Custom Parts & Fabrication

// 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.

● Delrin (Acetal / POM)

Thickness: 1/4” (0.25”) most common for VRC
Color: White or black
Feel: Stiff, slippery, very machinable
How you cut it: Bandsaw, scroll saw, hand cut with coping saw, or CNC router/X-Carve
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 (no printing, no tape, higher precision)

● Polycarbonate (Lexan)

Thickness: 1/8” (0.125”) most common; 3/16” for structural panels
Color: Clear (semi-transparent)
Feel: Flexible, impact-resistant, hard to crack
How you cut it: Polycarbonate scoring tool (hand), band saw, or X-Carve router
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.
Do not use laser: Polycarbonate releases chlorine gas when laser-cut. X-Carve router only for CNC.
Best workflow: Onshape sketch → DXF → X-Carve. 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

⚠️

Do not laser cut polycarbonate. It releases chlorine gas — toxic and corrosive. Laser cutting acrylic is fine. Polycarbonate must be cut with a mechanical tool (router, saw, score-and-snap). The X-Carve is the right machine for poly CNC work.

1 / 6

// 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.

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.

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.

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 / 6

// 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.

💡

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 / 6

// 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.

🔄

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 / 6

// 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.

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 / 6

// Section 06

Pre-Cut Checklist

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

📷 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

Design the part before you cut it

📝

Engineering Notebook

EDP phases, evidence documentation

💻

Onshape Setup

dusd.onshape.com, documents, library

6 / 6