Custom Parts & Fabrication | Spartan Design VRC

// Section 01

Choosing Your Material

Delrin and polycarbonate are the two custom materials you will use most in VRC. They cut differently, machine differently, and require different files out of Onshape. Know which you need before you start the drawing. Spartan Design's primary fabrication tool for custom plastic is the X-Carve Pro 4x2 CNC router — the lasers in the shop are for non-VRC work (see "Why not lasers" callout below).

⚠️

Before any fab operation: required reading is Shop Safety — PPE, before-each-cut checklists for the X-Carve Pro 4×2 and laser cutters, material hazards (Delrin formaldehyde under CO2 laser, prohibited materials), fire watch protocol, and emergency procedures. Mentor authorization required before solo operation of any machine in this guide.

    
  Delrin vs polycarbonate comparison
  
  Delrin (Acetal)
  
  Stiffness
  Very high
  Cut method
  Laser / mill
  Cut edge
  Clean, white
  Best for
  Brackets, mounts
  
  Polycarbonate
  
  Stiffness
  Flexible
  Cut method
  Laser / score-snap
  Cut edge
  Melts slightly
  Best for
  Leafsprings, flex

  

● Delrin (Acetal / POM)

Thickness: 1/16” (0.0625”) for VRC R24 compliance — max thickness is 0.070”
Color: White or black
Feel: Stiff, slippery, very machinable
How you cut it: X-Carve Pro 4x2 CNC router (Spartan Design's primary tool). Inventables explicitly lists Delrin as a supported material. Bandsaw, scroll saw, or hand cut with coping saw also work for simple shapes.
Best for: Motor mounts, custom brackets, spacers, gear guards, bearing supports
VRC advantage: Self-lubricating surface — great for sliding joints. Does not crack under impact like acrylic.
Current workflow: Onshape drawing → 1:1 PDF → print → tape to sheet → cut by hand
Better workflow: Onshape sketch → DXF export → X-Carve Pro (no printing, no tape, higher precision)
Do NOT laser cut Delrin on the Dremel LC40. Per the LC40 operating manual, Delrin (POM/acetyl) is on the prohibited materials list. The X-Carve Pro is the right tool.

● Polycarbonate (Lexan)

Thickness: 1/16” (0.0625”) for VRC R24 compliance — max thickness is 0.070”
Color: Clear (semi-transparent)
Feel: Flexible, impact-resistant, hard to crack
How you cut it: X-Carve Pro 4x2 CNC router (Spartan Design's primary tool) or polycarbonate scoring tool for straight cuts only
Best for: Robot side panels, protective covers, bumpers, intake guards
VRC advantage: Legal as a non-functional decoration and as structure. Light, tough, easy to see through for electronics access.
NEVER laser cut polycarbonate. Polycarbonate releases chlorine gas when laser-cut — toxic and corrosive. The Dremel LC40 manual prohibits it. The Flux HEXA also cannot cut it. The Flux Ador is a diode laser and Flux explicitly does not recommend cutting plastic on it. X-Carve Pro only for poly.
Best workflow: Onshape sketch → DXF → X-Carve Pro. PDF is less useful because hand-scoring poly along complex curves is imprecise.

Which Workflow to Use?

Situation	File from Onshape	Cutting Method	Best For
Hand Simple shape, straight cuts	1:1 PDF drawing (no centermarks)	Print → tape to Delrin → saw or score	Quick one-off brackets, simple motor mounts
Hand Straight poly cuts	1:1 PDF drawing	Score and snap with poly cutter along straight lines	Rectangular panels, simple cutouts
X-Carve Any precision part	DXF (from sketch, not drawing)	Import to Easel or CAD/CAM → run on X-Carve	Anything with curves, complex holes, or tight tolerances
X-Carve Polycarbonate panels	DXF (from sketch)	Spiral upcut bit, low feed rate, single-flute if possible	Side panels, protective covers, intake guards
X-Carve Repeat production	DXF (nest multiple parts)	Easel multi-part layout — cut several from one sheet	Making 4 identical gussets, spare brackets

⚠️

Why not lasers for VRC custom plastic? Spartan Design has three lasers (Dremel LC40, Flux HEXA, Flux Ador) but none of them are appropriate for VRC custom plastic work. The Dremel LC40 operating manual prohibits both Delrin and polycarbonate. CO2 lasers in general release chlorine gas when cutting polycarbonate. The Flux Ador is a diode laser — per Flux, "It is not recommended to laser cut plastic under any circumstances." The lasers serve other purposes (wood, leather, fabric, color printing on the Ador). For VRC plastic parts, the X-Carve Pro 4x2 is the right machine.

Machine Routing Matrix

Quick reference: which machine for which material. This is for VRC custom-plastic work specifically — the lasers handle wood, leather, fabric, and engraving for non-VRC purposes.

Material	X-Carve Pro 4x2	Dremel LC40 (40W CO2)	Flux HEXA (60W CO2)	Flux Ador (diode)
Polycarbonate (Lexan)	✅ Primary tool	❌ Prohibited (manual)	❌ Chlorine gas	❌ No plastic
Delrin / POM (acetal)	✅ Primary tool	❌ Prohibited (manual)	⚠️ Possible w/ formaldehyde ventilation — coach call	❌ No plastic
Acrylic / PMMA	⚠️ Possible	⚠️ Possible	⚠︐ Possible	⚠︐ Black only
Acrylic note: PMMA / acrylic is prohibited under R24f regardless of which machine could cut it. Don't use it on competition robots.
Plywood, hardwood, leather, fabric	✅ Wood	✅ Per material list	✅ Per material list	✅ Per material list

Sources: Dremel LC40 Operating & Safety Instructions Table 2 (Prohibited Materials). Flux Ador product FAQ. X-Carve Pro tech specs — lists Delrin and polycarbonate as supported materials.

1 / 8

// Section 02

Creating the Onshape Drawing

Whether you are heading to the PDF workflow or the DXF workflow, the part design process in Onshape is the same. Get this right and both outputs are clean.

🪓

Workflows

PDF (hand cut) or DXF (X-Carve). Choose by part complexity.

📐

Tolerance Tiers

Critical, important, cosmetic. Apply different precision to each.

✅

All

Pre-Cut Checks

Run the checklist before every cut — PDF or X-Carve.

📚

Sections

Material, drawing, PDF, DXF, tolerances, checklist, sourcing, coach.

Part Studio Setup for Custom Parts

Create a new Part Studio inside the team document

In your robot’s Onshape document, click the “+” tab at the bottom and select “Part Studio.” Name it: Custom — [Part Name] — [Material]. Example: Custom — Motor Mount — Delrin 1/4in. Never design custom parts in the same Part Studio as your assembly references — keep them separate so the assembly stays clean.

Sketch on the Top plane

Select the Top plane and click “Sketch.” Draw your part outline flat — as if you are looking down at the sheet material from above. Use the Line and Circle tools for the outline and holes. All dimensions go here.

Critical: Make your sketch fully constrained (no blue lines remaining). An unconstrained sketch will shift when you add dimensions or mates elsewhere. In Onshape, a fully constrained sketch turns all lines black.

Dimension everything relative to a fixed origin corner

Pick one corner of your part as the origin reference. Dimension every hole position from that same corner — not from other holes. This is called baseline dimensioning. It prevents error stacking: if hole 1 is off by 0.005”, hole 2 measured from hole 1 adds another 0.005” error. Measured from the same origin corner, each hole has independent accuracy.

VEX hole grid: All holes in VEX parts are on a 0.5” grid. Dimension your holes at 0.5” multiples from the origin corner so your custom part aligns perfectly with VEX structure without filing or shimming.

Extrude to material thickness

Exit the sketch, select it, and click Extrude. Set the depth to match your material:

Delrin 1/4” = 0.250”
Polycarbonate 1/8” = 0.125”
Polycarbonate 3/16” = 0.1875”

The extrude direction does not matter for 2D fabrication — it is just for visualization and interference checking in the assembly.

Assign material in Onshape

Right-click the part in the feature tree → “Assign material.” Select the material that matches what you are actually cutting. This sets the appearance correctly for notebook screenshots and also enables the mass properties tool to give you an accurate weight estimate — useful for center-of-gravity calculations on the full robot.

Alternate Entry: Assembly-First (In-Context) Sketching

The Part Studio workflow above starts in a clean Part Studio and assumes you know exact dimensions ahead of time. There's another workflow worth knowing: sketch directly on a face inside the Assembly, capture mating geometry from existing parts (a C-channel, a motor, an existing bracket), then derive the flat custom part from that sketch. This is called in-context design.

When to use it:

The custom part needs to mate to an existing VEX part with non-trivial geometry (e.g., a sensor mount where holes must align with a specific C-channel pattern)
You don't want to re-measure dimensions you already have in CAD
The custom part may need to update if a motor or C-channel moves — in-context sketches stay linked to the assembly

When NOT to use it:

The part has no geometric dependencies on existing assembly parts (e.g., a standalone gear guard) — just use the Part Studio workflow
The geometry is fully defined by VEX 0.5” grid coordinates — baseline-dimensioning from a corner is faster
You're a beginner and haven't built confidence with sketches yet — learn the Part Studio path first; come back to in-context when ready

💡

Cross-link: The Mechanism Concept Sprint guide covers in-context design in the context of designing a distance sensor mount. The steps below add the missing piece: how to take that in-context sketch and turn it into a flat part ready for the X-Carve Pro 4x2.

In-Context Workflow Steps

In the Assembly: select the face you want to sketch on

Open the Assembly tab. Click directly on the face of the existing part where your custom plate will mount — for example, the side face of a 1×5 C-channel. Onshape highlights the selected face.

Create an in-context Part Studio

Right-click in the assembly → "Create in-context Part Studio." Onshape creates a new Part Studio that's linked to the current state of the assembly. Name it: InContext — [Part Name] — [Material]. Example: InContext — Distance Sensor Mount — Delrin 1/16in. Onshape switches you into the new Part Studio with the assembly visible as a faint reference in the background.

What "in-context" means: the new Part Studio sees the assembly as it exists right now. If the assembly changes later, your in-context part can be updated to reflect the new state — or it can stay frozen at the current snapshot. You control this through the in-context version dropdown.

Sketch on the face of the existing part

Click Sketch, then click the face of the C-channel (or whatever existing part you're mating to). Onshape orients the sketch plane to that face. You're now drawing flat against the actual existing part — not in a separate Part Studio with imagined coordinates.

Use the "Use" tool to project existing geometry

This is the key move. With the sketch active, click Use (in the sketch toolbar). Click on the edges, holes, or features of existing parts that your custom part needs to mate to. Onshape projects those edges onto your active sketch as reference geometry. The hole pattern of the C-channel now exists in your sketch as actual sketch entities you can reference.

Why this matters: the projected geometry is exact. No measuring by hand, no transcription errors. If you Use a row of C-channel holes, your custom part's mounting holes are positioned to those exact holes, not to estimated coordinates.

Sketch your custom outline + holes around the projected geometry

Now sketch the outline of your custom part. Use the projected hole positions as direct snap points for your part's mounting holes. Add the rest of the part's features (sensor cutout, additional structural holes, edges).

R24 sanity check: as you sketch, keep an eye on the overall outline dimensions. Per Override R24, every piece must be ≤ 4″ × 8″ × 0.070″. If your sketch outline approaches 4″ in any direction, plan to break the part into multiple pieces. See Sourcing & Inspection for the full R24 rules.

Extrude to material thickness, assign material

Same as Steps 4 and 5 in the standard Part Studio workflow: exit the sketch, extrude to 0.0625″ for 1/16” Delrin or polycarbonate. Right-click the part → Assign material. The result: a fully modeled flat part that's dimensionally locked to the existing assembly geometry.

Fabrication: same DXF or PDF workflow as Section 3

From here, the workflow is identical to a standard Part Studio part. For the X-Carve Pro 4x2: right-click the original sketch in the feature tree (not the extrude — the sketch itself) → Export as DXF/DWG → load into Easel. For PDF cutting: insert a Drawing tab, set 1:1 scale, top view only, dimensioned title block. See Section 3 for X-Carve specifics or Section 2 for PDF specifics.

⚠️

One footgun to avoid: if you Use a feature that later gets deleted from the assembly (e.g., the C-channel gets replaced with a different size), your in-context sketch will throw a "broken reference" error. Two ways to handle this: (a) re-Use the new geometry, or (b) before deleting the original part, convert the projected sketch entities to permanent geometry by tracing them with regular sketch tools. Easier to fix in CAD than to discover at fabrication time.

Creating the Drawing View

Once the part is modeled, create an Onshape Drawing. This is used for both the PDF workflow and as a reference for the DXF workflow. (Same steps whether you used the Part Studio workflow or the in-context workflow above — both produce a Part Studio you can derive a Drawing from.)

Insert a Drawing tab

Click “+” at the bottom → “Drawing.” Select your custom part. Set paper size to A (8.5” × 11”) for small parts or B (11” × 17”) for larger plates. Set the view scale to 1:1 — this is critical for the PDF template workflow.

Add a Top (plan) view only

For fabrication, you only need the top view — looking straight down at the flat face of the part. Do not add isometric views or section views to the fab drawing — they are useful for the notebook but confuse the person cutting the part. Keep the fabrication drawing clean: one view, fully dimensioned.

Add dimensions — skip centermarks for PDF cutting

Add dimension annotations for: outer boundary (width × height), all hole diameters, and all hole positions from the reference corner. Skip center marks for the PDF-cut workflow — they clutter the print and when you are cutting by hand, the dimension annotation is what you measure from, not the cross. Center marks are useful only when you are drilling from a printed template without a CNC machine locating the holes for you.

For X-Carve workflow: You do not need any dimensions on the drawing at all. The DXF carries the geometry. The drawing with dimensions is for your notebook and for the person verifying the part after cutting.

Add a title block note

In the drawing, add a text note with: Part name, material and thickness, cutting method (“Hand cut” or “X-Carve”), quantity needed, and date. This goes in the bottom-right corner. Anyone who picks up this drawing six weeks later should know exactly what to make without asking you.

You are designing a motor mount plate in Onshape. The plate has 6 holes. How should you dimension their positions?

Measure each hole from the previous hole — chain dimensioning

Measure every hole from the same fixed corner — baseline dimensioning. This keeps each hole’s position independent so errors don’t stack.

Measure holes from the center of the plate

Dimensions don’t matter if the sketch is on the VEX 0.5” grid

2 / 8

// Section 03

PDF Workflow — Hand Cutting Delrin

The PDF template method works well for simple shapes with straight cuts. It requires no special software beyond Onshape and a printer. For anything complex or requiring tight tolerances, go to the DXF/X-Carve workflow instead.

📌 Quick Take PDF workflow = print template, glue/tape to plastic, cut by hand. Good for one-offs and prototypes. Quick start, but precision is limited and repeatability is low.

💡

When PDF works well: Rectangular plates, simple L-brackets, one-off parts with only straight cuts, parts you need in the next 20 minutes.
When PDF fails: Curved cutouts, radius corners, parts where hole position accuracy matters more than ±0.030”, any part you will make more than 2 copies of.

PDF Export from Onshape — Step by Step

Confirm scale is 1:1 in the drawing

In the Onshape Drawing, right-click the view and select “Edit view.” Confirm scale is set to 1:1. If it is 1:2, your printed template will be half size and every cut will be wrong. This is the most common PDF workflow error.

Export as PDF — no center marks, no title block scaling

In the drawing, click Export → PDF. In the export settings: uncheck center marks if they appear, set paper size to match your drawing sheet (A or B), and confirm “Fit to page” is OFF. “Fit to page” rescales the drawing to fill the paper and destroys the 1:1 ratio — turn it off.

“Fit to page” is the silent killer of this workflow. The PDF looks correct on screen but prints at the wrong size. Always print a test piece with a known dimension (say, a 1.000” square) and measure it with calipers before cutting your material.

Print with “Actual Size” / “100%” in the printer dialog

Open the PDF in Adobe Reader or Chrome. In the print dialog, set scale to “Actual size” or “100%” — never “Fit to page.” Print on standard paper first. Measure a known dimension on the printout with a ruler or calipers before cutting anything.

Verify print scale with a known dimension

On your printout, find a dimension you know — for example a 1.000” square you drew for this purpose, or the distance between two holes (e.g., 1.500”). Measure it on the paper with calipers. If it reads anything other than the exact dimension, your print settings are wrong. Fix before cutting.

Add a calibration box to every fab drawing. Draw a 1.000” × 1.000” square in the corner of every template. Label it “VERIFY: this square = 1.000””. This takes 30 seconds and catches scale errors every time.

Tape to material and cut

Use painter’s tape or spray adhesive to attach the paper template firmly to the Delrin sheet — no bubbles or wrinkles. For straight cuts: use a straight edge and mark the cut line with a scribe or fine marker before sawing. For holes: use the printed center to punch a starting point, then drill. Drill Delrin at medium speed with a sharp bit — it melts and gums up if the bit is dull or spins too fast.

Deburr and verify

After cutting, remove the paper template. Deburr all edges and hole rims with a deburring tool or fine file. Measure critical dimensions with calipers and compare to the Onshape drawing. If any dimension is off by more than 0.030”, decide whether it matters: hole position tolerance for VEX structure is forgiving (the holes are 0.201” diameter in 0.201” clearance holes), but a motor shaft bore needs to be within ±0.005”.

✅

Delrin drilling tips: Use a fresh high-speed steel or cobalt bit. Drill speed: 500–1000 RPM for 1/4” Delrin. Back the drill out every 1/4” to clear chips. Delrin chips look like small curls — if you see powder or smoke, the bit is too dull or too fast. No coolant needed. Clamp the material — never hold plastic freehand while drilling.

3 / 8

// Section 04

DXF Workflow — X-Carve Pro (CNC Router)

The DXF workflow is strictly better than PDF for anything you need repeated, anything with curves, and all polycarbonate work. Once the setup is done, the machine cuts more accurately than any hand method. This is how you scale up.

📌 Quick Take DXF workflow = export from Onshape, send to X-Carve Pro CNC. Repeatable, precise, no manual cutting. Use whenever you need more than one of the same part or anything with curves/holes.

🖼️

    [Image Placeholder: X-Carve CNC setup — part on spoilboard, DXF toolpath shown on screen, finished cut part beside machine]

🔄

What is DXF? DXF (Drawing Exchange Format) is a vector file that carries exact geometry — lines, arcs, circles — as coordinates. Unlike a PDF (which is a visual snapshot), a DXF file is machine-readable. The X-Carve software reads the DXF and converts it directly to toolpaths. No printing, no taping, no measuring by eye.

Getting the DXF Out of Onshape

Export DXF directly from the Part Studio sketch — NOT from the Drawing

This is the most important distinction. Open the Part Studio with your custom part. In the feature tree, right-click the sketch (not the extrude — the sketch itself) and select “Export as DXF/DWG.” Export as DXF format. This exports the flat 2D profile of your part — exactly what the X-Carve needs.

Why sketch, not drawing? Exporting from the Drawing adds dimension lines, title block text, and annotation geometry into the DXF. The CAM software will try to cut all of it — including your dimension arrows. Always export from the sketch for machining.

Check the DXF before importing to CAM

Open the exported DXF in a free viewer: LibreCAD (free, desktop) or drag it into Autodesk Viewer online. Confirm: the part outline looks correct, all holes are present, there are no stray lines, and the overall dimensions match your Onshape model. A 5-second check saves a wasted cut.

Import DXF into Easel (X-Carve’s software)

In Easel (easel.inventables.com), click File → Import → DXF. The part profile will appear on the workpiece canvas. Verify the dimensions in Easel match your design — Easel shows the bounding box in the shape panel on the right.

Units check: Onshape exports DXF in inches by default when your document is set to inches. If Easel imports your 3” × 2” plate as 76.2mm × 50.8mm (the millimeter equivalent), your units are consistent — just confirm Easel is set to inches or millimeters to match. If the part imports as 3mm instead of 3”, the unit setting in the DXF export was wrong — re-export with inches selected.

Set cut depths and toolpaths in Easel

For each shape in Easel, set:

Depth: Slightly more than your material thickness. For 0.250” Delrin: set to 0.270” (0.020” into the spoilboard). For 0.125” poly: set to 0.140”.
Cut type: “Outside the line” for the outer profile (the machine removes material outside your part). “Inside the line” for holes (the machine removes material inside the hole circle).
Profile vs Pocket: Use “Profile” (outline cut) for holes and outer shape. Use “Pocket” only if you are machining a recess or flat-bottom slot.

Set feed rate and bit for the material

Material	Bit	Feed Rate	Depth per Pass	Notes
Delrin 1/4”	1/8” single-flute upcut spiral	60–80 in/min	0.060” per pass	Hold-down tabs essential. Delrin melts and rewelding chips is common — keep feed rate up to clear chips.
Polycarbonate 1/8”	1/8” single-flute upcut spiral	50–70 in/min	0.040” per pass	Poly melts easily. Slow spindle speed helps. Remove protective film before cutting — it catches and tears.
Polycarbonate 3/16”	1/8” single-flute upcut spiral	40–60 in/min	0.040” per pass	More passes needed. Check clamps halfway through — vibration can loosen thicker material.

Add hold-down tabs in Easel

Tabs are small bridges of uncut material that hold the part to the stock sheet during cutting. Without tabs, the part lifts when the last cut completes and the bit grabs it — ruining the part and potentially breaking the bit. In Easel, enable “Tabs” in the cut settings. For a part up to 6” long, use 2–3 tabs. Tabs are typically 0.020” tall × 0.060” wide. Remove them with a flush-cut saw or sharp chisel after the job.

Zero the machine and run a test cut in MDF or scrap

Before cutting your actual material, run the toolpath on a piece of scrap MDF or scrap poly at the same thickness. This confirms: the part is the right size, holes are in the right place, and no tabs are missing. This costs 5 minutes and saves a sheet of material that costs $15–$40.

First-time setup on the X-Carve Pro: Home the machine, zero X/Y to the front-left corner of your material, and zero Z to the top surface using the Z-probe or paper method. Check with your mentor — the school may have a specific zeroing procedure for the machine.

⚙️

Nesting multiple parts on one sheet: In Easel, you can import multiple DXF files and arrange them on the same workpiece to minimize material waste. Cut inner profiles (holes) first, then outer profiles. This is how professional shops reduce material cost — and it directly ties to “resource management” in your engineering notebook.

You exported a DXF from Onshape and imported it into Easel, but your 3.000” × 2.000” part appears as 76.2 × 50.8 in Easel. What happened and what do you do?

The DXF is corrupted — re-export from scratch

Easel is interpreting the inch dimensions as millimeters (76.2mm = 3”). Switch Easel’s units to inches, or set the import unit to “inches” — the geometry is correct, only the unit display is wrong.

The Onshape model is wrong — the sketch dimensions need fixing

Easel cannot open Onshape DXF files — use a different CAM program

4 / 8

// Section 05

Tolerances — How Tight Is Tight Enough?

Not every dimension on your part needs the same precision. Knowing which dimensions are critical — and by how much — lets you choose the right cutting method and spot problems before assembly.

📌 Quick Take Three tolerance tiers: critical (mating holes, ±0.005″), important (general fit, ±0.020″), cosmetic (outline, ±0.060″). Tighten only what matters — over-spec wastes time.

VRC Tolerance Reality Check

Feature	Required Tolerance	Achievable by…	Why It Matters
VEX structural hole position	±0.030” (0.76mm)	Hand cut + drill, PDF template, X-Carve	VEX holes are slightly oversized — generous clearance. Screw goes through with room to adjust.
Bearing bore diameter	±0.002” (0.05mm)	X-Carve with sharp bit, or drill press only	Bearing must press-fit snugly. Too loose = bearing spins in mount. Too tight = cracks Delrin.
Motor shaft clearance hole	±0.005” (0.13mm)	X-Carve or drill press	Shaft must pass through without binding or wobbling.
Outer part boundary	±0.020” (0.5mm)	All methods	Edge position affects fit within the robot frame but rarely critical to 0.001”.
Tab removal smooth finish	Visual — no snag	File + sandpaper	Tab stubs that stick up will interfere with mating parts and are a safety concern on moving assemblies.

⚠️

Bearing bores are the one dimension you cannot hand-drill to tolerance. A 0.500” VEX bearing flat bore needs to be within ±0.002” — that is two thousandths of an inch. A freehand drill is ±0.015” on a good day. Use the X-Carve for any custom plate that carries bearing flats, or use a drill press with a correctly sized reamer after drilling.

Bit Size vs Hole Size in the DXF

The X-Carve cuts the center path of the bit along your DXF line. This means the actual cut opening is wider than your DXF line by half the bit diameter on each side. For a 1/8” (0.125”) bit:

A 0.201” VEX clearance hole in your DXF will be cut to 0.201” + (0.125” / 2 × 2) = 0.326” if you use “On the line” in Easel — way too big.
Using “Inside the line” in Easel compensates: the bit center path is moved inside by half the bit diameter, giving you a hole close to your DXF nominal.
For critical bores, design the hole in Onshape 0.005” smaller than your target, cut with “Inside the line,” then test-fit and enlarge with a reamer if needed.

💡

Always cut holes first, then the outer profile. If the holes are cut last and something shifts during cutting, the part is already detached. Cut holes while the stock is still clamped firmly, then cut the outer profile to release the part.

⚙ STEM HighlightManufacturing Engineering: Tolerances and Fits

The formal engineering system for specifying how much a dimension can vary is called GD&T — Geometric Dimensioning and Tolerancing. It defines not just size tolerances but also form (flatness, roundness), orientation (perpendicularity, angularity), and location tolerances. In industry, a bearing bore is often specified as an H7/p6 interference fit — a standardized fit that produces a predictable press-fit force. For VRC, you don’t need full GD&T — but understanding that different features need different tolerances is the same mental model NASA and automotive engineers use every day. When you specify “VEX clearance hole ±0.030”, bearing bore ±0.002”” on your fab notes, you are doing engineering-grade documentation.

🎤 Interview line: “We specify tolerances on our custom parts based on the functional requirement of each feature. Clearance holes for VEX screws can be ±0.030” — the VEX hole pattern is forgiving. Bearing bores need ±0.002” for a proper press fit. This is the same tolerance analysis engineers use in industry — you match the precision of the process to the precision the function actually requires.”

5 / 8

// Section 06

Pre-Cut Checklist

Run through this before every cut — PDF or X-Carve. Each item prevents one specific type of failure.

📌 Quick Take Pre-cut checklist prevents one of three failure modes. Wrong material thickness, wrong file orientation, missing kerf compensation. Each takes 30 seconds to check, hours to recover from.

📷 PDF / Hand Cut

⚙️ DXF / X-Carve

Notebook Evidence from Fabrication

Onshape drawing screenshot with all dimensions annotated — goes in the “Build” EDP phase entry for this part.
Photo of finished part with calipers on a critical dimension — proves the manufactured part matches the design. Write the measured value next to the photo in the notebook.
Easel screenshot showing toolpath (for X-Carve jobs) — shows the machine setup was intentional and documented, not guessed.
Material spec note — “Delrin 1/4”, white, cut 2025-03-15” — so any inspector or judge can trace the provenance of the part.
Before/after robot photo showing the custom part installed — CAD design → fabrication → installed. This chain of evidence is what Expert-level notebooks show.

Related Guides

🔧

CAD to Build Handoff

BOM, screw plan, fab notes overview

⚙️

Mechanism Concept Sprint

▶ CAD Track Complete

You’ve completed the full Onshape track. Now apply what you built — go to competition preparation and make sure your robot is legal and ready.

🚫 Robot Inspection Guide →

Design the part before you cut it

📝

Engineering Notebook

EDP phases, evidence documentation

💻

Onshape Setup

dusd.onshape.com, documents, library

🔬 Check for Understanding

You export a DXF from Onshape for X-Carve cutting. The cut part is 2mm larger than your CAD dimensions on every edge. What's the most likely cause?

The X-Carve is miscalibrated and needs a full re-calibration sequence

The DXF export used the wrong unit (inches vs mm)

The toolpath wasn't set for inside/outside cut — the bit is cutting on the wrong side of the line, adding one full bit radius to each edge

Delrin expands after cutting due to heat from the bit

Correct. A consistent oversize on all edges is the classic sign of wrong cut direction (inside vs outside path). The bit has a physical diameter — if it cuts outside the line instead of inside, every edge gains one full bit radius (~1mm for a 2mm bit). Fix the toolpath setting in Easel/Carbide Create, not the CAD. Document the correct toolpath settings in your Orange fabrication slides so the next cut is right immediately.

6 / 8

// Section 07

Sourcing & Inspection — Override R24

Where custom plastic comes from, how to verify a vendor product is legal, and how to pass inspection without surprises. Override changed the rule structure from previous seasons — if you remember the "single 12″×24″ sheet" framing, you're thinking of the old rule.

📌 Quick Take VRC legal plastics: HDPE, polycarbonate, ABS, Delrin/POM, acrylic. Source from major suppliers (Robosource, ApplyDC) or local plastics distributors. Verify the spec sheet matches V5RC R7 before cutting.

📋

Override v0.1 manual rule R24 — the structural change. Push Back (R18) said you could use plastic "cut from a single 12″×24″ sheet up to 0.070″ thick." Override (R24) replaced that with: up to 12 individual pieces, each no larger than 4″×8″×0.070″. Returning students who remember the old rule will get tripped up on inspection. Brief everyone on R24 before their first build session.

What Override R24 Allows

📋 R24 Plastic Allowance

Maximum 12 individual pieces per robot — counts both functional parts AND non-functional decorations
Each piece ≤ 4″ × 8″ × 0.070″ (no piece may exceed any of these three dimensions)
Mechanical alterations only — cutting, drilling, bending. Heating to aid in bending is OK.
Cannot chemically treat, melt, cast, or bond plastic to another part
3D printed parts are not legal for any purpose — including non-functional decorations
Plastic sheets sold by VEX (e.g., 276-8340 PET Sheets) count as custom plastic and are subject to R24

Legal Plastic Types per R24e

The Override manual lists these as legal non-shattering plastics. Read your vendor's product spec sheet to confirm the material is one of these — not just a generic "plastic" description.

Material	Common Name(s)	VRC Use
Polycarbonate	Lexan	Side panels, leaf springs, intake guards (do not laser cut)
Acetal monopolymer	Delrin (DuPont trade name)	Brackets, motor mounts, gear guards, bearing supports
Acetal copolymer	Acetron GP	Functionally similar to Delrin; usually cheaper
POM	Acetal	Generic acetal — same family as Delrin
ABS, PEEK, PET, HDPE, LDPE, Nylon (all grades), Polypropylene, PTFE, FEP	various	Niche uses; most teams use Delrin or polycarbonate

❌

Shattering plastics are prohibited per R24f: PMMA (also called plexiglass, acrylic, or perspex). Acrylic looks like polycarbonate but cracks under impact — never substitute it. If a vendor lists a sheet as "acrylic," it is not legal regardless of price or appearance.

What to Look for on a Vendor Listing

Before recommending any vendor product to your coach, check the product description against these criteria:

✅ Vendor Listing Checklist

Material name matches R24e. Look for "acetal monopolymer," "Delrin," "acetal copolymer," "Acetron," "POM," or "polycarbonate." Reject listings that just say "plastic" or "PVC" (PVC is not on the legal list).
Thickness ≤ 0.070″ (1.78mm). Common stocked thicknesses: 1/16″ (0.0625″) is fine, 1/8″ (0.125″) is too thick. Watch for vendors selling 1/4″ (0.25″) Delrin — this is common in industrial supply but exceeds R24's 0.070″ limit. You will need to confirm the listed thickness is ≤ 0.070″.
Sheet size ≥ 4″×8″ per piece you need to cut from it. A 12″×12″ sheet gives 3 maximum-size pieces; a 12″×24″ sheet gives 9. Buy enough that you have spares for fabrication errors.
Color is documented. White Delrin and natural Delrin are usually the same material (different finishing). Black Delrin is filled with carbon — still acetal monopolymer, still legal, but inspection benefits from being able to read marker tracings on lighter colors.
Vendor provides a spec sheet or material certification. Even a basic product page that names the polymer counts. Avoid listings that don't name the material specifically.

📝

Why white Delrin is usually the right choice for VRC. Lower cost than colored or filled Delrin. Easier to mark with pencil or sharpie when laying out cuts. Easier to spot cracks, wear, and impact damage during competition repairs. Inspection-day tracings show clearly. Black Delrin is fine but loses these advantages.

Documentation Requirements (R7)

Per R7: "Teams are responsible for providing documentation proving a part's legality in the event of a question. Examples of documentation include receipts, part numbers, official VEX websites, or other printed evidence."

For custom plastic specifically, this means:

Keep the vendor receipt with the material spec on it. PDF, paper, or screenshot — bring it to inspection if asked.
Keep the spec sheet (often a separate PDF download from the vendor product page). This is what a head referee will want to see if there's any doubt about whether the material is on the R24e list.
Label your sheets with the material name and thickness if you have multiple types in your build space. A box marked "1/16″ white Delrin" is faster to verify at inspection than "assorted plastic."

Inspection-Day Workflow

What happens at inspection for custom plastic:

Inspector counts the pieces. They may use a dry-erase marker on each piece as they count. Maximum is 12.
Inspector verifies size limit. Each piece must fit within 4″×8″×0.070″. They will measure if anything looks borderline.
Inspector may ask for 1:1 tracings. If a piece is complex (curved, irregular), present a 1:1 scale tracing showing the original cut shape. Diagonal cuts across an 8″ dimension — especially "diagonal across a 4″×8″ sheet to gain length" — may require more evidence per the R24 inspection note.
Documentation question. If asked "what material is this?" you should be able to name the polymer (Delrin / acetal monopolymer / polycarbonate, etc.) and produce the receipt or spec if requested.

💡

Pre-pack the inspection envelope. Put the vendor receipt(s), spec sheet(s), and 1:1 tracings of each plastic piece in one folder. Bring it to every event. This is also Notebook evidence (orange Build slide) — document where each custom part came from.

Common Inspection Failures

Failure	What Happened	Fix Before Inspection
13+ pieces counted	Forgot a non-functional decoration counts as a piece	Remove decorations or consolidate functional pieces
Piece exceeds 4″×8″	Old "12″×24″ sheet" thinking from Push Back	Cut the piece down to fit the new R24 limit
Thickness exceeds 0.070″	Bought 1/8″ Delrin instead of 1/16″	Replace with thinner stock; can't machine 1/8″ down on inspection day
Material is acrylic, not polycarbonate	Visual confusion — both are clear and rigid	Replace entirely. Acrylic is prohibited per R24f.
3D printed bracket on robot	Confusion about decoration vs functional	Remove the part. Override prohibits 3D printed plastic for any purpose.
No documentation when asked	Lost the receipt / spec sheet	Email the vendor for a copy — most will resend the order confirmation

Procurement Process for Spartan Design Teams

🏫

Students: do not order plastic yourself. Procurement is handled by Coach Tansopalucks through Downey USD-approved vendors. Bring vendor recommendations to your coach with the spec sheet attached — not a link to checkout. The coach owns the purchasing relationship; you own the spec verification.

The right workflow for a student who needs custom plastic:

Identify the part you need from your Onshape model. Print the drawing with dimensions.
Check R24 compliance. Is the planned piece ≤ 4″×8″×0.070″? Does the team have < 12 pieces total including this one? If not, consolidate or substitute.
Find a candidate vendor product. Look at the spec sheet. Confirm material name appears in R24e and thickness is ≤ 0.070″.
Submit a procurement request to Coach Tansopalucks. Include: part name, dimensions, vendor product link, spec sheet PDF, quantity needed, intended robot purpose.
Coach reviews and orders through DUSD-approved purchasing. Plastic arrives 1-2 weeks later depending on vendor.
Save the receipt and spec sheet to the team's shared documentation folder for inspection-day reference.

🎯

This is a real engineering process moment. Real engineers don't buy parts directly — they submit purchase requests with material specs to the procurement team. Practicing this now (with the coach as the procurement team) is exactly the workflow you'll see in any engineering job. Document the full procurement decision (alternatives considered, spec verification, why this material) in your Orange (Build) notebook slides.

For Returning Students — What Changed from Push Back

If you built custom plastic parts in Push Back (2025-26), here's what to unlearn for Override:

Push Back R18	Override R24	What This Changes
Single 12″×24″ sheet, 0.070″ max	12 pieces, each ≤ 4″×8″×0.070″	Can't cut a 10″×20″ piece anymore even though it'd fit the old "12×24 sheet" outline. Each piece is now individually capped at 4×8.
Inspector verified piece outline fits puzzle-back into 12″×24″	Inspector counts pieces and measures each one	Less geometric puzzle-fitting at inspection; more straightforward piece-by-piece measurement.
3D printed prohibited (same)	3D printed prohibited (same)	No change. Don't bring 3D printed parts to either season.
Acrylic prohibited (same)	Acrylic prohibited (same)	No change.

The practical effect: large structural panels are harder to make legal in Override. A 6″×10″ bracket that fit Push Back's rule is too long for Override. Plan part sizes around the new 4″×8″ cap from the start — don't design a part and then discover it's illegal.

7 / 8

For Coaches & Mentors

Manufacturing vocabulary, discussion questions, and the official PTC/Onshape Manufacturing unit guide.

📌 Quick Take Coach reference: vocabulary list, questions to ask students (why this material? why this tolerance? why this workflow?), and the PTC manufacturing unit for formal teaching.

⚠️

Prerequisite note from PTC: This unit is recommended for students who have completed the Creating Custom Components unit or have already done some Onshape modeling. Focus on the manufacturing sections that match your team's available equipment.

Key Vocabulary

These terms cover all three manufacturing types — 3D printing, laser cutting, and CNC. Focus on the terms that match what your team actually uses.

3D Printing

Building a physical object from a digital model by depositing material in layers. FDM (Fused Deposition Modeling) is the most common type used in robotics.

Slicing

Converting a 3D model into printer instructions. Software like Cura or PrusaSlicer generates the layer-by-layer toolpath the printer follows.

STL

Standard Tessellation Language — the file format exported from Onshape for 3D printing. Contains the surface geometry of the part as triangles.

Laser Cutting

Uses a focused laser beam to cut or etch flat materials. Fast and precise — great for polycarbonate brackets, Delrin parts, and acrylic panels.

Kerf

The width of material removed by the laser beam. Typically 0.1–0.3mm — account for kerf when designing parts that need to fit together precisely.

DXF

Drawing eXchange Format — a 2D vector file exported from Onshape for laser cutters and CNC routers. The universal format for flat part cutting workflows.

CNC

Computer Numerical Control — uses pre-programmed code to control a cutting tool's position and speed. Enables repeatable, precise parts from plastics and metals.

Additive vs. Subtractive

Additive (3D printing) builds up material. Subtractive (CNC, laser) removes material from stock. Each has different design rules and tradeoffs.

Tolerance

The permissible range of variation in a dimension. A hole designed at 0.170" with ±0.005" tolerance will fit an #8-32 screw even if the drill or laser is slightly off.

Prototyping

Building samples to test a concept before committing to final materials. 3D printing is ideal for prototyping — fast and cheap — even if the final part will be machined.

STEP

A 3D file format exported from Onshape for CNC CAM programs. More complete than STL — preserves exact geometry and is widely supported by CAM software.

Fixturing

Any device used to hold your workpiece while machining. Proper fixturing is critical for CNC — a part that shifts mid-cut is ruined and potentially dangerous.

Discussion Questions

3D Printing

When prototyping, what matters more — print speed or part strength? What about for competition-day parts?
What is the size of your printer bed? Which robot parts exceed that limit?

Laser Cutting

What materials will you use for prototyping? For final competition parts?
What kinds of robot parts make the most sense to design for laser cutting?
What materials can you NOT put in a laser cutter? (Hint: PVC, vinyl, and anything with chlorine)

CNC Routing & Milling

What parts are best suited for your router vs. your mill?
Who on the team is trained and authorized to use these machines?
What are the working envelope dimensions of your machines?

Official PTC/Onshape Resources

📚 Unit Guide — PTC / Onshape

Manufacturing

Full instructor guide covering 3D printing, laser cutting, and CNC — design considerations, export workflows, and discussion questions for each.

🔗 PTC Resource Center →

🛠 Design for Digital Fabrication

Onshape Article

PTC's guide to designing parts in Onshape specifically for digital fabrication — laser cutting, 3D printing, and export workflows.

🔗 Read Article →

🎓 Design for Manufacturing

Classroom Resource

PTC's classroom-focused guide on design for manufacturing — how to think about fabrication constraints from the start of the design process.

🔗 Read Guide →

8 / 8