can be uniform, where the same cell size is repeated in all directions of the part, or variable, where the size and spacing of the cells is different in different directions. There are four main techniques for applying lattice structures to additively manufactured parts:

Convert the entire part into a lattice

This technique transforms the entire volume of the part into a lattice structure (Fig. 4.16). It is commonly done for medical implants, and parts where the exterior surface of the part is not critical.

Fig. 4.16

Complete lattice structure (Courtesy of Olaf Diegel [1])

Fill the inner body of the part with a lattice structure, leaving an outer shell of a specified thickness:

In general, this method requires salt-shaker holes so that the unsintered powder can be removed from inside the part. If designed correctly, the internal lattice structure (Fig. 4.17) also acts as the support material for heat transfer within the part.

Fig. 4.17

Interior lattice structure (Courtesy of Olaf Diegel [1])

The part is subdivided into solid and lattice areas

Here a conscious decision is made as to which features of the part remain solid, and which get converted to lattices. The easiest way to achieve this is usually to split the part up into its different regions in the native CAD software the part was created in, and to then import the separate parts into the lattice conversion software to convert the required parts into a lattices while leaving those that must remain solid untouched (Fig. 4.18). Once this is done, a Boolean operation can be performed to join the lattice parts and solid parts to form a single part ready for AM.

Fig. 4.18

Hybrid lattice structure (Courtesy of Olaf Diegel [1])

Variable lattice structure based on FEA results

This uses any of the above techniques but, instead of a constant cell-sized lattice, uses a lattice structure where the cell size and spacing varies based on a finite element analysis to produce a dynamically-sized lattice structure. The more highly stressed areas of the part wither use thicker lattice members, or a denser spacing of the lattices.

The strut diameters used in lattice structures must be of a diameter such that they can both be manufactured as well as provide the required mechanical properties to the part. Theoretical minimum strut diameter for metal AM is around 0.15 mm. Common sense, however, tells us that a 0.15 mm strut will have relatively little mechanical strength or resistance to fatigue. A more sensible minimum strut diameter to use is, therefore, between 0.5 mm to 1 mm.

When designing lattices, it is important to use lattices that are self-supporting and can be printed without requiring support material. It is possible to have horizontal struts, but they must be short enough to have a surface area below that which requires support material. In the lattice cell shown below (Fig. 4.19), if forces are applied in the directions shown, then design B will resist the force better than design A, but may not be printable because of the horizontal strut. If, however, the cell is printed after being rotated by 90 degrees as shown in C, it will resist the forces and it will print better.

Fig. 4.19

Lattice cell A is weak against the forces, Lattice B is stronger but hard to print because of the horizontal strut. Lattice C both resists the forces and is easier to print (Courtesy of Olaf Diegel [1])

Overhangs and support material

Though it may sound like repetition, it is important to emphasize that supports are absolutely critical in the production of metal AM parts. Supports should not only be considered during part design but can become one of the factors that influence AM part design. The angle and surface area of any overhanging feature of the part determine whether the part will require supports. It is almost always a trade-off to orient the part for minimum build time, easy to remove supports (particularly from inside the part), surface quality, and part warpage. Some aspects will improve, while others deteriorate, depending on the support material being used.

In metal AM, support structures have several functions:

• Support the part in case of overhangs.

• Strengthen and fix the part to the building platform.

• Conduct excess heat away.

• Prevent warping or complete build failure.

• Prevent the melt-pool from sinking down into lose powder.

• Resist the mechanical force of the powder spreading mechanism on the part.

Most metal AM pre-processing software allows the selection of a number of different support types, each of which has different heat transfer and mechanical strength characteristics. Some of the support types offered by most AM preparation software include solid, walls, trees, cones, lattices, blocks, points, lines, webs, and gussets (Fig. 4.20). Which type of support to use very much depends on the part geometry, and how much residual stress it will contain, and how hard the support material will be to remove. The best advice to understand the effect of different types of support offered by your system is to design a part made up of a series of bridges, under which each bridge is printed with a different type of support. The effect of each type of support can then be observed, both in its impact on surface finish and on removal difficulty.

Fig. 4.20

Examples of different support types. Note that these are just used to show examples of different types of support material, and may not be ideal for this particular part (Courtesy of Olaf Diegel [1])

Printing parts with large horizontal surfaces

Parts with large horizontal areas of material will require much stronger supports than the rest of the part. This is because the sudden change in cross section to a large molten sheet of material will cause substantial stress and will, in all likelihood, cause cracks in the part if the support is not very strong and dense. In such situations, one must sometimes use ‘solid’ supports. If at all possible, parts should be oriented so as to avoid large horizontal flat areas, or sudden changes in surface area.

Angle for support material

A general guideline for angles that do not require support material are angles greater than 45° from horizontal. This does, however, vary from material to material and machine to machine. Specific angles relevant to particular materials are given in the table on “Feature type: overhang angle” later in this chapter. Some manufacturers specify angles from horizontal, while others specify them from the vertical. Remember also, that these angles represent the minimum angle at which the part can be produced without supports. In general, using angles that are steeper than those minimum, will yield parts with better surface qualities.

Unsupported angles, overhangs, and bridges

The area melted at the focal point of the energy beam cools very quickly and the stress generated tries to curl the material upwards. Supports act as an anchor to the build plate to avoid such upward curl.

Angles

Poor surface roughness is the result of building directly on loose powder instead of using the support structure as a building scaffold. It occurs because the laser penetrates the powder bed and agglomerates loose powder around the focal point instead of dissipating the heat through the support structure. At a certain point, the unsupported angle becomes such that the part either has an unacceptable surface quality or crashes the recoater mechanism.

Overhangs

Overhangs differ from self-supporting angles in that they are abrupt changes in a part’s geometry, such as a small feature that protrudes horizontally at 90 degrees. Powder bed fusion is fairly limited in its support of overhangs when compared to other 3D printing technologies. In general, any design with an overhang greater than 0.5 mm (0.020 in.) will require additional support to prevent damage to the part. As an overhang extends past about 0.5 mm, the surface quality either becomes unacceptable, or the upwards curl can become such that it causes the recoater mechanism to crash.

Bridges

A bridge is any flat down-facing surface that is supported by 2 or more features. The minimum allowable unsupported distance for the powder bed fusion process is around 2 mm (0.080 in.). Parts that exceed this recommended limit will have poor quality on the downward facing surfaces and may not be structurally sound. They can also cause the recoater mechanism to crash.

Residual stress

One of the most challenging aspects of producing good metal AM parts is residual stress. Like any welding process, metal AM induces a substantial amount of stress on the parts. This is one of the reasons why support material is often needed on metal parts. This residual stress and stress concentrations must be relieved through heat-treatment before the parts are removed from the build plate. Residual stress can, in some cases, be so large that it causes the entire build plate to bend, or the part to detach from the build plate, or crack the part itself. Residual stresses are stresses that remain in a solid material after whatever caused of the stresses has been removed.

Residual stress can occur from a variety of mechanisms including:

• temperature gradients existing from the surface to the centre of AM part during cooling (particularly in large masses of material) where the inside of the part cools slower than the outside of the part.

• inelastic (plastic) deformations.

• structural changes (phase transformation).

• Heat from the laser may cause localized expansion which, in AM, is taken up by either the molten metal or sections of the part that have already solidified. When the finished part cools, some areas cool and contract more than others, leaving residual stresses.

The very best solution to combatting residual stress is to try and eliminate as much of the residual stress out of the part as possible through its design

Designing to reduce residual stress

There are a number of relatively simple design techniques that can be employed to minimize residual stress. These include:

• Get rid of areas of uneven thickness. Large masses of material are the single biggest, but easily avoidable, source of residual stress.

• Try to avoid large changes in cross-section. This may, sometimes, mean having to print your component at an orientation other than horizontal.

• Pre-heat the build plate.

• Heat the build chamber.

In addition, many of the design rules for conventional casting apply equally to metal AM.

If large masses of material are completely unavoidable (which is rare), use different laser hatch parameter settings to minimize the build-up of residual stress.

• Smaller chess-board hatch patterns will, for example, create less residual stress than bigger ones, or than large scan areas. But they will slow down the build process a bit.

• Rotate each hatch scan, usually by 67°, for each layer.

Ultimately, some residual stress is unavoidable. The real question, however, is whether it will affect the function of the part. A well designed for AM part, however, can often require minimal, or no, heat treatment compared to a part that has not been designed for AM.

Stress concentrations

A stress concentration is a location in a part where stress is concentrated. These stresses occur both within the AM fabrication process, and in the heat treatment of AM parts. With metal AM, this is a design opportunity where a well-designed part can minimize the areas of stress concentration. Fatigue cracks almost always start at areas of stress concentration, so removing the areas in which such defects can occur can minimize such defects and greatly increases the fatigue strength of the part (Fig. 4.21).

Fig. 4.21

Stress concentrations are the areas where cracks will most naturally form. Eliminating such stress concentrations can be critical to part quality (Courtesy of Olaf Diegel [1])

The best way of minimizing the amount of heat treatment required is to design your parts to have as little stress induced or concentrated in them as possible. Simple strategies, like filleting all sharp corners (reduces stress concentrations), even wall thicknesses, and avoiding large masses of material (reduces residual stress), can help a lot. In the simple part below (Fig. 4.22), for example, the sharp internal corner has a good chance of causing a stress crack. In addition, the sharp corner has a larger mass of material than the horizontal and vertical walls and will, therefore, contain some residual stress which could cause the wall to distort. In contrast the filleted corner has eliminated the possibility of a stress crack, and it is even wall thickness has minimised the potential of residual stress.

Fig. 4.22

Example of simple filleting to eliminate both stress concentrations and residual stress (Courtesy of Olaf Diegel [1])

Horizontal holes

In metal AM, horizontal holes (or holes angled below the minimum support angle) over a certain diameter will require support material inside the hole. For pipes that are not straight, in particular, the support can be hard to remove from inside the pipe. As a general guideline, holes below a diameter of 8 mm (0.314 in.) can be printed without supports. If larger diameter holes are required, the most common technique is to change the hole from circular to a shape that can be printed without the need for support material. These shapes commonly include ellipses, teardrops, and diamonds (Fig. 4.23).

Fig. 4.23

Hole shapes that can be printed without the need for support material (Courtesy of Olaf Diegel [1])

4.4.2 Design for Laser Powder Bed Fusion (PBF-LB/M)

The design guidelines below apply to laser powder bed fusion metal processes. The guidelines will vary from machine manufacturer and model to machine manufacturer and model so, if in doubt, it is recommended to print a test piece to verify each set of design parameters.

The following pages contain guidelines on how to design features to be built using laser powder bed fusion.

Wall thickness
Minimum wall thickness (t)	Recommended minimum wall thickness (t)
0.3 mm (0.016 in.)	1 mm (0.039 in.)
Comments Problems may occur with extended lengths of unsupported walls (i.e., no ribs or intersecting walls). Without adequate reinforcement, large surface area thin walls are likely to distort. In this case, avoid using the minimum wall thickness, or reinforce the wall with ribs, gussets, or use extra support material to prevent it from distorting Always fillet the corners where the walls meet another surface. A good rule of thumb is to make the fillet ¼ of the thickness of the walls

Overhang angle
Maximum overhang angle (a)
DMLS stainless steel	60°
DMLS inconel	45°
DMLS titanium	60°
DMLS aluminium	45°
DMLS cobalt chrome	60°
Comments Overhang angles less than the numbers shown above (measured from horizontal) will require support material, which may be added automatically by the system software. Excessive supports that need to be removed manually will increase post-processing time Beware that some manufacturers measure support angles from the horizontal, while others measure it from the vertical Feature shapes (e.g., cooling channel profiles) can often be modified to minimize support requirements, and horizontal holes less than 8 mm (0.236 in.) can be built without supports. Se the chapter of this book on the design guidelines for horizontal holes

Clearance between moving parts
Minimum clearance
horizontal (h)	vertical (v)
0.2 mm (0.079 in.)	Adequate access to facilitate the removal of support material
Comments In general, with metal AM, all moving parts will need to be welded to the build platform, or connected to each other, so that they are now swept away by the recoater system. They only become moving parts once they have been cut off of the platform or the joining links have been cut Large areas of close proximity will make the removal of supports more difficult. Clearance between parts built separately and assembled later must be at least equal to the general build tolerance of the system

Vertical slots and circular holes
Minimum width for slot (w)	Minimum diameter for circular hole (d)
0.5 mm (0.02 in.)	0.5 mm (0.02 in.)
Comments As the thickness of the part increases powder inside the slots or holes may become hard, or impossible, to get out Values for horizontal features are not available as they are too dependent on each specific machine If possible, fillet all sharp internal corners to avoid stress concentrations

Vertical bosses and circular pins
Minimum width for boss (w)	Minimum diameter for circular pin (d)
0.5 mm (0.02 in.)	0.5 mm (0.02 in.)
Comments It is good practice to fillet the bottom of all pins and bosses. A general guideline is that the radius is ¼ of the thickness Values for horizontal features are not available as they are too dependent on each specific machine

Built-in external screw threads
Threads should always be built vertically, if at all possible
Comments Though threads down to about M4 can, theoretically be printed, their surface roughness means they will need to have a tapping die run over them to clean up the thread Tapping is recommended for all threads and sufficient space must be left around the post to allow access for the tapping die Fillet the bottom of the boss where it meets the wall to avoid stress concentrations. A good rule of thumb is to make the fillet ¼ of the thickness of the walls

4.4.3 Design for PBF-EB/M Guidelines

Electron beam melting is a powder bed fusion process that uses an electron beam as the energy source to melt each layer of powder. The electron beam is controlled by electromagnets that move it over the powder in a controlled manner to draw the slices of the part to be produced (more in Sect. 1.7.2).

Wall thickness
Minimum wall thickness (t)	Recommended minimum wall thickness (t)
0.6 mm (0.032 in.)	1 mm (0.039 in.)
Comments It is possible to build vertical walls with a thickness of 0.6 mm in solid material, but this can be difficult to achieve in all orientations and with walls of large surface area. A safe recommended wall thickness is 1 mm. For short lengths, such as in lattice structures, different melt strategies can be used so the part can be as thin as 0.3 mm. However, this is not suitable for structural walls as they can suffer from delamination or layer shift Always fillet the corners where walls meet each other

Vertical slots and circular holes
Minimum diameter for circular horizontal hole (h)	Minimum diameter for circular vertical hole (v)
0.5 mm (0.02 in.)	1 mm (0.04 in.)
Comments Holes, slots or tubes built into EBM parts at any angle will be filled with partially sintered powder. This block of powder allows different diameters to be built without the need for supports but can be hard to remove unless access to the hole is easily done with blasting media or with hand tools, so this must be considered during the design stage A minimum diameter of 1 mm vertically or 0.5 mm horizontally is recommended to ensure that rough surfaces do not cause the holes to close up In walls thicker than about 2 mm, vertical holes will generally need to be no smaller than 2 mm and, for horizontal holes, no smaller than 1 mm

Clearances to remove powder
Minimum clearance
horizontal (h)	vertical (v)
1 mm (0.04 in.)	1 mm (0.04 in.)
Comments As there is a partially sintered cake of powder surrounding the parts that are built, access must be given to allow trapped partially sintered powder to be blasted away from small gaps, holes and mechanisms. Larger spaces may have to be included around complex parts to ensure the cake can be removed. In general, 1 mm clearance is usually sufficient to thermally isolate each part on the build platform

Screw and threads
Threads should always be built vertically, if at all is possible
Comments Because of the relatively rough surface finish of EBM, all threads will need to be tapped/machined Fillet the bottom of the boss where it meets the wall to avoid stress concentrations. A good rule of thumb is to make the fillet ¼ of the thickness of the walls