Guides / Design
Designing a Bike Part a Shop Can Actually Cut
September 10, 2026
Two engineers can draw the same stem and get quotes that differ by a factor of two. The difference is rarely the shape. It is how many times the part has to be picked up, how deep the cutter has to reach and how small the corners are.
Here is what a machinist sees when your drawing lands.
Setups are the biggest lever
Every time a part is unclamped, turned over and re-clamped, somebody pays for fixturing, a new program and a new set of tool paths. Position accuracy between features on different faces also depends on that re-clamp, so a five setup part is both more expensive and less accurate than a two setup part.
What helps:
- Put features on as few faces as possible. If a boss can move from a side face to the top face without hurting the design, move it.
- Give the part a flat, clampable surface that is not a finished face.
- Leave a sacrificial tab or a stock area the fixture can hold, and say on the drawing where it is allowed to be.
- If the part is round, say so early. A part that can be turned on a lathe and milled once is much cheaper than the same shape milled from a block.
A part with features on four or five faces is not automatically expensive. It is expensive on a 3-axis machine. On a machine with a 4th or 5th axis it can be one setup. Shops know this. Telling them the part needs it lets them quote on the right machine.
Internal radii decide the cutter
Every internal vertical corner is cut by a round tool, so the corner has a radius whether you drew one or not. The radius you draw picks the tool.
| Corner radius | Largest sensible cutter | What happens |
|---|---|---|
| 1.5 mm | 3 mm | Slow, deflects, many passes, high tool wear |
| 3 mm | 6 mm | Workable |
| 5 mm | 10 mm | Fast, rigid, cheap |
| 6 mm and up | 12 mm | Fastest, usually invisible on the finished part |
On a stem or a brake adapter, opening every internal corner from 2 mm to 5 mm often costs nothing visually and takes a serious bite out of the cycle time.
Pocket depth and tool reach
A cutter’s stiffness falls with the cube of how far it sticks out. A pocket four diameters deep is routine. Eight diameters deep means light cuts, a slower feed and possibly a specialist tool.
Guidelines that keep quotes sane:
- Keep pocket depth under about four times the corner radius where you can
- Avoid deep narrow slots. A 3 mm wide, 20 mm deep slot is a difficult, expensive feature
- If a deep pocket is unavoidable, allow a larger corner radius at the bottom so a bigger tool can reach
Wall thickness and floor thickness
Thin walls chatter, and chatter means a poor surface and a slow cut. On aluminum, keep short walls above about 0.8 mm and tall walls above 1.5 mm, and watch the height to thickness ratio rather than the absolute number.
Pocket floors have the same problem. A large thin floor drums under the cutter. If you are removing weight from a wide area, a rib pattern is both stiffer and easier to machine than one large thin membrane.
Holes, threads and features that cost nothing to get right
- Use standard drill sizes. A 6 mm hole is a stock drill. A 6.15 mm hole is an interpolated feature.
- Keep thread depth to about 1.5 times the diameter. Deeper adds nothing to strength and risks a broken tap.
- Do not thread all the way to the bottom of a blind hole. Leave a relief.
- Chamfer the entry of every hole and thread. It is one tool, it stops burrs and it makes assembly better.
- Keep holes perpendicular to a face wherever possible. A compound-angle hole may need a 5-axis machine or an extra setup.
Tolerance only what has to fit
This is the single most common way a good design gets an expensive quote. A drawing with a default tolerance of plus or minus 0.02 mm on every dimension is a drawing that asks the shop to hold every dimension to 0.02 mm, including ones nobody will ever measure.
On a typical bike part, three to six dimensions genuinely matter: the bore that takes a steerer or a bearing, the clamp face, the bolt positions, the chainline offset. Tolerance those. Leave everything else at a general tolerance of plus or minus 0.1 or 0.2 mm. More on this in tolerances on bike part drawings.
What to send
A STEP file plus a PDF drawing. The STEP carries the geometry, the PDF carries the intent: which surfaces matter, which are cosmetic, what the finish is and where the part is allowed to be held. A shop with both will quote in a day. A shop with only a STEP file will guess, and guesses have padding in them.
Frequently asked questions
What internal corner radius should I use?
As large as the design allows, and never smaller than the radius of the smallest sensible cutter. A 2 mm internal corner forces a 4 mm or smaller end mill, which cuts slowly and deflects. Going to a 5 mm corner can cut the machining time on a pocket in half.
How thin can a wall be?
On aluminum, a rough guide is 0.8 mm for a short wall and 1.5 mm once the wall gets tall. The real limit is the ratio of height to thickness. Above about 10 to 1 the wall chatters and the shop has to slow down or add support, both of which you pay for.
Does the number of setups really matter that much?
Yes. Each setup is fixturing, a program, a tool change sequence and a new chance to lose position between faces. A part redesigned from five setups to two is often 30 to 40 percent cheaper and more accurate at the same time.
Need a quote for this part?
Send the drawing. We match you with up to 3 shops that machine bike parts and reply within 24 business hours.
Get matched with a bike parts shop