Type a tolerance callout and get back the cheapest process that actually holds it, the process chain if it needs more than one operation, what it multiplies the cost of that feature by, and which of four things is really governing: process capability, part stiffness, material stability, or thermal growth. It also writes the note you send the engineer. Feasibility is not one number, so nothing here is presented as one.
Last updated July 2026
This is achievable. It is not free. It needs Reamed rather than standard Bored or helically interpolated on a machining center, which is a real operation with a real price, not an impossibility. Say so that way to the engineer.
| Constraint | Floor it puts under the callout (in) | Percent of the allowance | Governing |
|---|---|---|---|
| Process capability | 0.00050 | 100% | yes |
| Part stiffness | 0.00036 | 72% | - |
| Material stability | 0.00032 | 65% | - |
| Thermal growth | 0.000065 | 13% | - |
Material stability eats up to 65% of the allowance before machining error is counted. Remove stock symmetrically and rest the part between roughing and finishing.
Part stiffness warning. At a span to thickness ratio of 24 the part flexes under the cutter, the clamp and its own weight. The part is too thin for the span the callout controls. Thicken it, add ribs, control the callout over a shorter length, or grind it on a magnetic or vacuum chuck with the full area supported. If the feature only has to be flat when bolted down, say that on the print and toleranced it in the restrained state per ASME Y14.5.
| Process | Capability here (in) | Typical Ra (uin) | Holds your callout |
|---|---|---|---|
| Drilled, as-drilled size | 0.0050 | 63 to 125 | no |
| Bored or helically interpolated on a machining center (routine) | 0.0020 | 32 to 63 | no |
| Reamed | 0.00050 | 32 to 63 | yes, cheapest |
| Fine bored with an adjustable head | 0.00030 | 16 to 32 | yes |
| Jig ground | 0.00010 | 4 to 16 | yes |
| Honed or lapped to a master | 0.000050 | 1 to 8 | yes |
Bilateral tolerances in inches on a nominal around 0.500 to 1.000 inch, and Ra in microinches. Figures are the commonly published ranges from design-for-manufacturability process capability charts and shop capability sheets. Sources disagree by roughly a factor of two at the tight end, so every row is a range and the relative cost column is a band. Relative cost is the machining cost of that one feature against a standard CNC milled baseline at the same quantity, not the cost of the whole part, and not a quote.
| Process | Typical achievable tolerance (in) | Typical Ra (uin) | Relative cost | When to reach for it |
|---|---|---|---|---|
| Band sawing, cut to length or thickness | plus or minus 0.020 to 0.030 | 250 to 1000 | 1.0x | Stock cutting. Always leave a machining allowance, never call a sawn face a finished dimension |
| Rough milling, hogging passes | plus or minus 0.010 | 125 to 250 | 1.0x | Getting close to size fast before anything is toleranced |
| Standard CNC milling | plus or minus 0.005 | 63 to 125 | 1.0x baseline | The default for machined surfaces and for anything inheriting the title block tolerance |
| Precision CNC milling, light finish pass | plus or minus 0.001 to 0.002 | 32 to 63 | 1.5x to 3x | Slip fits, bearing seats, mating faces, anything that has to assemble without a file |
| Drilling, as-drilled hole | plus 0.005 / minus 0.001 | 63 to 125 | 1.0x | Clearance holes only. Drills cut oversize and wander, so never call a drilled hole a bore |
| Turning | plus or minus 0.002 | 63 to 125 | 1.0x | General outside diameters, shoulders and faces |
| Precision turning, sharp insert finish pass | plus or minus 0.0005 | 32 to 63 | 1.5x to 3x | Press fits, seal diameters, bearing journals on non-hardened parts |
| Reaming | plus or minus 0.0005 | 32 to 63 | 1.4x to 2.5x | The cheapest honest way to hold a bore under a thou, if the size is a standard reamer size |
| Fine boring, adjustable head | plus or minus 0.0002 to 0.0003 | 16 to 32 | 2x to 4x | Bores at a size no reamer exists for, or a bore that must be concentric to the setup |
| Jig boring | plus or minus 0.0002 to 0.0005 | 16 to 32 | 3x to 6x | Hole-to-hole location under a thou across a plate |
| Wire EDM, with skim passes | plus or minus 0.0002 to 0.0005 | 40 to 125 as-cut, 16 to 32 with skims | 3x to 8x | 2D profiles, narrow slots, sharp internal corners, and thin or delicate parts with no cutting force |
| Surface grinding | plus or minus 0.0002 | 8 to 32 | 3x to 6x | Thickness, flatness and parallelism on a part rigid enough to chuck flat |
| Cylindrical or OD grinding | plus or minus 0.0002 | 8 to 16 | 3x to 6x | Round, straight and concentric outside diameters |
| Jig grinding | plus or minus 0.0001 | 4 to 16 | 6x to 15x | Located bores held under two ten-thousandths on size and position together |
| Honing | plus or minus 0.0001 to 0.0002 | 4 to 16 | 4x to 8x | Bore size, roundness and finish in one operation, especially on long bores |
| Lapping | plus or minus 0.00002 to 0.0001 | 1 to 8 | 10x to 30x | Gage-grade size and flatness. Hand work, one part at a time, against a certified master |
Geometric tolerances are not size tolerances. A flatness or parallelism zone gets harder to hold as the controlled span grows, so capability is a base plus a rate per inch of span. Rows 1 to 6 are flatness. The last six rows are perpendicularity, parallelism and profile of a surface for comparison. All figures are TOTAL zones, not plus or minus. They assume a part rigid enough that its own flexibility is not the limit, which is exactly the assumption the calculator above checks with the span-to-thickness rule.
| Callout and process | Capability rule | 2 in span | 6 in span | 12 in span |
|---|---|---|---|---|
| Sawn surface | 0.008 + 0.0020 per inch | 0.012 | 0.020 | 0.032 |
| Standard CNC milled | 0.0010 + 0.00050 per inch | 0.0020 | 0.0040 | 0.0070 |
| Precision milled, fully supported | 0.0005 + 0.00025 per inch | 0.0010 | 0.0020 | 0.0035 |
| Surface ground on a chuck | 0.0002 + 0.00008 per inch | 0.00036 | 0.00068 | 0.00116 |
| Ground, rested and reground | 0.0001 + 0.00004 per inch | 0.00018 | 0.00034 | 0.00058 |
| Lapped | 0.00005 + 0.00002 per inch | 0.00009 | 0.00017 | 0.00029 |
| Perpendicularity, milled one setup | 0.0010 + 0.00070 per inch | 0.0024 | 0.0052 | 0.0094 |
| Perpendicularity, ground on a sine plate | 0.0002 + 0.00010 per inch | 0.00040 | 0.00080 | 0.00140 |
| Parallelism, milled both faces | 0.0015 + 0.00060 per inch | 0.0027 | 0.0051 | 0.0087 |
| Parallelism, surface ground both faces | 0.0002 + 0.00010 per inch | 0.00040 | 0.00080 | 0.00140 |
| Profile, 3-axis milled from CAM | 0.0040 + 0.00080 per inch | 0.0056 | 0.0088 | 0.0136 |
| Profile, wire EDM or form ground | 0.0004 + 0.00010 per inch | 0.00060 | 0.00100 | 0.00160 |
Computed at 13.1 microinch per inch per degree F, which is the handbook value for both 6061 and 7075 over the 68 to 212 degree F range, and about 13.1 for 5000 series cast tool and jig plate. Published 7050 figures run from about 12.8 to about 13.2 depending on the source and the temperature range, so it is thermally the same material as 7075 for this purpose and the calculator uses the low end. Dimensional measurement standards reference 68 degrees F, so any dimension measured at a different temperature carries this error before anyone has made a mistake. A steel micrometer or gage block grows at only about 6.4 microinch per inch per degree F, so the differential between an aluminum part and a steel gage is roughly 6.7 microinch per inch per degree F, about half the numbers below. Compare the relevant row against the tolerance band on your print. If the growth is a large fraction of the band, the callout is inside the noise of the shop.
| Length or span (in) | Growth over 5 deg F | Growth over 10 deg F | Growth over 20 deg F |
|---|---|---|---|
| 0.500 | 0.000033 | 0.000066 | 0.000131 |
| 1.000 | 0.000066 | 0.000131 | 0.000262 |
| 2.000 | 0.000131 | 0.000262 | 0.000524 |
| 4.000 | 0.000262 | 0.000524 | 0.001048 |
| 6.000 | 0.000393 | 0.000786 | 0.001572 |
| 8.000 | 0.000524 | 0.001048 | 0.002096 |
| 12.000 | 0.000786 | 0.001572 | 0.003144 |
| 18.000 | 0.001179 | 0.002358 | 0.004716 |
| 24.000 | 0.001572 | 0.003144 | 0.006288 |
| 36.000 | 0.002358 | 0.004716 | 0.009432 |
| 48.000 | 0.003144 | 0.006288 | 0.012576 |
All lengths are in inches, tolerances in inches, stresses in psi, temperatures in degrees F. T is the requested tolerance: plus or minus for a size feature, total zone for a geometric callout.
D nominal size of the feature. S the part's longest dimension or the span the callout controls. t the thinnest wall or thickness anywhere in the part. base_i and rate_i the published capability of process rung i and, for geometric callouts, how fast it degrades per inch of span.
SIGMA_R indicative peak core residual stress in the stock, 1,500 psi for 6061-T651, 3,000 for 7075-T651, 1,800 for 7075-T7351, 2,000 for 7050-T7451 and 300 for 5000 series cast tool and jig plate. These are indicative figures, not spec values, and no mill certifies them. E elastic modulus, 10.0e6 psi for 6061, 10.4e6 for 7075, 10.3e6 for 7050 and for cast tool plate. The S^2 / t form comes from the plate warp beam model: released curvature scales as SIGMA_R divided by (E times thickness), and bow over a span scales with the square of the span.
w_m and w_s weight how much stability and stiffness actually reach the feature. A geometric callout across the whole part gets the full effect, w = 1.0. A length between features gets 0.50 for stability and 0.25 for stiffness. A thickness dimension gets 0.30 and 0.35. A local size feature such as a hole diameter, an outside diameter or a slot width gets 0.10 to 0.20, because a bow across the part barely changes a half inch bore.
r the low-force relief on the stiffness floor. Wire EDM applies no cutting force at all, and grinding, honing and lapping load the part far less than an end mill, so on a SIZE feature the part's own flexibility largely stops being the limit. That is exactly why wire EDM is the answer on thin work, and the tool sets r = 0.30 when the chosen finishing process is one of those. There is no relief on a geometric callout, r stays at 1.00, because a thin part still springs back the moment you release it from the chuck. Grinding a thin plate flat on a magnetic chuck and having it bow when you shut off the magnet is the classic version of this.
CTE 13.1 microinch per inch per degree F for 6061, 7075 and cast 5000 series tool and jig plate. For 7050 the calculator uses 12.8, the low end of a published 12.8 to 13.2 spread; the 3 percent difference never changes a verdict here, so it is stated as a range rather than as a settled figure. L_b the length the callout controls, which is the nominal size for a size feature and the span for a geometric callout or a length between features. dT the shop temperature swing. The 6.4 figure is the CTE of steel gaging.
q the quantity factor on the cost adder: 1.00 low and 1.25 high at 5 pieces or fewer, 1.00 and 1.00 from 6 to 50, 0.90 and 0.90 from 51 to 200, 0.75 and 0.80 above 200. o the second-operation factor, 1.00 when the feature stays on the same machine and 1.15 low with 1.35 high once it needs a separate machine, an extra setup and extra handling. The 1.4 to 2.0 base of the cost curve is the commonly published relationship that each halving of the tolerance past standard capability multiplies the cost of that feature by roughly 1.4x to 2.0x. The band is deliberately wide because real shop numbers vary by machine, fixture and operator, and a single invented multiplier would be worse than useless.
The verdict is ROUTINE when the required rung is at or below the standard machining rung, TIGHT when it is one rung past, VERY TIGHT when it is two or more rungs past, and NOT ACHIEVABLE BY CUTTING when either no rung holds it or the physical floor PF exceeds T. Those last two are different statements and the tool keeps them apart. No rung holding it means there is no price at which a cutting process gets you there. PF exceeding T means the machine could cut the number and the part, the material or the room cannot hold it, so the fix is a fixture, a different material or a temperature controlled bench, not a better spindle.
Everything here is guidance from published process-capability ranges. It is not a quote and it is not a capability study of any particular shop or machine. If the material-stability line is what is biting you, the fix usually starts with the stock: get an instant quote on 6061, 7075, 7050 and cast tool and jig plate cut to size, with a mill cert on every order so you know which temper you are actually holding a tolerance on.
A production CNC mill holds plus or minus 0.005 inch all day on a rigid aluminum part without anyone thinking about it. Plus or minus 0.001 to 0.002 inch is a precision finish pass with a sharp tool and a controlled fixture, and it costs real money. Plus or minus 0.0005 inch on a milled surface is at the edge of milling and usually goes to grinding instead. Below plus or minus 0.0002 inch you are grinding, jig grinding or lapping, not milling. Published capability charts disagree with each other by roughly a factor of two at the tight end, which is why this tool gives a band rather than a single number.
Because the print does not show the three things that decide whether a number is holdable. First, the process ladder: a 0.0005 inch bore is a reamer, and a 0.0002 inch bore is a jig grinder, which is a different machine, a different setup and a different price. Second, part stiffness: the same callout is routine on a solid billet and unholdable on a 0.125 inch web, because the part flexes under the cutter and the clamp. Third, material stability: plate carries residual stress from the quench, so the part moves after the cut. None of that is visible in a plus or minus symbol.
The relationship is roughly geometric, not linear. Each halving of the tolerance past what the standard process holds multiplies the cost of that feature by something like 1.4x to 2.0x, so going from plus or minus 0.005 to plus or minus 0.001 inch on a milled feature lands around 2x to 5x, and going to plus or minus 0.0005 inch lands around 3x to 10x. On top of that, once the feature needs a second machine you pay for an extra setup, extra handling and a different gage. That is the band this tool reports. It is guidance for the design conversation, not a quote.
No datums, so nobody knows what the geometric callouts are referenced to. A pile of trailing zeros, where 0.5000 inch means the CAD default rather than a real requirement. No tolerance and no title block default, so the shop has to guess. Flatness demanded on a part too thin to hold it, which is a physics problem no machine solves. A surface finish callout with no tolerance, or a tolerance with no finish callout, on a surface that has to seal. And a tolerance of zero, which is not a specification at all.
Both happen and they are different conversations. Expensive means a standard process holds it, just not the one you were planning to use: a reamer instead of an interpolated bore, a grinder instead of a mill, wire EDM instead of an end mill. Impossible means no cutting process gets there, which for aluminum starts somewhere under about 0.0001 inch on size and needs lapping to a certified master. It can also mean the part cannot hold the number even though the machine can, because the part is too flexible or the material moves after the cut. Saying impossible when you mean expensive destroys your credibility with the engineer, so name which one it is.
Yes, and it ends most arguments. Aluminum grows about 13.1 microinch per inch per degree F for 6061 and 7075. Published figures for 7050 run from about 12.8 to about 13.2 depending on the source and the temperature range, so treat it as thermally the same as 7075. Over a 6 inch part, a 10 degree F swing between the machine and the inspection bench moves the dimension 0.000786 inch. On a plus or minus 0.0005 inch callout that is 79 percent of the 0.001 inch total band, or more than 1.5 times the one-sided room you have in either direction, from temperature alone. Steel micrometers and gage blocks grow at only about 6.4 microinch per inch per degree F, so the differential between the aluminum part and a steel gage is roughly 6.7 microinch per inch per degree F. Dimensional standards reference 68 degrees F, and unless both parties measure there they will disagree about in-tolerance parts.
Because rolled and quenched aluminum plate carries a self-balancing residual stress profile, compressive at the surfaces and tensile through the core. Machine into it and the stress rebalances, and the part bends. On a thin part that movement can be several thousandths in free state, which is larger than the whole tolerance band. The machine held the number while the part was clamped and the part moved when you released it. 5000 series cast tool and jig plate is cast and thermally stress relieved rather than rolled and quenched, so it carries almost no residual stress and stays put after machining. Overaged tempers such as 7075-T7351 and 7050-T7451 are a middle ground.
Lead with the process, not with no. Tell them what holds the callout, what it multiplies the cost by, and what the two physical limits under the number are, using their own dimensions. Then ask three questions: what does the title block default say, what is the datum scheme for this feature, and does the function actually need this number. Offer the next looser standard rung with its own multiplier so they have a concrete trade to make. The note this tool generates is written to be sent as-is.
For cost purposes they are close, and confusing them is one of the most common print errors. A geometric callout such as flatness, parallelism, perpendicularity or profile of a surface is a TOTAL zone, not a bilateral tolerance. Flatness 0.002 is a 0.002 inch wide zone, which costs about the same as a plus or minus 0.001 inch size callout, not a plus or minus 0.002 inch one. This tool treats geometric inputs as total zones and size inputs as plus or minus, and labels the input accordingly.
This tool judges whether one callout is achievable by any process. It does not stack a chain of tolerances, so use the stack tolerance calculator for that. It does not predict the surface finish a given feed and nose radius will leave, so use the surface finish predictor for that. And it does not model how far your plate will actually bow after a specific cut, so use the plate warp calculator for the real number behind the material-stability line.