? Help · how to use
1. Pick a thread. Tap the size and start typing — 1/4-20, m6, 1/2 npt or a diameter like .375 all work. Tap the ☆ on any size to make it a favorite (or press * on a highlighted row). Favorites, recent picks and the most-used sizes are pinned at the top; every UNC, UNF, UNEF, ISO metric, NPT, NPS, BSPT and BSPP size is below, grouped by series.
2. Cut or form tap. A cut tap cuts the thread out. A form tap pushes the metal into shape (no chips), so it needs a bigger drill. Default % thread: 75% cut, 65% form. You can type 50–100%.
3. Read the drill. You get the exact drill size, the nearest standard drills just under and just over (fraction / number / letter and metric), and the real % thread each one gives.
- Green = good. Amber = check it (shallow thread, or a pipe thread that uses a table drill). Red = high torque, the tap may snap.
- More than ~75% thread barely adds strength but adds a lot of tap torque.
- Thread class. Pick 2B or 3B (inch) — metric is 6H. The green band in the drawing is the allowed minor Ø; the chip says if your drill lands in it, under it (tight) or over it. Form taps don't cut the minor, so check those with a gauge.
- Clearance drill for the bolt in the mating part has its own card right below the Drill panel: close fit and free fit (inch chart, ISO 273 metric). Pipe threads don't show it.
- Pipe threads (NPT, NPS, BSPT, BSPP) don't use the % formula. The app shows the published table drill. Tapered threads: check depth with an L1 plug gauge. NPS lists the NPSM drill first and the NPSC (coupling) drill under it.
4. Speeds & feeds. Set the work material and its hardness once (HB or HRC). Leave hardness blank and the app uses a typical value for that material. If the material is too soft for the HRC scale, switch to HB.
5. Make the numbers yours. Tap SFM and the drill's Speed, Spindle and Feed/rev boxes show the calculated values. Type over any of them (a dashed underline means you can edit it). Drill speed and spindle are linked through the drill Ø, so changing one updates the other. Tap use calculated to go back. Going above the published range shows a heads-up in the notes.
6. Hole depth. Pick Blind or Through, type the full thread depth (or part thickness), the tap chamfer and the drill point (118° or 135°). The app works out Tap to Z (thread + chamfer threads) and Drill to Z (on blind holes, one pitch of clearance but never less than .050" / 1.27 mm, the Haas minimum, plus the point; on through holes, a small breakout plus the point) and fills them into both code boxes.
7. G-code. The tap box gives a Fanuc rigid-tap block (M29 + G84). The drill box picks the cycle from the hole depth: G81 (no peck), G73 (chip-break peck) or G83 (full-retract peck), with the peck depth Q. Z comes from Hole depth (Z0 = top of the part). Each amber ? is yours to fill in: X Y (hole position) and R (retract plane), plus Z if no depth is set. Never run a block that still has a ? in it. Copy above each box copies the whole block.
8. Tap style & holder. Under Rigid tap, pick the tap you're running: spiral flute (lifts chips out, the pick for blind holes), spiral point (pushes chips ahead, through holes only) or straight flute (short-chipping work like cast iron, shallow holes). Form taps make no chips, so style doesn't apply. Holder: rigid, synchro (minimal compensation) or tension/compression. With M29 rigid tapping, a floating tension/compression holder can pull the tap and cut oversize. Both choices are saved on this device and feed Troubleshoot.
9. Troubleshoot. Pick what went wrong (tap broke, thread oversize or tight, drill wanders, chips packing, drill burns, bad finish, Fanuc rigid tap). Each card is a sourced cause and fix. Cards that match your current settings light up amber (YOUR SETTINGS) or red (HIGH RISK for the worst ones) and show your number; green CHECKED cards are ones your settings already pass. Tap a source to open it.
10. Inserts (STI). Turn on Insert (STI) under the thread to repair a stripped hole or put a stronger thread in soft metal. Jump to Inserts takes you straight to the section. It gives the STI drill, the STI tap, a % thread check, insert lengths from 1×D to 3×D with hole depth and Tap Z for each, a Fanuc STI tap block and the install steps. When the Heli-Coil, Recoil and Emuge charts disagree on a size, buttons let you pick which chart to follow. Anything your chart doesn't publish comes from Heli-Coil and is tagged in copper. The section only shows for sizes the charts cover, and not for pipe threads. Repair or scrap? (DEMO $) compares the cost to repair with an insert against a new part, using sample numbers you can type over.
Every speed and feed is a conservative starting point from published maker charts (Morse, Redline, Tru-Edge, Haas, OSG, Gühring, Emuge). Harvey Tool is listed as a second source where its miniature carbide drill chart agrees. Harder material lowers the numbers or blocks them. Always check your own tool maker's chart and listen to the cut.
in | mm in the header flips every length, feed and the G-code (G20 / G21).
DEMO $ (gold, bottom): sample numbers only. Wear cost includes the time to swap a worn tap (Tap change min). Method: cost per hole = (tap price + change time) ÷ holes per tap, plus breakage. Dollar defaults are samples, not published data. Type your own to estimate. They stay on your device.
On a PC the tap and drill panels sit side by side. On a phone, add it to your Home Screen and it works offline after the first visit.