School of Engineering · Playlist

Digital Fabrication

Preparing CAD models for 3D printing and laser cutting, and choosing a fabrication process.

  1. 3D Printing from CAD
  2. Laser Cutting and Engraving from CAD
  3. Choosing a Fabrication Process
Engineering Graphics and CAD/Digital Fabrication

3D Printing from CAD

Export a solid model, choose how its layers carry load, and inspect the sliced toolpaths before printing.

Build the part by adding layers

Build the part by adding layers

Additive manufacturing makes a shape by adding material. This page uses thermoplastic-filament material extrusion: a printer feeds filament through a heated nozzle and deposits it along paths, much like a controlled hot-glue gun. Fused filament fabrication (FFF) is generic usage for this route; fused deposition modeling (FDM) is a registered trademark of Stratasys.

A slicer divides the model into horizontal cross sections and plans the paths for each layer. The nozzle and build surface move relative to one another to build the next layer. A CAD model describes the desired shape; the sliced file describes how a particular printer will make it.

This page focuses on filament printing. Resin, powder and metal routes use different placement, joining and post-build mechanisms; compare them in Additive Manufacturing Process Families. Their preparation, handling and finishing procedures are not interchangeable.

Export the model, then check its size in the slicer; Checklist

Export the model, then check its size in the slicer

  • Finish and save the editable CAD model. Check that the intended part is a closed solid; see Feature-based Modeling.
  • Export the intended body as STL or 3MF if supported by both programs. Inspect curved surfaces for coarse facets.
  • Import into the slicer and compare a known dimension with the CAD model. Check units, scale, and the number of bodies.
  • Select the actual printer, nozzle, and approved material profile. Do not assume settings imported with a file match the available machine.
  • Orient the part, set walls, infill, layer height, and supports, then slice and inspect the layer preview.
  • Export the printer's required job format using the posted procedure. Save the slicer project so you can revise the setup.

Supporting detail: Addendum 1 — STL and 3MF carry different information.

Use walls for the shell, infill for the interior, and supports where needed

Use walls for the shell, infill for the interior, and supports where needed

Walls, also called perimeters, trace the outside and hole boundaries. Infill fills some of the interior. Solid top and bottom layers close the part. Increasing infill is not a substitute for choosing suitable walls and orientation.

Layer height sets the thickness of each deposited layer. Smaller layers can reduce the steps on sloped surfaces but usually add print time. They do not by themselves make a thin wall or tiny hole printable: nozzle size and extrusion width matter too.

Supports are temporary material beneath regions that cannot print reliably in the chosen orientation. They use material and time, may leave rough contact surfaces, and must be reachable for removal. A short bridge between two supported edges differs from an unsupported overhang; check the machine's demonstrated capability instead of assuming one universal angle limit.

A side view shows stacked layers and temporary supports under an overhang. A top slice shows perimeter walls surrounding sparse infill.

Supporting detail: Addendum 2 — Why more infill does not solve every strength problem.

Orient for load direction, surface quality, and support removal; Practice

Orient for load direction, surface quality, and support removal

Ask which way the part will be pulled or bent. Filament prints are often weaker when a load pulls adjacent layers apart. For a straight bar pulled along its length, laying its length in the build plane is usually a better starting point than printing it upright. Test a representative part before relying on it under load.

Then consider the important faces. A face against the bed takes the bed's texture; a supported underside may need cleanup; a slope shows layer steps. Rotating the part can improve one surface while making another worse. A broad, stable bed contact usually makes the start easier than a narrow footprint.

Practice choosing an orientation

Try it: orient a bracket for support, layer direction and load; Interactive

Try it: orient a bracket for support, layer direction and load

Turn an L-bracket on the build plate and read three consequences together: which downward faces would need support, whether the load in use runs parallel to the layers or must cross the bonds between them, and how layer height leaves steps on the curved faces.

Challenge: this bracket will be screwed to a wall and carry a weight hanging from its arm. Which way up should it print? Read three consequences together: overhangs that need support, the direction of the load relative to the layers, and the steps that layers leave on curved faces.

The bracket: arm 60 mm, back plate 50 mm, both 8 mm thick and 30 mm wide, a 10 mm inner fillet with a concentric 18 mm outer round, and a 6 mm gusset across the inside corner. These are chosen illustrative dimensions.

  • Needs support: downward and flatter than the threshold
  • Downward but at or steeper than the threshold
  • Resting on the plate, or inside the first layer
  • Upward or vertical: never flagged
  • Stretched path: blue = parallel to layers, red-orange = normal to them
A. Arm flat on the plate
Unsupported overhang (proxy)
329 mm²329 mm² of downward faces flatter than 45°, projected onto the plate. Flagged faces do not overlap in plan; plate footprint about 330 mm².
Resting on the plate
1,260 mm²Downward faces on the plate are supported by it.
Height and layers
50.0 mm · 250 layers⌈50.0 ÷ 0.20⌉ at 0.20 mm
Load-to-layer angle
up to 90°Around the bend the stretched direction ranges from 0° to 90° from the layer planes. Part of it is mostly normal to the layers, so that load must cross the bonds between layers.
Layer steps on the curves
inner 0.08 mm, outer 0.09 mmMeasured in the drawn cut; not a roughness value.
B. On its side
Unsupported overhang (proxy)
428 mm²428 mm² of downward faces flatter than 45°, projected onto the plate. Flagged faces do not overlap in plan; plate footprint about 430 mm².
Resting on the plate
768 mm²Downward faces on the plate are supported by it.
Height and layers
30.0 mm · 150 layers⌈30.0 ÷ 0.20⌉ at 0.20 mm
Load-to-layer angle
up to 0°Every stretched direction lies within the layers (0°): no part of the load has to cross the bonds between layers. The road (raster) direction inside each layer is set by the slicer and is not modelled here.
Layer steps on the curves
none on the curved faces (vertical walls)Measured in the drawn cut; not a roughness value.
Two orientations of the same bracket, 0.20 mm layers, 45° threshold, hanging weight
OrientationUnsupported overhang (projected)On the plateHeight · layersLoad-to-layer angle (max)
A. Arm flat on the plate329 mm²1,260 mm²50.0 mm · 25090° (hanging weight)
B. On its side428 mm²768 mm²30.0 mm · 1500° (hanging weight)

What the comparison shows: standing up (A), the bend's stretched path must turn through the layer stack, so part of it pulls layers apart, and the lower outer round needs support. On its side (B), the stretched path lies within the layers and the curves print as vertical walls, but the gusset now overhangs the open corner. Neither is free: you choose which consequence to accept, or change the design (for example a chamfer instead of a downward-facing round, or no gusset).

Layer steps on a curved face

12
Vertical cut through the front of the bracket: thin line = CAD shape, stepped line = 167 layers of 0.30 mm.
1 mm
1 Inner fillet: largest gap between the true curve and the layer steps in this cut 0.12 mm
1 mm
2 Outer round: largest gap between the true curve and the layer steps in this cut 0.12 mm

How the numbers are worked out

  • Build direction: +z, from the plate toward later layers. Layers are horizontal planes.
  • Face inclination θ = arccos|nz| from the horizontal plate (0° horizontal, 90° vertical), where n is the face's outward unit normal. A face is downward when nz < 0.
  • Needs support when downward and θ is less than the threshold (45° here; 44° is flagged, 46° and exactly 45° are not). A face resting on the plate, or lying wholly within the first layer, is supported by the plate. Upward and vertical faces are never flagged.
  • Unsupported-overhang proxy As = Σ Ai·|nz,i| over flagged faces: their area projected onto the plate. Example A: the outer round is flagged from 30 × (18 sin 45° − 18 sin 5.6°) ≈ 329 mm² (the lowest facet sits inside the first layer).
  • Layers N = ⌈H ÷ h⌉. Example A: ⌈50 ÷ 0.20⌉ = 250.
  • Load-to-layer angle φ = arcsin|dz| for the stretched direction d: 0° lies within the layers; 90° is normal to them and must cross the bonds between layers. Within a layer, the slicer also chooses the road (raster) direction; this model does not include it.
  • Layer steps: each layer is the cut at its mid-height, extruded straight up through the layer. The figure measures the largest gap between that stepped outline and the CAD curve in one vertical cut.

Model limits: a geometric teaching model, not a slicer. The support figure is a projected-area proxy: it is not support volume, print time or a promise that a face will print. Bridging between two supported edges, support landing on the part, interface gaps, cooling and removal are not modelled. The 45° threshold is an adjustable guideline, not a universal limit. The load angle is a direction only: no strength value, failure prediction or material data.

Supporting detail: Addendum 3 — Where the threshold and the load rule come from.

Use the preview and the failed part to find the next check

Use the preview and the failed part to find the next check

Missing thin feature
Inspect the sliced paths. A feature visible in CAD may be too thin for the selected extrusion width; revise the feature or an approved setup.
Loose first layer or lifted corners
Check bed preparation, first-layer setup, and the material profile against the machine procedure. Warping involves shrinkage as the part cools.
Sagging underside
Check the orientation, unsupported spans, and support placement before repeating the same job.
Gaps, strings, or shifted layers
Check material condition, extrusion, temperature/profile, and machine motion as appropriate. These symptoms have several possible causes; change one justified factor at a time and record the result.

In the preview, inspect the first layer, small holes, supports, and the final top layers. Estimate time and material before starting. Follow Equipment Operating Procedure and Machine Hazards and Housekeeping for operation and handling; the nozzle and build surface may remain hot after motion stops.

For parts that must fit together, continue to Choosing a Fabrication Process and Tolerances and Fits.

Engineering Graphics and CAD/Digital Fabrication

Laser Cutting and Engraving from CAD

Separate cutting paths from engraved areas, preserve scale, and account for the material removed by the laser.

Use vector paths for outlines and raster scans for filled marks; Practice

Use vector paths for outlines and raster scans for filled marks

A vector operation follows lines and curves. A raster operation scans across an area to make a surface image or filled mark.

A vector path can cut through a sheet or make a shallow score, depending on the material and settings. Raster engraving typically changes the surface without cutting out the part. A bitmap picture of an outline is not automatically a usable vector cutting path.

Vector motion follows a continuous rectangular boundary. Raster motion scans parallel rows across a filled rectangular area.

Practice choosing cut or engrave

Prepare a full-size profile and assign each operation deliberately; Checklist

Prepare a full-size profile and assign each operation deliberately

  • From CAD, export the intended planar face or sketch as a supported vector format such as DXF. View the face normal to its plane; a perspective picture is not a true-size profile.
  • In the vector editor, set units and page/piece size. Import the file and measure a known feature to confirm 1:1 scale.
  • Remove unwanted dimensions, notes, borders, and duplicate paths from the fabrication copy. Check for gaps in outlines that should be closed.
  • Assign cut paths, score paths if used, and raster areas to the correct operations. Inspect fills as well as strokes.
  • Match page/piece size and placement in the artwork and machine software. Preview the job and check its extent against the actual sheet.

CorelDraw is one possible vector editor. Line weight and color can tell a particular driver how to treat an object, but those conventions are not universal. Follow the posted procedure for that driver and confirm the operation in its preview.

Supporting detail: Addendum 4 — Why a hairline is a workflow setting, not a cutting guarantee.

Offset the path toward the waste by half the kerf; Practice

Offset the path toward the waste by half the kerf

Kerf is the width of material removed by a cut. In the simple model below, the laser follows the center of a constant-width kerf. Half the removed width lies on each side of the path.

For an outside part boundary, move the path outward by kerf / 2. For an opening, move the path inward toward the material being removed. Without compensation, a cutout part becomes smaller and a hole becomes larger.

An outside part has its cutting path outside the desired edge, while a hole has its cutting path inside the desired edge. Each path is half a kerf into the waste.

For a desired outside width W, the path-to-path width is W + k, where k is kerf. For a desired opening width H, it is H − k. These are whole-width changes; the offset at each edge is only k / 2.

Measure a test cut in the same material and setup. Kerf can vary with thickness, focus, and settings, and cut edges may taper. If software already compensates the path, do not apply the same allowance again. See Tolerances and Fits for fit requirements.

Practice an outside dimension Practice an opening

Treat power, speed, and pulse settings as a matched setup

Treat power, speed, and pulse settings as a matched setup

Power controls laser output; speed controls how quickly the spot travels. With other conditions held fixed, higher power or slower travel generally puts more energy into a length of cut. That can also increase scorching or melting rather than improve the edge.

Frequency or pulse settings control how pulses are delivered. Controls may use pulses per second, pulses per distance, or a machine-specific scale; read the manual's definition. A percentage from one machine is not a transferable recipe for another.

Use the posted procedure and the manufacturer's starting settings for the exact machine, material, and thickness. Confirm the result on an approved test piece. Check that the cut separates and that engraving is readable before running the complete job.

Supporting detail: Addendum 5 — Manufacturer guidance for selecting a starting setup.

Confirm the material and stay with the operating laser

Confirm the material and stay with the operating laser

Only process materials approved for that machine. Suitable grades of wood and acrylic are common CO₂-laser examples, but coatings, adhesives, thickness, and machine capability matter. A material that can be marked is not necessarily one the machine can cut through.

Do not cut or engrave PVC or vinyl containing PVC. Do not guess the identity of an unknown plastic. Never leave an operating laser unattended. Use the required extraction and follow the machine procedure for a flare-up or other abnormal condition.

Use Equipment Operating Procedure, Fire Safety, and Personal Protective Equipment for the shared safety rules.

Supporting detail: Addendum 6 — Manufacturer safety reference.

Engineering Graphics and CAD/Digital Fabrication

Choosing a Fabrication Process

Match geometry, load, surfaces, and fit to filament printing or laser-cut sheet construction.

Choose from the required shape and material first

Choose from the required shape and material first

Start with what the part must do. A process is useful only if it can produce the geometry in a suitable material with the required performance.

Filament printing
Builds three-dimensional shapes in layers. It suits changing cross sections, bosses, and internal features when those features can be printed and supports can be removed. Layer direction and service temperature affect the choice.
Laser-cut sheet
Produces planar profiles from a sheet of existing thickness. It suits flat panels, plates, and repeated outlines. Three-dimensional structures need joints, stacked layers, or another forming operation.

A flat nameplate with surface lettering is a natural laser candidate if the sheet is approved. A one-piece curved knob with a raised boss is a natural printing candidate if a suitable printable material meets the load and temperature requirements. Neither choice establishes production time without a job estimate.

For setup details, use 3D Printing from CAD and Laser Cutting and Engraving from CAD.

Design features the selected process can actually make

Design features the selected process can actually make

Printed walls and holes
Check that the slicer generates the intended paths. Leave access for support removal. Do not assume a CAD hole prints at its nominal size; measure a representative sample.
Laser-cut webs and corners
Leave enough material between cuts for the part to survive fabrication and use. Account for kerf and heat effects. An infinitely sharp CAD corner does not guarantee an infinitely sharp cut corner.
Sheet joints
Design slots from measured sheet thickness and the intended clearance. Kerf compensation controls the cut edge; clearance controls how two finished parts fit. They solve different problems.
Assembly
Plan how pieces enter their final position and how they are held. A collision-free CAD assembly does not prove that real parts will fit or can be assembled; see Assembly Files and Mates.

Supporting detail: Addendum 7 — Why there is no universal minimum wall or perfect press-fit allowance.

Test the critical feature before making the full part; Checklist; Practice

Test the critical feature before making the full part

  • State the required shape, material, load direction, surface, and fit.
  • Identify the feature most likely to fail: a thin wall, loaded layer joint, supported surface, or mating slot.
  • Make an approved small sample that preserves that feature and the intended process setup.
  • Measure or test the sample against the requirement. Record the setup and the result.
  • Revise the design or setup, then compare time, material, cleanup, and assembly effort before making the full part.

Practice selecting a process Practice clearance and kerf

Supporting detail

Addendum

Additional evidence, standards context, and background referenced from the main text.

  1. Engineering Graphics and CAD/Digital Fabrication/3D Printing from CAD

    Addendum 1. STL and 3MF carry different information

    STL represents the surface with triangles and does not record a unit of length. A 3MF file can carry units and multiple objects; a slicer's 3MF project can also carry settings. Support for those extra settings varies between applications. Neither filename alone proves a job is ready for your printer. Prusa documents saving projects as 3MF and its supported file formats.

    Back to reference 1

  2. Engineering Graphics and CAD/Digital Fabrication/3D Printing from CAD

    Addendum 2. Why more infill does not solve every strength problem

    Material near the outside can be especially useful when resisting bending. Infill also supports top surfaces and can help resist compression. The useful balance depends on the load and shape. Prusa's infill guidance discusses these different roles.

    Back to reference 2

  3. Engineering Graphics and CAD/Digital Fabrication/3D Printing from CAD

    Addendum 3. Where the threshold and the load rule come from

    PrusaSlicer's overhang threshold is measured the same way as here: Prusa's support material guide calls it "the most horizontal slope (measured from the horizontal plane) that you can print without support material." Prusa's modeling guide says printers can cleanly print overhangs at "an angle between 45 and 60 degrees, depending on your nozzle diameter and settings," and warns that a fillet facing the bed creates a steep overhang. That is why 45° is only a starting value here.

    Ahn and colleagues measured FDM ABS specimens and found that strength depends on the direction of the deposited roads; their first build rule is to "build parts such that tensile loads will be carried axially along the fibers" (S.-H. Ahn et al., Anisotropic material properties of fused deposition modeling ABS, Rapid Prototyping Journal 8(4), 2002). The tool shows only the direction; it gives no strength values.

    The build-direction convention follows ISO/ASTM 52900: for planar layer-by-layer processes, the positive z-direction runs normal to the layers, from the first layer to later ones.

    Back to reference 3

  4. Engineering Graphics and CAD/Digital Fabrication/Laser Cutting and Engraving from CAD

    Addendum 4. Why a hairline is a workflow setting, not a cutting guarantee

    The teaching deck uses hairline strokes for vector cuts and strokes of at least 0.5 pt for raster content. Preserve those values only when the specified driver procedure calls for them. Stroke width alone does not establish cut depth, material suitability, or a safe setting.

    Back to reference 4

  7. Engineering Graphics and CAD/Digital Fabrication/Choosing a Fabrication Process

    Addendum 7. Why there is no universal minimum wall or perfect press-fit allowance

    Printer paths depend on nozzle and profile; laser edges depend on the sheet and setup. Material batches and finishing change dimensions too. A small test of the critical feature supplies evidence that a generic dimension cannot. Use Tolerances and Fits to distinguish the intended size from acceptable variation.

    Back to reference 7