日本語简体中文

5-AXIS CALCULATORS5-axis calculations

Small calculations for checking a 5-axis program. Everything is calculated in your browser; the values you enter are not sent anywhere.

FF value for G93 inverse time feed

F for G93—1/min
Time to finish the move—sec

F_inv = 1 / T = F_mm / L (T: minutes)[3][1][2]

While G93 is active, write F in every cutting block (the previous F is not carried over). Example from NIST and Siemens: F2 finishes the move in 0.5 min.

∠Ball end mill tilt angle (angle that keeps the tool center out of the cut)

Tilt more than this—deg

θ = arccos(1 − ap / R)[4]

Cutting with the tool center, where surface speed is almost 0, crushes the material instead of cutting it and tends to leave marks. In a KISTEC experiment (R3, ap 0.3), the tool center cut at 15° and did not touch the surface at 30° or more (the formula gives 25.8°). However, in the same experiment the surface roughness Rz was smaller with no tilt, so decide based on whether you weight appearance (gloss) or roughness more.

↗Angles from the tool direction vector

Tilt angle (from the Z axis)—deg
Swivel angle (from the X axis)—deg
Angle from the XY plane—deg

Tilt angle = arccos( K / √(I² + J² + K²) ), swivel angle = atan2( J, I )[5]

The vector points from the tool tip toward the tool holder; its length doesn't matter. Siemens example: (1, 1, 1) → tilt 54.73561°, swivel 45°. The actual rotary axis angles (A, B, C) depend on the machine configuration, and there may be two solutions.

↻How a rotary axis turns (shortest direction and reducing the displayed value)

Rotation in the shortest direction—deg
Rotation if moved as is—deg
Displayed value reduced to under 360°—deg

Δ = ((target − current + 180) mod 360) − 180 Reduced value = displayed value mod 360[6]

On a rotary axis that counts beyond 360°, 350° → 10° can take the long way around, −340°. Some controls have a function that turns the shortest way (such as Heidenhain M126) or one that reduces the displayed value before moving (M94 on the same control). If you command 180° while the displayed value is 538°, the axis turns −358°.

Other 5-axis machining pages

◇

5-axis machining basics

The difference between 3+2 and simultaneous 5-axis machining, the advantages of 5 axes, and terminology.

⟲

5-axis machine configurations

The three types (head-head, table-table, head-table) with their advantages and drawbacks, the names and directions of rotary axes A, B, C, vertical vs. horizontal machines, and multitasking machines.

G

5-axis NC functions

Tool center point control, tilted working plane commands, and 3D tool radius compensation. A comparison of commands by NC maker, G93 inverse time feed, tool length and the center of rotation.

◎

Calibration, collision, workholding and tools

Kinematics calibration with a reference sphere, accuracy test standards, collision checking and simulation, 5-axis vises, tool stick-out and how to tilt a ball end mill.

!

Common 5-axis mistakes

Singularities, the two solutions of a rotary axis and the long way around, feed units, forgotten tool length, and forgetting to cancel a tilted plane. A checklist to verify on the shop floor.

⌗

CAD/CAM

CAM workflow, toolpaths, a list of software, and data formats.

📚Sources

  1. National Institute of Standards and Technology (NIST), “The NIST RS274NGC Interpreter – Version 3 (NISTIR 6556, 2000)”
  2. Siemens AG, “SINUMERIK 840D sl/828D Fraisage ISO, Manuel de programmation 02/2012 (6FC5398-7BP40-3DA0, French edition)”
  3. Haas Automation, Inc., “G93 Inverse Time Feed Mode (G-code reference page)”
  4. Kanagawa Institute of Industrial Science and Technology (KISTEC), Tomohiro Yokota, “A Study of Machined Surface Quality in Ball End Milling,” KISTEC Research Report 2020
  5. Siemens AG, “Milling with SINUMERIK — 5-axis machining Manual, Edition 05/2009 (DocOrderNo. 6FC5095-0AB10-0BP1)”
  6. DR. JOHANNES HEIDENHAIN GmbH, “TNC 640 User's Manual Conversational Programming, NC Software 340590-01 / 340591-01 / 340594-01, 4/2012 (892903-20)”