CAD Output for FDM - Stratasys Direct Manufacturing

CAD Output for FDM - Stratasys Direct Manufacturing
Design for Additive Manufacturability:
CAD Output for FDM
Your Computer Aided Design (CAD) file tells the story of
your potential part. It holds the data and information about
material, tolerances, geometry and features. CAD applications
use a universal set of surface and solid definitions that make up
a part. Additive manufacturing systems (3D printers) require
a different set of data, basically made up of triangles forming
the surface of a part. In order for an additive manufacturing
system to build a part, the CAD file needs to be exported into
an STL file. Often information can get lost in this translation
from CAD to STL. It is important to prepare your files for the
export to ensure quality expectations and design intentions
are maintained from CAD to final part production.
There are a number of ways to optimize and prepare your
CAD data to guarantee clean files ready for processing and
production. There are adjustments you can make to complex
geometry data, such as wall thicknesses, or even small changes
to file size and features that will help create a pristine STL
file and accelerate processing. This article will explain some
important considerations specifically for the Fused Deposition
Modeling (FDM) process. We recommend reading Design
for Additive Manufacturability: FDM Basics first to learn the
differences between designing your part for 3D printing vs.
traditional manufacturing processes.
The STL file format is used to exchange information on the part geometry between CAD and
a 3D printer. The STL format approximates the surfaces of a solid or surface model or point
cloud with triangles. In an STL file, each and every triangular ‘facet’ is defined in terms of the
coordinates of its three vertices. The triangles are tessellated, arranged in a gapless, repeating
pattern of non-overlapping figures, to create the STL file. The triangulation of the surface causes
faceting, in which the triangles or facets deviate from the design intent. When the faceting is too
coarse you can see flat spots on curved surfaces when viewing the STL file. These flat spots will
show up when the part is produced. To avoid this, it is important to find the right file resolution
for your application.
File resolution
Faceting can be controlled by the following settings when exporting the STL file from
the CAD system:
• Angle control – the maximum angular deviation between adjacent triangles
• Chordal tolerance/deviation – the maximum distance between the surface of
the original design and the tessellated surface of the STL model
The majority of parts can be produced to meet the application’s requirements simply using
the default export settings. However, more demanding applications often require specific
settings to achieve the goals of the application. Coarse faceting is nearly always caused by the
angle setting being too high or the deviation/chord settings being too high, or a combination
of both. For example, a deviation/chord height setting around 0.0004 inch in SolidWorks will
usually produce a good quality FDM part, but increasing the resolution may be necessary for
parts with fine or rounded features.
But increasing the resolution will also increase file size. Large files take longer to transfer and
process which could increase lead time and the cost of part production. A good rule of thumb
is to keep file size below 15 Megabytes because going above this value will rarely improve
part quality. The goal is to produce a file detailed enough that the features will build to the file
dimensions while maintaining a manageable file size.
Excessively fine
A contour is the material deposited along the perimeter curve on each layer that makes up the
outer extent of the part on that layer. Most parts have just a single contour but multiple contours
can be used to increase the stiffness of the part and wall thickness. The thickness of the contour
is equal to the extrusion path width, which is determined by the diameter of the tip used to
produce the part. For example, a T16 tip has an inside diameter of 0.016 inch, a minimum
extrusion path of 0.016 inch and a maximum extrusion path of 0.032 inch. The thickness of
vertical walls should be at least twice the slice thickness in order to avoid creating flimsy walls
that are prone to buckle.
The outer perimeter of the part and
edges illustrate contours. The interior
material illustrates raster.
Rasters and fills
The material used to fill the interior of the part between the contours is called a raster.
The raster can be set to fill the interior with a sparse (honeycomb) or solid fill. A sparse fill
requires a minimum of two contours to define the exterior of the layer and has an air gap
between extrusions in the interior, reducing the cost and weight of the part. A sparse fill also
adds porosity to the part which can be useful in situations where you need a lightweight part or
certain tooling applications such thermoforming and paper pulp molding. The sparse fill air gap
can range from 0.001 to 0.5 inch while 0.080 to 0.150 inch is most common. An overall part wall
thickness of 0.200 inch or greater is where you’ll see cost savings from sparse fill since it uses
less material than if you were to fill it solid.
No changes need to be made to the part geometry
to use a sparse fill. Work with your project engineer
or designer to determine if sparse fill is a good option
for your part or application. Another option is to use a
negative air gap on top level surfaces to compress the
raster fill to a higher level of density than a solid fill. This
approach provides a particularly good surface finish.
Different fills can also be used in different areas of the
part. For example, a thermoforming tool might have a
normal air gap on the surface to impart a smooth finish
on the produced part and a positive air gap in others so
that air can be drawn through the tool.
In designing parts to be produced by CNC machining, a general tolerance such as
+/- 0.005 inch is often specified for areas of the part where no other tolerance is noted.
This does not usually cause problems because tolerances of this magnitude are relatively
easy to hold with CNC machining. For FDM parts, close tolerances should be specified
when necessary. Precise tolerances are achievable with FDM, but secondary operations may
be required which then requires leaving extra stock on your part design that can later be
machined down to your specifications.
top of part
top of sliced curve
Zoomed in side shot
of a file after slicing.
notice how the top red
line is not equal to the
top surface of the part?
this is due to the height
of the part not being in
increments of the z slice
Close tolerances may also make it necessary to use a thinner slice thickness, which in turn
gives you a more accurate part, but will drive up the build time and increase cost. Both
cost and accuracy of an FDM part can be optimized by carefully considering the tolerance
requirements and application, selecting the largest slice thickness that can be used to achieve
these tolerances, then dimensioning the part in increments of this layer thickness. For example,
if the decision is made to use a 0.010 inch layer thickness then whenever possible the z-axis
dimensions should be defined in multiples of 0.010 inch, such as 0.050 and 0.100 inch. In that
case, the part will be produced with near-perfect accuracy in the z-axis.
Living hinges
A living hinge is a unique feature that is traditionally complicated to manufacture. Flexible
materials, like FDM Nylon 12 which provides twice the elongation at break of SLS Nylon 12,
make hinges easier to produce and can deliver scores of full 0 to 180 degree opens and
closes. However, a living hinge should only be produced with FDM for prototyping or concept
modeling applications with a short service life.
Living hinges should be designed and optimized with the best build orientation to last through
a small amount of cycles – see an example below. The hinge wall needs to be thick and strong
enough to withstand mechanical stress and bending. The hinge itself should be kept thin and
will normally consist of two contours. If a 0.010 inch tip is used then the hinge can range from
0.032 to 0.040 inch total thickness.
good hinge
The hinge feature, when sliced, is on
the same layer as the body of the
part. this gives it the most strength.
Bad hinge
In this orientation, the hinge would
only be connected to the main body
with one layer.
Fastening hardware
Mechanical fasteners and inserts are common among prototyping and end use applications.
With FDM, washers, nuts, bolts, threaded rods, or other objects can be inserted mid-build
at the specified area without secondary operations, accelerating the process and decreasing
delivery time. In order to embed hardware into the build, create a cavity in the design file with
no clearance where the insert will be placed and let your project engineer know to adjust the
clearance in the file based on tip size, depth and insert call out. The build can only be paused in
the Z orientation in order to embed the insert in the clearance, therefore build orientation needs
to be on the X/Y plane (see the illustration below).
top of cavity
part continues to
build after object
is inserted
This illustrates the correct build orientation
for mid-build inserts. Once the part builds to
the top of the cavity for the object, we pause
the build, insert the object and then resume
the build.
This orientation is impossible for mid-build
inserts because the inserted object would
be sticking out above the last layer printed,
preventing the printer head from building the
next layer on top of the object.
FDM parts can also be drilled and tapped, but the threads will only last through a few fastenings
so heat staked inserts are preferable for most applications. Heat staked helicoils provide a high
torque limit and greatly reduce the potential for the thread to be stripped with repeated use.
Bosses, ribs and gussets
Bosses are usually added to a part to later be drilled and tapped. If the wall thickness of the
boss is less than other areas of the part, it may be necessary to use a smaller tip size which will
produce a more accurate hole. To ensure the correct diameter, consider reaming the hole to the
correct size. For optimum performance, the boss diameter should be minimum 3x that of the
insert diameter. A larger boss diameter decreases the chance of fracture when using interference
fits and increases the strength of the boss.
Often ribs and gussets are used in injection molding to avoid warp or sink marks that occur
during cooling. These additional features aren’t necessary when using FDM unless they’re critical
to the part function, but can increase the amount of stress a feature can endure.
Multiple Shells, Nested or Tabbed Parts
To ensure accurate quoting and quick delivery of assemblies, tabbed or nested parts, you
should always save each individual piece as a separate STL file. If files aren’t separate, they
often appear as one part and will most likely be difficult to quote and build because you can’t
optimize orientation for each separate part. Tabbed parts are also difficult to build because
the break-away walls are too thin. An example of a tabbed part is a model airplane kit. Each
individual part is connected together by tabs that when twisted, remove individual components.
Multiple shells are possible and should be used when your part contains moving components,
such as gears or a flag hinge. Just make sure to include enough air gap clearance between
moving parts that will be built up with removable support material and leave an appropriate
air gap. We recommend discussing orientation with a project engineer when producing
multiple shells.
Example of a file with
nested parts.
Inversed Normals, Edges and Surfaces
A clean STL file is referred to as “water-tight”, meaning there are no missing surfaces in the
file, the surfaces do not overlap, and there aren’t any inversed or bad edges. Typically most
solids modeling CAD applications, such as SolidWorks, Inventor or ProE, produce clean,
water-tight files. CAD applications based on surfaces, such as Rhino, or STLs that come
straight from scanned data may not be clean and need to be repaired before processing.
You can easily find errors in your STL file by using an STL viewing tool. All tools provide visual
information, but some also offer specific information on areas of concern within your native file.
If surfaces aren’t trimmed correctly, the 3D printer will not be able to properly read the data,
causing delays in production.
Adding text can enhance the aesthetics of parts, whether it is to brand a part with a company’s
name or to customize the look of a part. However, there are a few guidelines to follow when
adding text to a part’s surface. The minimum suggested text is 16 point bold on the top or
bottom build plane of an FDM model and 10 point bold on vertical walls. Text above the surface
of the part is more efficient to produce than cut text because support material is easier to
remove from the surface than it is in small crevices.
STL Export Units
Each CAD program has unique STL export settings. As a rule of thumb, make sure to set your
STL export units to inches or millimeters. FDM’s software only interprets inches or millimeters
so if your STL export from CAD is in centimeters, the geometry will be correct, but the part
won’t be built to scale.
Production doesn’t begin when we hit print; it begins in CAD with
your design. Each CAD system is different, but understanding your
data, designing your parts for 3D printing and properly exporting STLs
accelerates the manufacturing process so your order arrives on your
desk sooner than you needed and exactly how you designed it. Follow
the suggestions in this guide and consult with experts at RedEye to
start making better files and improving your production process.
8081 Wallace Road
Eden Prairie, MN 55344
• ISO 9001:2008 Certified
• AS9100 Revision C Certified
• ITAR Registered
©2014 RedEye. All rights reserved. RedEye is a business unit of Stratasys, Inc.
Stratasys, RedEye, FDM, FDM technology, Fused Deposition Modeling, ABS,
ABS-ESD7, ABS-M30, ABS-M30i, ABSi, PPSF, FDM Nylon 12, and PC-ISO are
trademarks or registered trademarks of Stratasys, Inc. and/or its subsidiaries
or affiliates and may be registered in some jurisdictions. PolyJet is a trademark
of Stratasys Ltd. and/or its subsidiaries or affiliates and may be registered in
certain jurisdictions.
ULTEM is a trademark of SABIC Innovative Plastics IP BV.
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Download PDF