5-Axis Transformation (TRAORI)

On a 3-axis mill the tool always points straight down, so “the position” and “the tool tip” are the same thing. The moment you add rotary axes that swing the tool at an angle, they stop being the same: tilt the head 20° and the tip swings away from where the linear axes say it is. TRAORI — Siemens’ orientation (5-axis) transformation — closes that gap. With it active, the programmed X/Y/Z always mean the tool tip, and the control automatically moves the linear axes to compensate whenever the rotary axes turn, so the tip stays exactly where you put it. It is the SINUMERIK equivalent of Fanuc’s Tool Center Point control (G43.4/G43.5) and Heidenhain’s FUNCTION TCPM. This page is derived from Siemens’ SINUMERIK 840D sl / 840D / 840Di sl NC Programming manual (A5E47432823B AA, 06/2019), §3.9.2.

The Core Behavior

Straight from the manual: “When the transformation is enabled, the positional data (X, Y, Z) always relates to the tip of the tool. Changing the positions of the rotary axes involved in the transformation causes compensating motion of the remaining machine axes — which means that the position of the tool tip remains unchanged.” In three-, four-, and five-axis transformations the programmed position always relates to the tip, which is tracked orthogonally to the machined surface in space. You program where the tip goes and how it’s oriented; the control solves for the actual machine-axis moves.

Activating and Deactivating

Siemens describes the parameterized form as TRAORI(transformation number, orientation vector, rotary axis offsets). Parameters can be omitted if the correct order is kept — e.g. TRAORI(, , , ,A,B) enters only the rotary-axis offset. As an alternative to programming the offset directly, it can be taken automatically from the currently active zero offset (configured in machine data).

Because tool-length compensation must act along the tool-orientation direction, set the working plane (G17/G18/G19) so the length offset works in the direction the tool points.

The Orientation Vector

The vector (X,Y,Z) in the parameterized call is the component of the orientation to which the tool points — and the manual is specific about direction: “Orientation transformation always points from the tool tip to the tool adapter.” So the vector runs tool-tip → adapter (up the tool). The examples:

The transformation assumes the rotary axis is orthogonal to the orientation plane, and orientation is possible only in the plane perpendicular to that rotary axis. It supports both moving-tool and moving-workpiece machine types — two-axis swivel head, two-axis rotary table, or one-axis head plus one-axis table.

Programming the Tool Orientation

The vector in the TRAORI() call only sets the basic orientation. The useful part is changing the orientation as you cut, and SINUMERIK gives you several ways to say where the tool points — with a G-code group choosing how the values are read:

Two things bite here. Near the pole (tool axis parallel to the 1st rotary axis) an ORIWKS reorientation can demand runaway rotary speed — $MC_TRAFO5_POLE_LIMIT / NON_POLE_LIMIT (24540/24530) bound how the control passes through it. And an orientation-vector or Euler orientation cannot be combined with thread cutting (G33/G331/G332), G04, G63, G74/G75 or REPOS — that raises alarm 12130; a doubly-programmed orientation raises 12240.

Singularities and the Pole

The two orientation axes span a coordinate system of longitude and latitude over a sphere; the pole is where they converge — the tool axis lined up with the 1st rotary axis. Near it, a tiny change in tool orientation demands a huge rotary swing, so one or more axes want to move very fast. Rather than run away, the control raises Alarm 10910 “irregular velocity run in a path axis” and caps the programmed velocity to the maximum axis velocity — it slows through the region instead of gouging. How it negotiates the pole is set by two machine data:

Practical upshot: don’t program an orientation change right at the pole; if a toolpath must cross it, expect the machine to either slow down (10910) or snap the tool through. Interpolating in ORIMKS (machine-axis reference, below) sidesteps the worst of it, because it moves the rotary axes directly rather than trying to hold the tool vector on a straight line past the singularity.

ORIWKS vs. ORIMKS — Reference for Orientation Interpolation

When the tool re-orients between two blocks, the path the orientation sweeps depends on which reference system it’s interpolated in. That’s ORIWKS vs. ORIMKS:

ORIWKS is the basic setting, and Siemens advises: for a 5-axis program where it isn’t yet obvious which machine will run it, always select ORIWKS — because its motion is kinematics-independent, the program behaves the same everywhere. Reach for ORIMKS only when you need actual machine movements (collision avoidance). Whether the reference follows these G commands is itself machine-data-gated (a set-up mask can force one system).

TCARR — The Orientable Toolholder

Not every “5-axis” job runs a full transformation. For a manually or mechanically set orientable toolholder, SINUMERIK computes tool-length compensation from the holder’s orientation with TCARR and the TCO… path commands:

The tool-length offset is re-calculated when you switch between TCOFR and TCOABS. TCARR pairs naturally with the swivel plane cycle — a swivel-mounted workholder or head can be handled as a TCARR toolholder for 3+2 work, while TRAORI is for continuous orientation change.

Resetting at Program Start

Siemens recommends clearing any active transformation and swivel at the top of a program so a leftover state can’t corrupt the setup:

Parameters by Axis Configuration

TRAORI’s behaviour is fixed by machine data the MTB commissions — but those machine data are worth knowing, because they literally encode whether the rotaries are on the head, the table, or split between them. The master switch is $MC_TRAFO_TYPE_1 (MD24100): its value declares the kinematics.

The newer generic 5-axis transformation collapses that to one value per kind: 24 = rotatable tool (T), 40 = rotatable workpiece/table (P), 56 = mixed (M), 72 = read the kinematics straight from the orientable toolholder. The geometry vectors that go with the transformation — some of which mean different things depending on type:

Notice where the axis pair is encoded. In the classic transformation it’s baked into the type number itself (AB head = 16, BC table = 35, …). In the generic transformation the type stays 24/40/56 and the pair lives in the rotary-axis direction vectors: $MC_TRAFO5_AXIS1_1 / AXIS2_1 = [1,0,0] / [0,1,0] for AB, [1,0,0] / [0,0,1] for AC, [0,1,0] / [0,0,1] for BC (any direction is allowed, so a non-orthogonal axis just gets its true unit vector). Either way the offset vectors above are full measured geometry, not a per-pair component subset — the same principle as Fanuc, which carries the pair in its 19682 / 19687 direction codes rather than in the offset components.

On a machine with an orientable toolholder, the same geometry lives in the TCARR data set and $TC_CARR23 selects the kinematic type there — T rotatable tool (head), P rotatable part (table), M mixed. The head/table split is explicit in how the offset vectors are used: for a type-P (table) holder l1 is ignored and l2/l3/l4 carry the geometry; for a type-T (head) holder l1 is significant and l4 is ignored. And note the two manuals differ on the orientation-reference default: the NC-programming manual calls ORIWKS the basic setting while the Function Manual calls ORIMKS basic — the true default is set per machine by $MC_GCODE_RESET_VALUES[24].

Transformation machine data from SINUMERIK 840D sl Transformations Function Manual (F2), A5E47435470B AA (06/2019) — §3.2.3 (type table p.147), MD list §2.9; orientable-toolholder $TC_CARR fields from the Tools Function Manual (W1), A5E47435126B AA §2.8.

See also — the same idea on other controls: Fanuc keeps the tool tip on path with Tool Center Point control (G43.4 tool-axis / G43.5 vector); Heidenhain uses FUNCTION TCPM (M128’s successor). For the neighbouring Siemens features: Swivel Plane (CYCLE800) for 3+2 tilted-plane work and Workpiece Alignment (CYCLE998 & frames). For how TCP and tilted-plane machining compare across brands, see the cross-control primer on TWP and TCPM.

Sources: SINUMERIK 840D sl / 840D / 840Di sl NC Programming Programming Manual, A5E47432823B AA (06/2019) — §3.9.2.2 Three, four and five axis transformation (TRAORI), §3.9.2.6 Reference of the orientation axes (ORIWKS, ORIMKS), and §3.13.9 Tool length compensation for orientable toolholders (TCARR, TCOABS, TCOFR, TCOFRX/Y/Z). Transformation machine data: SINUMERIK Function Manual, Special Functions (F2).