Home / Guides / Design

Twelve design changes that take real money out of a machined part

August 21, 2026

Machining cost comes from time on a machine and from the risk a shop carries. Almost every design decision that raises the price does one of three things: it forces a smaller tool, it forces another setup or it forces an inspection step. Here is the list worth running before the drawing goes out.

Geometry

1. Give internal corners a generous radius. A cutter cannot produce a sharp internal corner. Every internal corner gets the radius of the tool that cut it. Specifying a small radius forces a small cutter, which means slower feeds, more passes and more time. Wherever possible make internal corner radii at least a third of the pocket depth, and use one radius throughout so the shop can cut the whole part with one tool.

2. Keep pockets shallow relative to their width. Tool deflection grows fast with length. A pocket deeper than about four times the cutter diameter needs a longer tool, lighter cuts and more passes. If a deep narrow feature exists for clearance rather than function, open it up.

3. Avoid tall thin walls. Walls thinner than about 0.8 mm in metal chatter and deflect, which means slow finishing passes and scrap. Under 0.5 mm, expect a conversation.

4. Do not ask for a flat bottomed blind hole unless you need one. A standard drill leaves a conical bottom. A flat bottom means a second tool and a second operation.

5. Limit the number of faces that carry features. Every additional face is potentially another setup. If two features on opposite faces can move to the same face without hurting function, that is a whole operation removed.

Holes and threads

6. Use standard drill sizes. A hole that matches a stock drill is one operation. A hole at an arbitrary diameter with a tight tolerance has to be drilled then bored or reamed.

7. Do not over-thread. Thread engagement beyond about 1.5 times the diameter adds nothing structurally in most materials and adds tapping time and tap breakage risk. Specify the thread depth you need, not the depth of the hole.

8. Keep thread sizes standard and few. Three different thread sizes means three taps and three tool changes. Consolidating to one size across the part is free money.

Tolerances and finish

9. Tolerance only what matters. A general tolerance of ±0.1 mm with three critical features called out costs far less than a blanket ±0.02 mm. The blanket version forces inspection of everything.

10. Match the finish to function. Ra 3.2 is what comes off the machine. Ra 0.8 needs care. Ra 0.4 and below usually needs grinding or polishing. Specify the better finish only where a seal, a bearing or a visible surface requires it.

11. Mark the datums. A drawing without datums makes the shop choose, and the shop will choose what is convenient rather than what your assembly needs. This is the cheapest single improvement you can make to most drawings.

Material and stock

12. Pick a material the shop can buy locally. Machining time can be identical between two grades while the material lead time differs by four weeks. In Vietnam, aluminium 6061 and 6063, stainless 304 and 316 and common carbon steels are on the shelf. Exotic alloys and certified heats are imported to order.

It is also worth checking how much of your block becomes chips. A part machined from solid that is 80 percent air might be better as a weldment, a casting with machined faces or a simpler two-piece design.

How to use this before a quote

Run the list, fix what is cheap to fix and leave a note in your request about what is deliberate. A line such as “corner radii are 3 mm throughout, can be larger if that helps” invites a shop to tell you something useful.

Then ask every shop that quotes for one DFM comment. The answers are a free supplier assessment: they show you who looked at the model and who dropped it into a pricing tool.

The five minute version

If you only have time for one pass over a model, look at these five things in this order. They account for most of the avoidable cost on a typical part.

Check	What good looks like	What it costs if wrong
Smallest internal corner radius	One radius, at least a third of pocket depth	Small tool, slow finishing on the whole pocket
Deepest pocket relative to that tool	Under four times tool diameter	Long tools, light passes, poor corner finish
Number of faces with features	One or two	An extra setup each
Tolerance scheme	General note plus two to five callouts	Inspection of everything, priced risk
Material and stock size	Locally stocked grade, standard thickness	Weeks of waiting or a block that becomes chips

What to do with the answers

Fix what is free, leave what is functional and tell the shop which is which. A request that says “the 2 mm corner radii are functional because of a mating part, everything else can change” gets better feedback than a request that says nothing.

Then ask each quoting shop the same question: what would you change on this drawing to make it cheaper at my quantity. Collect the answers side by side. You will usually see one feature named by every shop, and that feature is where the money is.

The companion guides on tolerances and on what drives the price of a machined part go deeper on the two items that move the number most. When the design is settled, send the drawing.

Questions we get on this

Keep reading

• What a DFM review actually changes, with the numbers
• Wall thickness, pocket depth and corner radius: the three numbers that price your part