What is a tool offset for?
When you write a program you do not think about the real size of the tool. You write where the contour has to run. But the tool in the machine has a particular length and a particular diameter — and every tool’s are different.
The tool offset is how you tell the control about that difference. When the tool is called, the control takes the offset data into account; you write the contour and the control works out where to drive the tool centre.
That is why the order matters: measure tools first, set the work offset second. A Z zero taken before tool lengths are entered will be wrong.
$TC_DP parameters), the split between geometry and wear, the TCP concept and matching it to CAM, tool types, entering offsets by hand, measuring tools in JOG mode and calibrating the tool probe.T and D: two numbers, two jobs
On SINUMERIK every tool has a T number — its place in the magazine or its identity. Every tool can have one or more D numbers (cutting edges).
Every data field in the offset memory is invoked with a T and a D number. If a tool has more than one cutting edge (a step drill, say, or the same tool used with separate offsets for roughing and finishing), each one sits under its own D number.
What is inside the offset memory?
The offset memory holds far more than “length and diameter”. This is the manual’s own structure — the values P1…P25 in the offset memory can be read and written by the program through system variables:
| Parameter | Meaning | Remark |
|---|---|---|
$TC_DP1 | Tool type | Determines how the control interprets the tool |
$TC_DP2 | Cutting edge position | Turning tools only |
| Geometry — length compensation | ||
$TC_DP3 | Length 1 (L1) | Allocated to axes by type and plane |
$TC_DP4 | Length 2 | |
$TC_DP5 | Length 3 | |
| Geometry — radius | ||
$TC_DP6 | Radius 1 | Milling / turning / grinding tool |
$TC_DP7 | Corner radius (length 2 on tapered milling tools) | Milling tools |
$TC_DP8 | Rounding radius 1 | Milling tools |
$TC_DP10 / $TC_DP11 | Angle 1 (face end of tool) / Angle 2 (tool longitudinal axis) | Tapered milling tools |
| Wear — length and radius compensation | ||
$TC_DP12/13/14 | Wear on length 1 / 2 / 3 | Added on top of the geometry value |
$TC_DP15/16/17 | Wear on radius, corner radius, rounding radius | |
| Tool base dimension / adapter | ||
$TC_DP21/22/23 | Length 1 / 2 / 3 offset | Adapter or holder allowance |
| Technology | ||
$TC_DP24 | Clearance angle | Turning tools only |
Why keep geometry and wear apart?
The geometry column is the tool’s measured, real size. The wear column is a correction added on top. As the tool wears, or when you find 0.02 mm out on a dimension, you leave geometry alone and write into wear.
The benefit: when you replace the tool you clear the wear cells and the geometry value is still there, untouched. Someone who writes corrections into geometry will not know two weeks later what the tool’s real size actually is.
$TC_DP6–DP8, $TC_DP10, $TC_DP11, $TC_DP15–DP17, $TC_DP19 and $TC_DP20 have another meaning depending on tool type. On a slotting saw, for instance, $TC_DP6 is not the radius but the diameter, and $TC_DP7 is the slot width. Choosing the wrong type has the same effect as typing the right number into the wrong cell.TCP — which point of the tool are you measuring?
When you measure tool length you are really answering one question: which point of the tool is the reference? That point is the TCP (Tool Centre Point).
The source document’s warning here matters:
- On Siemens controls the TCP is taken to be at the tool tip.
- CAM systems may define the TCP position differently depending on tool shape. On ball-nose cutters the TCP may not be at the tip but at the centre of the radius.
- If the CAM system uses a different TCP position, that difference has to be taken into account when determining tool length.
The practical consequence: machining a die with a ball-nose cutter, if you and the CAM programmer do not agree once — and write down — where the TCP sits, the whole part comes out deep or shallow by the tool’s radius.
Tool types
The tool type ($TC_DP1) tells the control how to interpret the tool. On the milling side the most common are:
| Type | Tool | Remark |
|---|---|---|
| 110 | Cylindrical die-sinking milling tool | Named that way in the manual; in certain cases the system uses this type automatically |
| 111 | Ball-nose cutter | Outside the corner-rounding evaluation |
| 120 | End mill (cylindrical) | Per the manual, types 120 and 156 have identical effect |
| 121 / 131 | Toroidal (corner-radius) milling tool | The corner radius is evaluated separately |
| 130 | Angled / tapered milling group | The angle parameters come into play |
The manual’s rule is clear: corner-rounding dimensions are evaluated only for cutter types with a cylindrical shank, toroidal millers (types 121 and 131) and, in the limit case, cylindrical die mills (type 110). All other permitted tool types are interpreted as cylindrical cutters and the dimensions entered for corner rounding are not evaluated.
Entering tool offsets by hand
In shops with a tool presetter, dimensions are determined outside the machine, the tool goes straight into the magazine and the values are typed in from the panel. The path in the source document:
- Select the Parameter operating area.
- Select Tool data. The tool list window opens.
- Select the tool with “T No. +” / “T No. −”.
- Select the cutting edge (offset) number with “D No. +” / “D No. −”.
- Enter the length, radius and, where relevant, corner radius.
- Make sure the tool type is set correctly.
The same screen usually offers: select next/previous tool, step to the next higher or lower offset number, delete a tool or a cutting edge, search for a tool, list all tools, and create a new tool or a new cutting edge.
Measuring tools in JOG mode
If the machine has a mechanical tool probe, measuring is semi-automatic.
Prerequisites
- The measuring cycle options must be configured on the machine.
- The mechanical tool probe must be calibrated and the tool mounted in the spindle.
Steps
- Select the Machine operating area.
- Select JOG on the machine control panel.
- Call the “Measure tool” function. The vertical softkey bar offers three choices: “Radius”, “Length” and “Calibrate tool probe”.
- Choose “Radius” or “Length” according to what you are measuring.
- Fill in the input screen; enter the V offset if required (V is a positive value).
- Press NC START. The measurement starts automatically.
- The calculated “Radius” or “Length 1” offset is written into the active tool offset data.
Measuring tools in AUTO
Tools are also measured in automatic mode during production to keep track of wear. The measurement determines the tool wear values, so the tool’s diameter and length are redefined.
With measuring cycles in automatic mode you can select one of three outcomes: measure only, correct the workpiece zero offset, or correct the tool offset. For wear tracking it is the third.
Common mistakes
Taking a Z zero before entering tool offsets
The Z zero works together with the tool length. The correct order is measure tools first, work offset second.
Leaving the tool type at its default
Corner radius, taper angle and saw dimensions are only evaluated on the right type. On the wrong type there is no alarm — just a wrong part.
Writing corrections into geometry instead of wear
Do it once and the tool’s real size is lost. Corrections belong in the wear column.
Not checking the CAM system’s TCP
On ball-nose cutters the CAM reference point may not be at the tip. On the Siemens side the TCP is the tool tip; the difference has to be accounted for.
Writing into the wrong D number
D1 and D2 of the same tool are different offsets. Call D1 in the program and write the measurement into D2 and the machine runs on the old value.
Skipping probe calibration
It produces a systematic deviation in the same direction on every tool, and tracing it takes days.
Deleting the wrong row in the tool list
Deleting removes the selected T/D data and cannot be undone.
Frequently asked questions
What is the difference between T and D?
T identifies the tool, D identifies that tool’s cutting edge (its offset set). A tool can have several D numbers; every data field in the offset memory is invoked with a T and a D.
Can I write tool offsets from the program?
The values P1…P25 of the offset memory can be read and written through system variables. But this directly changes how the machine cuts, and access level and write timing come into it. For someone starting out, the right route is the panel.
How large a wear value is acceptable?
It is a correction, not a substitute for the tool. A large deviation is usually not wear but a broken tool, a wrong geometry entry or a clamping problem. Getting used to large corrections hides the real fault.
Can I use the same tool with different offsets for roughing and finishing?
Yes — define a second cutting edge (D2) and keep a different radius or wear value there. In the program you call T1 D1 and T1 D2.
What goes in the radius cell for a slotting saw?
On the saw type, $TC_DP6 is the diameter, not the radius, and $TC_DP7 is the slot width. That is exactly why entering dimensions before setting the tool type correctly is wrong.
Does this apply to an 828D as well?
The structure of the offset memory and the meaning of the $TC_DP parameters are defined in the manual shared by 840D sl and 828D. Panel screens, softkey names and menu paths vary with the control version, the options that are active and the machine builder’s configuration.
Sources
- Siemens AG — SINUMERIK 840D sl / 828D Job Planning, Programming Manual, 01/2015, document no. 6FC5398-2BP40-5BA2: Section 10.1 Offset memory — T/D number structure, the “Flat D No.” structure, reading and writing P1…P25 through system variables, and the
$TC_DP1…$TC_DP25parameter table (pp.366–368); corner-rounding evaluation rules for tool types 110, 120/156, 121 and 131 - Siemens AG — SINUMERIK Advanced CNC Operation and Programming, 05/2010: Section 2.1 Measuring tools, 2.5 Measuring tools in JOG (TCP and matching CAM, entering tool offset data by hand, the “Radius / Length / Calibrate tool probe” options, the V offset)