Every drawing hides a few calculations between the print and the finished part. How much stock to leave for anodize. Whether a hole that looks out of position actually passes with bonus tolerance. How much to slow the feed when an end mill circles a small bore. This guide explains the math behind each calculator above: when to use it, the formula, and the mistakes that scrap parts.
How to calculate pre-anodize and pre-plate dimensions
A drawing almost always gives the finished size, after coating. The machinist has to work backward to a pre-plate or pre-anodize dimension. Get it wrong and a bore that measured perfect before anodize won't take its gauge pin afterward.
Where the coating goes decides how much it changes the size. Hardcoat anodize (MIL-A-8625 Type III) converts the aluminum surface into oxide. Roughly half the coating grows outward and half penetrates into the base metal. A .002" hardcoat therefore adds about .001" per surface, which is .002" on a diameter. Type II sulfuric anodize is thinner, and about one third of it is build-up. Electroless nickel, chrome, zinc and most electroplating sit entirely on top of the surface, so the full thickness is build-up on every side.
The calculation must also account for the coating's own tolerance. Finishers rarely hold an exact thickness. A common callout is .003" +20% / −10%, which means the coating can land anywhere from .0027" to .0036". Averaging that range gives the mean thickness, and half the spread is the coating tolerance. The anodize and plating build-up calculator then works the worst case:
- External features (OD, width, boss): subtract the build-up. The largest pre-plate size, plus the thickest coating, must stay under the drawing maximum.
- Internal features (ID, bore, slot): add the build-up. The smallest pre-plate bore, minus the thickest coating, must stay above the drawing minimum.
That worst-case approach explains a common surprise. The pre-plate tolerance is always tighter than the finished tolerance, because the coating tolerance is taken out of it twice, once per side. If the coating range is wider than the part tolerance, there is no machinable pre-plate size at all. At that point, ask the finisher for a tighter thickness range, mask the feature, or plan to hone or grind after plating. Threads need special attention, because build-up on a thread flank changes pitch diameter by about four times the build-up per surface. Many shops run taps and thread mills oversize for anodized or plated threads.
True position: the formula and how bonus tolerance works
True position is the most-used control in GD&T and the one most often calculated wrong. The tolerance in the feature control frame is a diameter: a cylindrical zone centered on the basic, theoretically exact location. The feature's axis must fall inside that cylinder.
To check it, measure the actual X and Y of the feature, subtract the basic dimensions, and apply the Pythagorean theorem. The distance from nominal is the radius, so double it to compare against the diametral tolerance:
Forgetting the "× 2" is the classic error. It makes parts look twice as good as they are. The true position calculator takes nominal and actual coordinates directly, so you can enter CMM or height-gauge readings without doing the subtraction yourself.
Bonus tolerance is where money is saved. When the position callout carries the MMC modifier (Ⓜ), the tolerance applies only when the feature is at its maximum material condition, the smallest hole or the largest pin. As the feature departs from MMC, the difference is added to the position tolerance. A .159–.164" hole with Ø.010 position at MMC that measures .163" gets .004" of bonus, for a total of Ø.014. The physics makes sense: a larger hole leaves more clearance around its mating fastener, so it can sit further off location and still assemble.
LMC (Ⓛ) works the opposite way. It protects wall thickness and edge distance, so bonus grows as the feature moves toward the largest hole or smallest pin. RFS (no modifier) gives no bonus at all. One rule applies to all three: the feature size must be inside its own limits first. A hole that is oversize fails no matter how much bonus it would create.
Profile tolerance: finding shift versus form error
Profile of a surface and profile of a line control shape, size, orientation and location of irregular features in a single callout. With an equal-bilateral profile, the tolerance zone is split evenly around the true profile: a .030 profile on a .347 basic allows .332 to .362.
Report the measured profile the same way a CMM does: twice the worst deviation from nominal. If the extreme points are .3325 and .3645, the worst side is .0175 from nominal, so the measured profile is .035 and the part fails. The profile tolerance calculator also shows the form range, max minus min. In this example that is .032. A form range close to the tolerance tells you the shape itself is the problem. A small form range with a failing profile tells you the feature is shifted, and the calculator gives the offset needed to re-center it. That is often a quick work-offset or wear-offset fix instead of a new program.
Circular interpolation feed rate and drill speeds
CNC controls apply the programmed feed rate to the tool center. On a straight line, the center and the cutting edge move at the same speed. On an arc they don't. Inside a pocket or bore, the cutting edge travels a larger circle than the center and moves faster. Around a boss or post, the edge travels a smaller circle and moves slower.
The correction grows as the tool gets closer to the feature size. A 1/8" end mill in a .195" pocket needs about 36% of the straight-line feed. Programming the full linear feed there more than doubles the chip load at the edge, which is a common way to break small end mills in thread-mill pre-bores, counterbores and O-ring grooves. Some CAM systems apply this adjustment automatically and some don't. The circular interpolation feed calculator shows chip load per tooth before and after, so you can compare it to the tool maker's chart.
For drilling, speed starts from surface feet per minute. The drill speed and feed calculator uses RPM = SFM × 3.82 ÷ D, where 3.82 is 12 ÷ π, and IPM = RPM × IPR. Micro drills are the edge case. A .016" carbide drill at 200 SFM wants almost 48,000 RPM, which most spindles can't reach. When the machine caps the RPM, keep the feed per revolution the same and let the IPM drop. Don't push IPM up to "make up" for the lost speed. To switch between inch and metric programs, use the IPM to mm/min and chip load converter.
Don't forget the drill point. A 118° point adds about 0.3 × D of tip length, and a 135° split point adds about 0.207 × D. If the drawing calls for a full-diameter depth, add the tip length from the drill point length calculator to your Z depth. Otherwise blind holes come up short and threads run out early.
Press fits and thermal expansion
ANSI B4.1 force fits (FN1 through FN5) are hole-basis fits. The hole tolerance starts at nominal and goes up, and the shaft is made larger than the hole. FN1, the light drive fit, needs only light assembly pressure and suits thin sections, long engagement and brittle outer members like cast iron. For a .1245" nominal, FN1 puts the hole at .1245–.1248" and the pin at .1249–.1251". That gives .0001–.0006" interference. The FN1 press fit calculator gives those limits for any size up to 1.58". Check reamed holes with go / no-go gauge pins, because a bore that is .0002" oversize can turn a press fit into a slip fit.
Temperature changes size as well. Aluminum grows about 13 millionths of an inch per inch per °F. A 20" aluminum plate that is 9°F warmer than the 68°F inspection standard measures .0023" long, enough to fail a tight tolerance on a part that is actually good. The thermal expansion calculator covers common alloys and plastics. Use it for shrink fits (chill the pin in dry ice or liquid nitrogen, or heat the housing), for parts that come off the machine hot, and for plastics like acetal and PTFE, which move five times more than aluminum.
Bolt torque, material weight and right triangles
The short-form torque equation T = K × D × F links tightening torque to clamp force, also called preload. K is the nut factor: about 0.20 for dry steel threads and 0.15 to 0.18 lubricated. Lubrication matters more than people expect. The same torque on an oiled bolt can produce 10–35% more clamp force, which can strip a helicoil in aluminum or crush a thin-wall part. The bolt torque to clamp force calculator solves in both directions and includes a light-duty reference table for fixture work.
Stock weight feeds quoting, shipping and lifting decisions. Multiply volume by density: 6061 aluminum is .0975 lb/in³, steel about .284 and stainless about .289. The material weight calculator handles round bar, discs, plate and tube.
Finally, most shop geometry comes back to the right triangle: chamfer sizes, taper angles, bolt-circle hole positions, sine-bar gauge-block stacks and the X/Y deltas behind true position. Enter any two known values in the right triangle calculator to get every side and angle.
Check the numbers against the drawing
Each calculator here uses the same standard formulas found in Machinery's Handbook and the ASME Y14.5 and ANSI B4.1 standards. They are only as accurate as the inputs, so confirm the finisher's real coating range, the tool maker's recommended SFM and chip load, and the exact callouts on your drawing before cutting production parts. If a job has a tolerance stack or finish requirement you'd rather hand off, our CNC programmers and machining team handle that work every day.