Tolerances and fits for knife scales: what to call out, what to leave general

Handle a drawing to five shops and the quotes will vary by a factor of two. Most of that spread is tolerance. Not because shops disagree about difficulty, but because a drawing with forty tight callouts forces every one of them to price inspection and scrap they should not need.

Here is what actually needs to be tight on a knife scale, and what does not.

The features that control fit

Screw hole positions. This is the one. Scales bolt to a liner or a frame, and if the pattern is off, the scale sits proud on one side or the screws bind. Call out true position relative to a stated datum, typically within 0.05 mm. Positional tolerance, not plus-minus on each coordinate — the difference matters and it is cheaper to hold.

Counterbore depth. Screw heads that stand proud are the most visible defect on a finished knife. Tolerance perhaps plus-minus 0.05 mm on depth; the diameter can be looser.

Overall thickness at the mating face. Determines whether the scale sits flush. Plus-minus 0.05 mm is usually enough. Note that this is the thickness at the face, not the maximum thickness including a contour.

Any surface that indexes against the liner. If there is a step, a rebate or a locating boss, that is a fit feature. Everything else on the back face is cosmetic.

Pivot clearance bore, if present. Needs to clear, not to fit. Give it generous tolerance on the large side.

What does not need to be tight

The outer profile. The contour. The chamfer widths. The pocket depths that exist for weight reduction. The thumb ramp geometry. All of these are felt rather than measured, and none of them stack into an assembly.

Leave them to the general tolerance block. ISO 2768 medium is the sensible default and is what most shops assume when a drawing is silent — which is fine on a contour and disastrous on a screw pattern, which is precisely why you call out the screw pattern explicitly.

Why tight tolerance costs money

Four separate costs, which is why the multiplier surprises people:

1. Slower machining. Lighter finishing passes, more of them.
2. Better tooling, replaced sooner. A worn tool that still produces an acceptable cosmetic surface will not hold a tight dimension.
3. More inspection. A 0.02 mm callout usually means CMM rather than a caliper, which is time per part.
4. Scrap. Parts that would have shipped now do not.

Each of those is modest. Together they are the difference between a workable quote and one you argue with.

Datums

State one. A drawing with tolerances and no datum scheme is ambiguous, and the shop will pick a datum that suits its fixturing, which may not be the face that matters to your assembly.

For a scale, the usual choice is the flat mating face as primary and one screw hole as secondary. Say it on the drawing.

Surface finish

Ra 1.6 micrometres is a normal as-machined surface and is what most finishes go over. Ra 0.8 costs real money and is only worth it under a polish. Anything below that is not an EDC requirement.

Note that the finishing process changes the surface anyway — stonewash and bead-blast both erase the machined texture. Calling out a fine Ra on a face that will be blasted is money burned.

Matched pairs

If left and right scales must be symmetric to the eye, say so, and ask for them to be produced and inspected as a pair rather than as two part numbers. Two individually in-tolerance scales at opposite ends of the band can look visibly mismatched on the finished knife.

The rule

Call out the three or four dimensions that control assembly. Leave the rest general. State a datum. That single discipline takes fifteen to twenty percent off a typical EDC quote without changing anything a customer will ever notice. Send the drawing and we will tell you which callouts are doing nothing. Related: how to write an RFQ a shop can quote.

ISO 2768 in practice

Most EDC drawings rely on a general tolerance block whether they say so or not. ISO 2768 is the standard that defines it, and knowing the numbers helps you judge whether the default is adequate.

For linear dimensions, ISO 2768 medium (m) gives approximately:

Nominal size	Permitted deviation
0.5 to 3 mm	±0.1 mm
3 to 6 mm	±0.1 mm
6 to 30 mm	±0.2 mm
30 to 120 mm	±0.3 mm

ISO 2768 fine (f) is roughly half those values. For EDC parts, 2768-f is a reasonable default — it is well within what any competent shop holds without special effort, and it keeps the cosmetic dimensions tighter than medium without triggering inspection cost.

Write the class on the drawing: “General tolerances ISO 2768-f unless otherwise stated.” One line, and it removes an ambiguity that otherwise gets resolved by whoever is programming.

True position versus plus-minus

For a screw pattern, plus-minus tolerance on X and Y coordinates creates a square tolerance zone. True position creates a round one.

The round zone is larger in area for the same maximum error, which means the shop has more usable tolerance for the same functional result. It is both more correct and cheaper to hold. Use it for hole patterns.

A callout like “position 0.1 mm diameter, datum A-B” is more useful, more standard and less expensive than “±0.05 in X and Y”.

Tolerance stack-up

The failure that catches people: every dimension is in tolerance and the assembly still does not work.

A scale, a liner and a screw each carry tolerance. If the scale counterbore is at the shallow end, the liner at the thick end and the screw head at the tall end, the head stands proud even though nothing is out of spec.

Two mitigations:

1. Do the arithmetic before you release the drawing. Add the worst-case deviations on the features that stack and see whether the result still works.
2. Tighten only the one feature that dominates. Usually it is the counterbore depth. Tightening one dimension by half is cheaper than tightening four by a quarter.

Flatness, and why scales bow

Flatness is a form tolerance, separate from thickness. A scale can be exactly 3.00 mm thick everywhere and still be visibly curved.

It happens because material removed unevenly from rolled plate releases residual stress. The fixes are stress-relieved plate (T651 temper — see 6061 vs 7075), a stress relief operation between roughing and finishing, or machining the part symmetrically so the stress releases evenly.

If flatness on the mating face matters, call it out explicitly: “flatness 0.05 across the mating face”. Without a callout, nobody is checking it.

Threaded holes

Two things worth stating rather than assuming:

Thread class. 6H is the standard internal fit and the sensible default. Say it.

Depth of full thread versus drill depth. A blind hole has an incomplete thread at the bottom. If your screw needs five full threads of engagement, specify the depth of full thread, not the hole depth.

Writing the drawing

A workable EDC drawing has:

• A title block with part name, revision, material, finish and units
• A general tolerance note naming ISO 2768-f
• A datum scheme, usually the mating face plus one hole
• Three or four dimensions marked as critical, with real tolerances
• Everything else dimensioned but untoleranced, falling to the general block
• A note on edge condition and whether dimensions are before or after finish

That fits on one sheet and it is a complete specification. Send it with the STEP — see which CAD file to send.

FAQ

What tolerance can a good shop actually hold? Routinely ±0.02 mm on a well-supported feature with proper workholding. ±0.005 mm is achievable with CMM verification and grinding, at real cost. The question is never what is possible, it is what is worth paying for.

Should I tolerance the contour? No. Give it a profile tolerance if it genuinely matters for fit, otherwise leave it to the general block. Contour is felt, not measured.

How tight should the screw hole diameter be? Loose. A clearance hole should clear. Position is what matters, not diameter.

What if I do not know which dimensions are critical? Describe the assembly instead: “this face sits against the liner, these holes take M2 screws through to the frame”. Any competent shop will identify the critical features from that and tell you. It is a better brief than guessing at tolerances.

Does a tighter tolerance improve quality? Only on features that control function. On everything else it increases cost and scrap without changing anything a customer perceives.

Can I loosen tolerances after the first article? Yes, and it is worth doing. If the first article shows the shop is holding a dimension comfortably, loosening the callout on the production run can reduce inspection cost. Ask.