June 2007 Edition

Controlling Interest

Principles of Machine Setup

Zero is nothing to argue about

I used to teach CNC. One of my classes argued for hours about the right way to set up a CNC machine tool. To prevent this from happening again, I developed the following ideas to explain the setup task:
      1. The work system is located with a translation from machine zero. While this translation can be the
vector sum of a sequence of translations, most users employ only the settable zero offset, G54.
      2. The machine coordinate system is the system of the servo axes. The origin of the machine coordinate system is synchronized to the work envelope of the machine with the reference return operation. Machine zero, the origin of the machine coordinate system, is the point in space occupied by the tip of the standard tool when the X, Y, and Z axes are at their machine zero position.
      3. All modern setup procedures use a standard tool, even if this fact is transparent to the programmer and operator. a. The machine zero point is the point in space occupied by the tip of the standard tool when the axes are at their machine zero position. b. When the standard is a tool of zero length; the tool is in the spindle; and the X, Y, and Z axes are at their machine zero position, the machine zero point is the point in space occupied by the tool reference point, since this is the tip of the zero length standard.
      4. Tool length offset and cutter radius offset are the difference in geometry between the actual tool and the standard tool. You program the path you want the actual cutting edge of the tool to interpolate and when length and radius compensation functions are programmed as well, the CNC takes care of tool geometry compensation.

The application of these ideas can be illustrated with a simple vertical bed mill of X, Y, and Z. The two examples that follow assume the Z-axis is “up” when it is at its machine zero position.

Machine Setup Diagrams: Job Shop without Preset Tooling
The method depicted in Diagram 1 is popular in job shops that do not use preset tooling.

Work zero is on the top surface of the workpiece. The operator chucks a tool and touches it to the work zero surface. The number the operator sees in the Z-machine display is put in the D-code as the tool length offset in Z. The operator does this for every tool.

In Diagram 1, the tool length offset is the air gap from the tip of the actual tool to the work zero surface.

Although the operator does not think in terms of a standard tool, the diagram shows that when the Z-axis is at its machine zero position, the standard is really a distance from the spindle gauge plane to the work zero surface. This distance does not need to be known.

Since machine zero is the tip of the standard tool when Z is at its machine zero position, machine zero is also on the work zero surface. Thus, the Z-register of G54 – or whatever settable zero offset is selected – is set to 0 because the translation from machine zero to work zero is zero.

If G53 is a blockwise cancellation of the zero offset, the command G0 G53 Z0 D0 positions the spindle all the way “up” by positioning the tip of the standard tool to the machine zero surface. The command G0 G54 Z0 D1 positions the tip of the actual tool to work zero. Be cautioned that G53 is not every CNC vender’s universal cancellation of all possible zero offsets. Siemens’ G53 does not cancel the base offset that plays a role in the next example.

Machine Setup Diagram: Preset Tool with Machine Zero “Up”
With preset tooling, the machine zero point is occupied by the tool reference point – the tip of the zero length standard – when the axes are at their machine zero position. Thus, when the machine zero position is “up,” the machine zero point is also “up.”

The value LL0 – a negative number – is set in the Z-register of the base offset.

The value LL3 – a positive number – is set in the Z-register of G54, or whatever settable zero offset is used.

It should be clear that the vector sum of base offset and settable zero offset is LL0+LL3. This sum is the vector LL4.

The command G00 G54 Z0 D1 positions the tip of the actual tool to the work zero surface. The command G00 SUPA Z0 D0 positions the spindle head “up” to its machine zero position. The Siemens’ SUPA (suppress all [offsets]) has been used instead of G53 because with Siemens, G53 does not cancel the base offset.

Norman Bleier manages Siemens machine tool applications engineering in support of U.S. OEMs. His special interest is technology on the shop floor.

What do you think?
Will the information in this article increase efficiency or save time, money, or effort? Let us know by e-mail from our website at www.ModernApplicationsNews.com or e-mail the editor at pnofel@nelsonpub.com.