Most of what a machined part costs is decided in CAD, long before anyone sets up a vise. Two parts that look nearly identical can differ by half in price because one of them asked for something the machine has to work around. None of this is obscure - it is just rarely explained by the people quoting the job.
Here is what to send, what to put on the drawing, and the design choices that move the number most.
What to send
| Send this | Why |
|---|---|
| STEP (.step / .stp) | The universal exchange format. Reads cleanly into any CAM system and carries solid geometry faithfully. |
| Your native file too, if you have it | SolidWorks, Inventor and the rest keep feature history, which helps if we need to ask about an intent. |
| A drawing, as PDF | This is the part that governs. Tolerances, datums, finish, material and quantity live here, not in the model. |
| IGES only if that is all you have | Older surface format. It works, but surfaces sometimes arrive with gaps that have to be repaired first. |
A model on its own is a shape. A model plus a drawing is a part. If you send geometry with no drawing, everything on it is assumed to be a default tolerance, and if something on that part actually mattered, nobody finds out until it is inspected.
Tolerance only what actually matters
This is the single biggest lever on price, and the most common mistake. A blanket tight tolerance across every dimension on the page tells the shop that every feature needs slow finishing passes and full inspection, when usually two or three features do.
Call out the fits, the bores, the mating faces, and the features that locate something. Leave everything else at a sensible default. We hold ±0.001" routinely and can go to ±0.0001" on the Hardinge when a drawing calls for it, but tenths on a clearance hole costs you money and buys nothing.
The design details that cost the most
Internal corner radii
A pocket is cut by a round tool, so an internal corner can never be sharp. If you leave the corner sharp in CAD, someone has to decide what to do about it. Worse, a very small radius forces a very small cutter, which is slower, deflects more, and breaks.
Give internal corners a radius slightly larger than the cutter you expect - as a rule of thumb, a third of the pocket depth or more. A bigger radius means a bigger, stiffer tool and a faster cut. One of our customers put it better than we would have:
Great machine shop, very good communication when they find issues on drawings and where small design changes can lower the cost of the finished product, example, can you increase this radius so I can use a bigger tool to cut more material faster.
Deep pockets and thin walls
Tool deflection grows fast with reach. A pocket four times deeper than it is wide needs a long, slender tool taking light cuts, and the cost climbs accordingly. The same goes for thin walls, which chatter and push away from the cutter. If a wall can be thicker or a pocket shallower without hurting the design, it is nearly free money.
Features that need a second setup
Every face that has to be machined from a different direction means another setup: re-fixturing, re-indicating, more time, and one more chance to introduce error between features. A part that can be finished in one or two orientations is meaningfully cheaper than one needing five. If a hole on the back face could live on the side instead, ask whether it must be where it is.
Threads
Call threads out on the drawing by size, pitch, class and depth. Do not model the helix - it bloats the file and we will cut the thread with a tap or a thread mill regardless. And specify thread depth separately from hole depth, because a blind tapped hole needs room below the last full thread.
Material and finish, stated plainly
Say which alloy and temper, not just "aluminum". 6061-T6 and 7075-T6 behave differently and cost differently. Same with finish: if 16 Ra matters on one face, say so on that face. If the rest can be as-machined, say that too - it is one of the easiest places to give cost back.
Put the boring information on the drawing
- Quantity now, and quantity you expect later - it changes how we fixture and program the job
- Material and temper, with an acceptable substitute if you have one
- Surface finish where it matters, and a default for everywhere else
- Deburr and edge-break expectations
- Any inspection or documentation you need with the parts
- The date you actually need them, not a padded one
That last one matters more than people think. If a job is genuinely needed Friday we will plan around it. If every job is marked urgent, none of them are.
What happens when something is missing
We call. Every quote here is looked at by someone who will also be programming or running the part, so a question about an unclear callout gets asked before it becomes a scrap part rather than after. If a feature looks expensive for no reason, we will say that too, and suggest the change that makes it cheaper.
That is not a service we charge for. It is just faster for everyone than machining the wrong thing correctly.