CNC Dash Board

User guide

From drawing to program on the machine

A walk through every screen of the app, using a 5-frame CR profile as the example (multiple frames are a PRO feature).

Video tutorial · 38 seconds

Machining a 30° × 3 chamfer on a Ø25 pin

From drawing to G‑code with the CR profile — just 4 fields to fill in.

  1. Read the drawing: Ø25 pin, 30° chamfer, depth 3 — plus R0.3 to round the cone tip.
  2. Enter them in CR PROFILE: Dx-A = 25, C1 = 3, α = 30, R = 0.3.
  3. G‑code + 2D path: N1 T101 roughing, N2 T202 finishing, the running line highlighted.
  4. Check in 3D: rotate and zoom on the chamfered end — end face Ø21.19.
  5. Dimensioned drawing: A X25.0 Z-3.0 · B X21.709 Z-0.15 · D X21.189 Z0.

Video tutorial · 53 seconds

Read the drawing, fill in CR‑H: 55° taper · R4 · Ø32 pin

A real drawing never uses the app's field names — this video shows how to circle the 5 numbers you need and type them into CR-H PROFILE.

  1. Read the drawing: zoom into the taper – fillet – pin and circle Ø40 (Dx), 20.46 from the face to the Ø40 edge (C1), 55° taper angle to the axis (α), R4 (R) and Ø32 (Hx).
  2. Stock from the title block: Ø40 round bar — the app fills in ⌀40 · L 30.46 by itself (AUTO). The C0.5 face chamfer is the default (M_tori 0.5).
  3. Type it in: Dx 40, C1 20.46, α 55, R 4, Hx 32 — the preview redraws as you type.
  4. Apply → simulate: N1 T101 roughing, N2 T202 finishing, the running G‑code line highlighted.
  5. Check the 図 drawing (15.58 · ⌀35.41 · C0.50) and the 3D model before it goes to the machine.

Video tutorial · 57 seconds

Read the drawing, fill in KANTSUGI: SR24 ball · R3 · Ø22 pin

Only 4 numbers from the drawing — the app works the ball radius R1 out from Dx. The video circles each one and types it into KANTSUGI PROFILE.

  1. Read the drawing: circle Ø48 — the largest diameter of the ball (Dx), 42 from the face to that largest Ø (C1), R3 blending pin and ball (R2) and Ø22 (Hx).
  2. SR24 needs no input: R1 = Dx / 2 = 24, worked out by the app. Stock Ø48 from the title block → the app fills in ⌀48 · L 52 (AUTO).
  3. Type it in: Dx 48, C1 42, R2 3, Hx 22 — the preview redraws as you type.
  4. Apply → simulate: N17 roughing layer by layer, N8 T808 finishing with G42, the running G‑code line highlighted.
  5. Check the 図 drawing (18.86 · ⌀24.72 · R24 · R3) and the 3D model before it goes to the machine.

Video tutorial · 47 seconds · part 2

KANTSUGI tail: closing the Ø48 ball with TAIL R+r

Follow-up to the previous video: flip the part and machine the tail. One drawing with head and tail, 66 overall — the tail needs just 2 numbers.

  1. The full drawing: head Ø22 · R3 · SR24 ball up to Ø48 at 42 (setup 1, KANTSUGI — previous video); the tail is the back half of the same ball, Ø48, 24 long (setup 2, TAIL R+r). Overall 66 = 42 + 24.
  2. Circle the tail: SR24 → R = 24; the ball closes on the centre line → pick Theo X_A, X_A = 0; 24 is L — worked out by the app; Ø48 = 2R is just a check.
  3. Type into TAIL R+r: R 24, r 5 stays default (with X_A = 0 there is no small arc), switch to Theo X_A, enter 0.
  4. Apply → simulate: roughing layers follow the R24 arc, the running G‑code line highlighted.
  5. Check the 図 drawing (24 · R24 · ⌀48 · X0) and 3D; the tail stock ⌀48 · L34 is filled in by the app.

Video tutorial · 51 seconds · bore · PRO (2 frames)

NKE RCR: reading a two-taper bore drawing

A taper bush drawn in section: Ø28 mouth, taper to Ø26, an R1 arc, a 20.02° taper down to the Ø21.8 hole. Circle the 9 boxes of the 2 frames — or tap THAM SỐ MẪU → MẪU XA28.

  1. Count the tapers: 2 tapers joined by an arc → N_frame = 2.
  2. Frame 1: Ø28 mouth on the face (XA), 9.2 from the face to the corner between the tapers (C1), R0.3 mouth radius (R_leader), Ø26 where the tapers meet (Hx-E). The first taper angle (4.43°) is worked out by the app.
  3. Frame 2: R1 joining arc (Rconnect), 20.02° second taper to the axis (α), Ø21.8 exit hole (Hx-E1), R1 bottom radius (R2).
  4. Type it in: tap THAM SỐ MẪU → MẪU XA28 fills all 9 boxes; open tabs 1 / 2 to see each frame.
  5. Apply → simulate (N1 T101 roughing, N2 T202 finishing with G41), then check the 図 drawing and the 3D half-section — one colour per frame.

Video tutorial · 41 seconds · ball seat

3R: reading a ball-seat drawing — just 3 numbers

A concave SR17.05 seat: the sphere centre sits 4 mm outside the face, Ø28 hole at the bottom. The r1, r2 blends and the mouth Ø are found by the app.

  1. Read the drawing: SR17.05 sphere radius (R), 4 from the face to the sphere centre — outside the part (c1), Ø28 bottom hole (hx).
  2. Nothing else to type: mouth blend r1 (0.5426), bottom blend r2 (1.85) and the mouth Ø (33.99) are searched by the app so the arcs stay tangent (AUTO badge). Type into r1 / r2 if your drawing gives other values.
  3. Type it in: R 17.05, c1 4, hx 28; open THÔNG SỐ CẮT for w / u / Follow Rough.
  4. Apply → simulate: roughing layers from the Ø28 pilot hole out to the mouth, then the G41 finishing pass r1 → R → r2.
  5. Check the 図 drawing (A B C E, every radius) and 3D — the SR17.05 reference sphere shows the seat lies exactly on the sphere.

Video tutorial · 46 seconds · 1-frame taper bore

NKE RCR, 1 frame: a 25° taper bore — 5 numbers

A cone seat: R3 mouth, 25° taper 30 deep, R10 into the Ø20 hole. Only 2 boxes change from the defaults; the mouth Ø is worked out by the app.

  1. Read the drawing: 25° taper to the axis (α), 30 from the face to where the taper meets the Ø20 hole (C1), R3 mouth radius (R_leader), Ø20 hole (Hx-E), R10 into the hole (R2).
  2. Mouth Ø51.80 (XA) needs no input — worked out from α, C1, R_leader and Hx.
  3. Type it in: N_frame 1; from the defaults only C1 40 → 30 and α 14 → 25 change.
  4. Apply → simulate: roughing layers from the Ø20 hole out to the mouth, the running G‑code line highlighted.
  5. Check the 図 drawing (32.22 · ⌀51.80 · α 25°) and the 3D half-section.

Video tutorial · 51 seconds · outer grooves

SPOOL: 3 O-ring grooves — read one, repeat ×3

A Ø15.55 shaft with three 3.4-wide O-ring grooves down to Ø11.96. Pick RÃNH mode and circle 9 boxes — or tap THAM SỐ MẪU → O-RING.

  1. Count the grooves: 3 identical grooves → RÃNH mode, 3 frames.
  2. One groove: Ø15.55 shaft at the mouth (D), 3.4 width (L rãnh), Ø11.96 bottom (BORE), C0.35 mouth chamfer, R0.2 bottom radius.
  3. Spacing: 2.3 between grooves (W), 2.3 face → first groove (Z đầu), 2.5 last groove → end (Z đuôi).
  4. Type it in: switch CUNG → RÃNH, tap THAM SỐ MẪU → O-RING — it fills all 3 frames and the W2.0 grooving tool.
  5. Apply → simulate groove by groove (rough + finish), then check the groove detail on 図 and in 3D.

Video tutorial · 45 seconds · internal pocket

Internal Grooving: a Ø22 pocket inside a Ø15.2 bore

A 14-long bush, Ø15.2 bore, a Ø22 pocket 2.5 in from each face, R2.5 corners — cut with a W3 round-nose grooving tool. The 2D and 3D simulations run together.

  1. Read the drawing: 14 part length, Ø22 pocket, R2.5 corner radius, 2.5 walls on both sides (face → pocket), Ø15.2 bore.
  2. Ø30 outside is only for the 3D model (in THÔNG SỐ CẮT).
  3. Tool: pick ĐẦU TRÒN W3 (round nose) in the Dao móc row — a round nose cuts the R2.5 corners.
  4. Check the 図 drawing (pocket 9 · L14 · Ø22 · R2.5).
  5. Simulate: the 2D frame and the 3D half-section run on one clock — the pocket opens pass by pass, N5 T505 follows the program.

Video tutorial · 52 seconds · internal grooves

SPOOL INTERNAL: 2 grooves in a Ø14 / Ø12 stepped bore

A 20-long stepped bore Ø14 → Ø12 with two 3.4-wide grooves down to Ø16. One frame per groove — these are the O6410 defaults.

  1. Count the grooves: 2 grooves → RÃNH mode, 2 frames (one per groove).
  2. Frame 1: Ø14 mouth bore (Ø lỗ tại A), Ø12 bore after groove 1 (Ø lỗ phía xa), 3.4 width, Ø16 bottom (BORE), R0.2 mouth, R0.5 bottom. Frame 2 starts in the Ø12 bore.
  3. Spacing: 2 face → groove 1 (Z đầu), 6.6 between grooves (W), 4.6 groove 2 → end (Z đuôi). The Ø30 outside is only for the 3D.
  4. Type it in: open tabs 1 / 2 and type each frame; w/u stock and mouth/bottom extras sit in LƯỢNG DƯ.
  5. Check the 図 drawing, then the 3D half-section simulation: rough then finish, groove by groove.

Video tutorial · 42 seconds · spherical washer

WASHER: a spherical-face washer — 4 numbers

A washer with a Ø9 bore and Ø15 outside: the front is an SR20 sphere, then a 2-long flat land. The 2.95 thickness comes out by itself.

  1. Read the drawing: SR20 sphere radius (R) — the dashed circle shows the face lies on that sphere.
  2. Ø15 outside, where the sphere ends (chord1); Ø9 bore, the sphere starts at its edge (chord2); 2 flat land behind (offset).
  3. No corner radii on the drawing → r1 = r2 = 0. The 2.95 thickness = sphere depth + land, worked out by the app.
  4. Type it in: R 20, chord1 15, chord2 9, offset 2 — then Apply.
  5. Simulate, then check the 図 drawing and the 3D with the SR20 reference sphere.

Video tutorial · 43 seconds · arc body

ARC BODY: an R505 barrel — 3 numbers make the arc

A 200-long roller, Ø30 at both ends, swelling to Ø50 in the middle with one R505 arc. The drawing is at 1 : 4 so it reads well.

  1. Read the drawing: 200 length (L), Ø30 both ends (D), R505 arc radius (R).
  2. No neck: the arc runs straight to the face → N = 0.
  3. Ø50 in the middle (Dmax) and the end angle θ 11.42° are worked out by the app — just a check.
  4. Type it in: L 200, D 30, R 505, N 0; stock Ø55 sits in THÔNG SỐ CẮT.
  5. Simulate (long roughing layers, then the finishing pass along the arc), check 図 and 3D.

Video tutorial · 44 seconds · round bead

MULTI BEAD: one R0.8 bead on a Ø10 core

A Ø10 pin, 22 long, with one R0.8 round bead 1.5 wide, 0.5 from the face. Tap THAM SỐ MẪU → MẪU ⌀10 and every box is filled.

  1. Count the beads: 1 bead → N_gờ = 1. Ø10 core (D_core).
  2. The bead: R0.8 radius (R input mode), 1.5 width along Z — the chord (P_gờ).
  3. Position: 0.5 face → bead (L_right), 20 bead → chuck side (L_left). The bead top Ø11.04 (X_gờ) is worked out by the app.
  4. Type it in: tap THAM SỐ MẪU → MẪU ⌀10 (stock Ø20 included), or type 6 numbers.
  5. Simulate, then check 図 and 3D — the bead has its own colour.

Video tutorial · 36 seconds · G19 arc milling

ENMILL G19 ARC: an end that sits on a Ø27.2 pipe

A Ø25 bar, 17 long, its end milled hollow to fit a Ø27.2 pipe whose centre is 25.5 from the left end — a T-joint onto a pipe. Milled with G19 arcs.

  1. Read the drawing: the dashed circle is the pipe to fit — Ø27.2 → D_pipe.
  2. 25.5 from the left end to the pipe centre → Pitch; 17 part length → L; Ø25 bar → Ø stock.
  3. Mặt gia công = Cung R: the end is milled along an arc so it hugs the pipe.
  4. Type it in: D_pipe 27.2, Pitch 25.5, L 17, Ø stock 25 — then Apply.
  5. Simulate the G19 arc layers, then check the 3D with the pipe as a wire cylinder.

Video tutorial · 39 seconds · flange

ENMILL FLANGE: a 2-ear flange — 5 numbers + the tool

The end of a Ø107 bar, 30 long, milled 10 deep into a flange: 2 ears R12 with centres 83 apart, a round Ø50 middle. Read from the end view and the side view.

  1. End view: R12 ear radius (r_end), Ø50 width across the middle (D_mid), 83 ear centre → ear centre (span).
  2. Side view: 30 bar length (L), 10 milling depth (Z_emill).
  3. Stock Ø107 = span + 2·r_end, worked out by the app (D_cut 0 = AUTO).
  4. Type it in: r_end 12, D_mid 50, span 83, L 30, Z_emill 10; tap the ⌀32 suggestion for d_tool → 1 layer.
  5. Simulate (tool fixed, C axis turns), check the toolpath order and the 3D.

Video tutorial · 42 seconds · eccentric turning

ECCENTRIC TURNING: a pin 3 off centre — Y·C or X·C

A Ø24 pin, 60 long, whose axis sits 3 away from the axis of the Ø30 bar. Turned with the C + Y axes (Y·C G17) or with the X·C macro.

  1. Read the drawing: two centre lines — the bar axis and the pin axis. Ø30 bar (ø phôi), Ø24 pin (ø chốt).
  2. 3 between the two centre lines → e = 3; 60 pin length from the face → L.
  3. No twist on the drawing → H = 0; AP = 0 means one pass, full depth.
  4. Type it in in Y·C G17 mode, Apply, simulate, then check the 3D.
  5. Switch to X·C macro: the same pin as a macro program.

Video tutorial · 37 seconds · two flats

ENMILL 2-PLANE: two parallel flats on a round bar

A Ø30 bar, 30 long, with two flats 16 apart, 10 long at the end. Note: the app takes the RADIUS R, while the drawing gives the diameter.

  1. End view: bar Ø30 → the app wants the radius: R = 15.
  2. 16 across the two flats → W.
  3. Side view: 30 bar length (L), 10 flat length = end-mill depth (Z_emill).
  4. Type it in: Ngoài · Two Face, R 15, W 16, d_tool 12 (only draws the tool in the simulation).
  5. Simulate both flats, check the toolpath order and the 3D.
Profile picker by shape, outer turning group
PRO profile card ring
01

Pick a profile

The first screen asks “Bạn cần gia công gì?” (what do you need to machine?). Pick a type: TIỆN NGOÀI (outer turning), ĐẦU CẦU (ball end), LỖ TRONG (bore), PHAY (milling) or REN (thread).

  • For outer turning, then pick what you see on the drawing — CÔN (taper), ĐOẠN TRỤ (cylinder), ĐUÔI (tail), KHUNG BẬC (step) and the number of arcs — and the list below keeps only the matching profiles.
  • Already know the name? Switch to Tìm theo tên (search by name).

PRO adds the card ring: swipe sideways to change card, swipe up/down to flip it over, hold for 1 second to open.

CR parameter sheet with preview and 5 frames
02

Enter the drawing numbers

Opening a profile brings up the Thông số (parameters) sheet. The preview at the top redraws as you type, with ⌀, lengths, angles and point names just like the drawing.

  • THAM SỐ MẪU (sample sets): tap to load a ready-made set of numbers, then adjust it to your part.
  • N_frame − / +: chain several sections (tapers, cylinders, shoulders) on one part; the 1, 2, 3… buttons open each frame. For CR and NKE RCR, multiple frames are a PRO feature (the free edition uses 1 frame).
  • Labels with a ⇆ (e.g. C1 ⇆, α ⇆): tap the label to switch that field to the other quantity your drawing gives.
  • Thanh trượt (sliders): drag to adjust quickly within the valid range. When done, tap Áp dụng (apply).

If a value can't build the shape, the app tells you right away instead of producing wrong G‑code.

THÔNG SỐ CẮT section: w, u, Follow Rough, CuttingMount, compensation, roughing style
03

Cutting parameters

Open the THÔNG SỐ CẮT (cutting parameters) section of the sheet:

  • w / u — stock left in Z and in X for the finishing tool.
  • CuttingMount — depth of cut per roughing layer.
  • Follow Rough — the end of each roughing pass follows the profile for this length (mm); 0 = off.
  • Bù dao N2 — tool compensation G41 or G42. Kiểu cắt thô N1 — roughing style: Ngang (layers in X) or Dọc (layers in Z).
Roughing simulation running, matching G-code line highlighted
04

Tool path simulation

Close the parameters sheet and tap the drawing to run the simulation: each roughing layer, then the finishing tool along the profile.

  • The G‑code sits right below; the line being run has a ▶ and a highlight, so you can match every block to the tool movement.
  • Tapping again while it runs jumps to the end result. Hold the drawing for about half a second to reopen the parameters.
図 drawing of the 5-frame part with magnified arc cells
05

図 drawing

The ruler button in the top bar opens the drawing: diameters, lengths, angle α and radius R of every frame.

  • Small arcs are magnified in detail cells below (×2.9, ×3.8…) so the tangent points are easy to read.
  • Use + / − / ⟲ or two fingers to zoom in and out.
3D model coloured by frame
06

3D model

The cube button opens the 3D model of the part. Each frame has its own colour, with a legend below.

  • Rotate with one finger, zoom with two fingers or + / −, and ⟲ to go back to the starting view.
Data page: tapped point line C1, point lit on the drawing
G-code page: N1 T101 roughing, N2 T202 finishing with G41, running line highlighted
07

Data and G‑code

Below the drawing there are two pages: Dữ liệu / 図 (data / drawing) and G‑code.

  • The Dữ liệu page lists the inputs, the coordinates of every point and the roughing layers. Tap a point line (e.g. C1) and that point lights up in yellow on the drawing.
  • The G‑code page: the free edition has the G‑code program (the app's own N1 roughing / N2 finishing). For CR, CR-H, RCR, KANTSUGI, TAIL R+r, WASHER, NKE RCR and 3R, PRO lets you tap the tab again (marked ⇆) to switch to FANUC G‑code (G71 / G70 cycles) or OKUMA G‑code (G85 / G87 cycles with NLP).
ENMILL POLYGON parameter sheet with hexagon preview
3D polygon milling simulation, stock turning on the C axis
08

Milling on the lathe · PRO

Milling profiles use a live tool and the C axis. Example ENMILL POLYGON: choose VIỀN NGOÀI ⇆ (outer profile) or inner pocket, number of sides, width across flats W, corner radius R and tool diameter.

  • Z output / L sets the Z origin (メイン / サブ) and the stock length.
  • In 3D the stock turns with the C axis and the end mill removes material exactly as the program says — leftover stock or gouges show up at once.

Milling needs the PRO unlock (one-time purchase).

M12x1.75 thread drawing page: section with ⌀d / d2 / d1, 60° basic profile, info cards
Okuma G33/G92 G-code: one X line per pass
Okuma G71/G76 G-code: the whole thread cycle in one block
09

Threading

Type the thread code (e.g. M12x1.75) — the app recognises the thread system (M, R, G, UN) and shows ✓ Mã hợp lệ (valid code); Các loại ren hỗ trợ (supported threads) lists the codes — tap one to fill it in. Pipe threads R / Rc / PT, Rp / Ps, G / PF are part of PRO.

  • Enter the thread length L, the entry point V and the Z origin.
  • Choose the control Okuma / Fanuc, external / internal thread, and the G71/G76 or G33/G92 cycle.
  • The BẢN VẼ (drawing) page describes the thread: a section with ⌀d / ⌀d2 / ⌀d1, pitch P, height h, L and V; the 60° (or 55°) basic profile with its formulas; and info cards giving the standard and the 6g / 6H tolerance for metric threads.
  • The G-CODE page: G33/G92 prints every pass as its own X line; G71/G76 packs the whole thread cycle into one block.
10

Machining calculator

The formulas you reach for next to the machine — cutting speed, spindle speed, feed, roughness, time, power, tap drills, fits, materials — right in the app, no pocket calculator or handbook needed.

Profile picker with the calculator button circled in yellow and magnified
1

Open the calculator

On the profile picker, tap the round calculator button next to VI / EN and ☀︎/☾ (in both the list and the card ring).

Turning group: cards for cutting speed, cutting time, roughness and power
2

Pick a group

Four groups: Turning · Milling · Drill · Standard, each a set of formula cards. Tap the open group again to return to the welcome screen.

Cutting speed: v 260 and D 40 give N 2069, with tags G96 S260 and G97 S2069
3

Type — the result shows at once

Tap a card: the top panel shows the formula and what each symbol means, the bottom panel the input fields. Results update as you type (black box, yellow number) — there is no Calculate button. Tap the G96 S… / G97 S… tag to copy the command.

Radio button on N: typing 2069 rpm gives a cutting speed of 260
4

Pick the field you type

Two-way formulas (v ⇄ N, fz ⇄ F, mm ⇄ inch): the radio button marks the field you type, the other one is solved. Tap a radio button or the result box to swap — the current number is kept.

Theoretical roughness: R 0.8 and f 0.15 give Rz 3.52 and Ra 0.9
5

Surface roughness

Enter the nose radius R and feed f to get the theoretical Rz and Ra. Example: R0.8, f 0.15 → Rz 3.52 µm, Ra 0.9 µm. An explanation of Ra and Rz sits below.

Table feed: fz 0.05, N 3000, Z 4 give F 600
6

Milling: table feed

F = fz × Z × N, plus cutting power and time. Example: fz 0.05, 4-flute cutter, 3000 min⁻¹ → F600 mm/min. The Drill group has speed, time, and power · thrust · torque.

Tap drill for M10×1.5: drill 8.5, D1 from 8.376 to 8.676
7

Tap drill · taper

In Standard: type the M thread diameter and pitch → suggested drill and minimum / maximum minor bore D1 for 6H. Example: M10×1.5 → ⌀8.5. Also taper angle ⇄ 1 : x and mm ⇄ inch.

Fit tolerance for a 20 mm H7 bore: upper deviation +21 µm, lower 0
8

Fit tolerances

ISO 286 / JIS B 0401: enter the size, choose Shaft or Bore, the tolerance zone and IT grade → upper / lower deviation and maximum / minimum size. Example: ⌀20 H7: +21 µm / 0.

Material cross-reference: SCr440, SCM430, SCM435 with matching AISI, DIN and GB grades
9

Material cross-reference

Search steel grades across JIS · AISI · DIN · GB (e.g. S45C, 1045, C45). Next to it is Unit conversion: length, speed, mass, force, pressure, power, torque.

The Ks and K factors and the equivalent steel grades are reference values — check them against your tool catalogue and material certificate. The trash button clears every number; tapping back into a field that holds a number selects it, so typing overwrites it.

11

Taking the program to the machine

Before running on the real machine:

  • Check that tool numbers, M-codes and the Z origin match your machine and setup.
  • Dry-run without cutting, with reduced rapid speed the first time.
  • Compare the G‑code with the simulation — every line was highlighted as the simulation ran through it.

Always verify the program, confirm M-codes for your machine, and dry-run before cutting.

Find the profile that matches your part