Sheet Cutting Design Guidelines

This guide is designed to help engineers and designers prepare CAD and STEP files that meet manufacturing standards. Following these design requirements prior to order submission helps prevent file rejections, shorten lead times, and reduce overall manufacturing costs.

Note: Material-specific values—including minimum hole size, internal radius, and thickness limits—vary by material and process. 

1. File Formats & Submission Requirements

Select the appropriate file format based on whether your part is flat or contains 3D forms/bends.

Unsupported Formats

Mesh Files: .stl, .obj, etc., are not accepted for flat/formed sheet cutting.

Raster Images: .jpg, .png, .tif, .bmp, etc. All raster artwork must be converted to vector geometry prior to submission.

2. Vector & CAD File Cleaning

A production file should contain only the closed cutting geometry required to manufacture the part. Clean all construction elements and annotations before exporting.

Scale & Units

• 1:1 Scale: Build files at full final cut size. Written dimensions inside drawings are ignored by automated processing systems.
• Units: Imperial (inches) is preferred. Metric (millimeters) is acceptable when used consistently between the file and quote. Centimeters and meters are not supported.

Manufacturing Geometry Only

Remove all dimensions, title blocks, borders, guides, notes, and annotations. 

Convert Text to Outlines

Convert all text to vector outlines (or explode/expand text in CAD). Editable fonts/text boxes cannot be recognized as cutting geometry.

Closed Cutting Profiles

Every cut path must form a fully closed shape. Inspect geometry in wireframe/outline mode before export to detect unclosed paths or tiny gaps.

Duplicate & Overlapping Lines

Delete duplicate, overlapping, or intersecting vector entities. In multi-entity geometry, duplicated lines can be interpreted as double-cutting paths and ruin cut quality.

Dedicated Layer Usage

Place all final cut paths on a designated cut layer. Move construction geometry or annotations to separate layers or delete them entirely prior to export.

Bridging Floating Interiors

Internal "islands" (e.g., the centers of letters like O, A, B, or donut-shaped cutouts) will become detached during cutting. Add bridges or stencil connections to retain them. Bridge width depends on material thickness.

3. Part Dimensions & Multi-Part Nesting

Establish part envelopes and multi-part arrangements early to avoid sizing and production rejection issues.

Part Size Limits

Size limits vary by material and manufacturing process.

• CNC Routing Size Limits:

○ Minimal part size: 2mm (0.08in)

○ Maximal part size: 1000 mm (40in)

○ Minimal diameter: 0.3mm (0.01in)

These are general size restrictions; the specific restrictions vary depending on the material. For details, please upload your file and wait for an engineer to review it to determine if it is acceptable.

Multi-Part Ordering & Pre-Nesting

• Single File Upload (Recommended): For multiple copies of the same part, upload one file containing a single part and set the desired quantity at checkout.
• Pre-Nesting Rules: Pre-nested layouts are permitted only when:

1. All parts share the same material and thickness.
2. The file is a supported 2D vector format (.dxf, .dwg).
3. Pre-nested 3D formats (.step/.stp/.iges/.igs/.sldprt) are not accepted. Bending, tapping, or hardware-inserted parts must be uploaded as individual single-part files.

No Common-Line Nesting

Do not share a cutting line between adjacent parts. Common-line cutting does not account for kerf, beam width, tool diameter, or stream width (which introduces a gap ranging from ~0.006″ to 0.012″ depending on material). Separate each part geometry according to process tolerance limits.

Directional & Mirrored Materials

Materials with distinct surface finishes (e.g., brushed ACM, mirrored acrylic, textured ABS, hardboard) require specific top/bottom orientation. Save mirrored variations as separate files when orientation matters.

4. Feature Design Tolerances & Limits

Check hole sizes, internal corners, narrow walls, and cutout density against process limitations before finalizing artwork.

Feature Limits Summary

Narrow Walls & Isolated Features

Extremely narrow walls or small isolated features tend to distort or overheat during cutting. Maintain minimum feature dimensions as specified for your target material and process.

Dense Cutout Patterns

Intricate patterns (e.g., grilles, speaker grates) increase cutting times and heat buildup, potentially causing warping or thermal marks in thin stock. If burn marks occur on fiber laser cut samples, increase the line/web thickness between cutouts.

5. Process-Specific Design Guidelines

Selection of laser, waterjet, or CNC routing depends on material composition, stock thickness, and required edge quality.

 Laser Cutting

• Ideal for sheet metals, acrylic, and select boards.
• Mind the heat-affected zone (HAZ) and kerf allowance on small, intricate features.

Waterjet Cutting

• Preferred for heat-sensitive or thick materials (composites, rubber, foam).
• Internal corner radii are constrained by the ~0.032″ waterjet stream diameter.

CNC Routing

CNC routing uses a rotating bit for flatbed cutting on materials like ACM, plastics, wood, and boards.

• 2D Flatbed Limitation: CNC routers perform 2D flatbed cut-throughs only. They cannot produce V-grooves, 3D surface contours, partial-depth cuts, double-sided cuts, or counterbores. Tapping and countersinking are handled via separate post-processing services.
• Dogbone Fillets for Square Corners: Because a rotating bit leaves an internal radius (min. 0.063″), a square peg will not seat flush into a standard routed pocket. Add dogbone fillets (corner over-cuts) to provide proper clearance for mating components. Standard chamfers do not eliminate the tool radius.\

Sizing Formula:

Dogbone Diameter ≥ Tool Bit Diameter+ 0.005″(0.13mm)

(Example: When routing with a standard 0.125″ bit, design your dogbone circles with a diameter of at least 0.130″.)

•  Fixturing Tabs: Small perimeter tabs retain routed parts during cutting.

○Tab size: ~0.1875″ wide × 50% material thickness deep.

○Tabs are removed/sanded post-process and do not alter functional geometry.

○Edge geometry must allow at least 0.400″ spacing between vertex nodes for tab placement.

• Material Removal Limit: Do not remove more than 50% of total material on perforated or skeletal designs to prevent parts from shifting or breaking during routing.
• Edge Finish: Routed edges may display minor witness marks, steps, or friction discoloration. These are standard for the process and do not affect structural performance.

6. Formed & Bent Sheet Metal Parts

When submitting parts that require bending, folding, or forming, follow true sheet-metal modeling rules.

One Solid Body Per File

Each .step or .stp file must contain exactly one solid sheet-metal body. Multi-body solids or assemblies cannot be processed within a single part file.

Model True Sheet-Metal Geometry

Use dedicated sheet-metal design tools in your CAD software. Extruded solids or mesh objects are not valid substitutes for sheet-metal bodies.

Uniform Thickness & Simple Features

• Maintain uniform material thickness throughout the part.
• Include a flat edge face at every boundary.
• Do not model partial-depth features, tapered edges, or countersinks directly into the 3D model. Model simple through-holes only; specify secondary services (tapping, countersinks) during quoting.

Reference Plane Alignment

Align at least one major flat face parallel to a primary CAD reference plane to ensure accurate flat-pattern unfolding.

Material Rules & Bend Parameters

Apply a sheet-metal rule matching your target material thickness, bend radius, and K-factor. Mismatched bend parameters cause open-contour or flat-pattern export errors.

STEP Export Verification

Ensure the single sheet-metal body is selected before exporting. A file reading as 0″ × 0″ upon upload indicates an unselected body or missing solid geometry.

Bending Geometric Guardrails (Keepout Zones)

Placing holes or small features too close to a bend line will cause material stretching and feature distortion during die press braking. Follow these minimum spacing requirements:

• Hole-to-Bend Line Minimum Distance:

Minimum Clearance= (2 × Material Thickness) + Bend Radius

(Holes placed closer than this limit will deform into ovals during bending.)

• Minimum Flange Height (Bend Leg Length):

Minimum Flange Length= 4 × Material Thickness

(Flanges shorter than this limit cannot sit stably across the lower press brake die during forming.)

• Cutout Relief at Bends:

When a cutout intersects a bend line, add bend relief slots extending at least 1× Material Thickness beyond the bend line on both sides to prevent material tearing.

7. Troubleshooting Common File Errors

8. Pre-Submission Checklist

Verify the following before uploading your production file:

• File Format: Vector (.dxf, .dwg) for flat parts; 3D Solid (.step, .stp, .iges, .igs, .sldprt) for bent parts.
• Scale & Units: Created at 1:1 scale using consistent Inches or Millimeters.
• Clean Geometry: All dimensions, notes, construction lines, and borders removed.
• Text Outlined: All text converted to vector paths.
• Closed Paths: All cutting profiles form fully closed shapes.
• No Duplicate Lines: Overlapping and shared geometry removed.
• Islands Bridged: Floating interior cutouts connected with stencil bridges.
• Feature Limits: Hole diameters and internal radii satisfy selected process minimums.
• CNC Requirements: Dogbones added to internal square corners; material removal ≤ 50%.
• 3D Sheet Metal: Exactly one solid sheet-metal body per file with uniform thickness.
• Nesting Setup: Single part per file (no common-line cutting); separate directional or mirrored parts into distinct files.