GibbsCAM Online
GibbsCAM Forums

Most Popular
Recently Added
Recently Updated

Mill Post Label Definitions and Code Issues

Mill Post Label Definitions and Code Issues

Mill post names use letters to signify their capabilities. The designation may be a single letter or multiple letters to specify the post's capability. Following the letter designation is a unique number for this post.

The general format of a post can be described as :

<control name>[client initials]###.##

Note that a metric post will end with an “m”.

Following is a description of how Mill Posts are named and what they do. Also included are brief explanations of code issues that might be encountered in Mill Posts.

3-Axis Mill

Label Definitions:

  1. M – This designates a regular 2- or 3-axis mill post. A 3-axis mill post has 3 linear axes (X, Y, and Z) that can position and cut simultaneously.
    Example: Fanuc 6M [VG] M001.19
  2. N – This designates a mill post that does not use subprograms. This is known as a "Long Hand post". Subprograms are frequently used for multi-process drilling, Z-repeat milling, patterns, thread milling, rough & finish mill bore, multiple parts, etcetera. Any mill post can be modified into a Long Hand post.
    Example: Fanuc 6M [VG] NM001.19
  3. U – This designates a Mill post that supports Spline Interpolation (also known as NURBS).
    Example:
    Fanuc 15M [VG] UM001.19

Code Issues:

  • Cutter Radius Compensation

There are two different Cutter Radius Compensation (CRC) options available in the system: From Tool Center and From Tool Edge. This preference can be found in FilePreferencesMachining.

From Tool Center outputs code to the center of the tool in contouring and roughing operations.

From Tool Edge outputs code to the edge of the tool in contouring operations. However, it outputs to the center of the tool in roughing operations.

Most CNC machines require that CRC be turned on (e.g. G41/G42) on the entry line move and turned off on the exit line move. The entry and exit moves immediately preceed and follow your toolpath moves and is programmed in the process dialog window.

If the From Tool Center option is selected, the value entered into the offset register on the control should be 0. The system has already compensated the values in the output by the tool radius.

If the From Tool Edge option is selected, the value entered into the CNC control’s offset register should be the tool radius. The values in the output are to the edge of the tool.

  • Sub-programs/Sub-routines vs. Long Hand g-code

Prefer Subs - This checkbox only toggles between subprograms and long hand output for multiple Z steps in contouring and roughing operations. It will not eliminate all subs in your program or even for this operation.

The Prefer Subs checkbox is not available for drilling operations. If multiple processes are used for multiple holes, drilling subprograms will be created.

Patterns, multiple parts, and rotary repeats will always output sub-programs in a standard mill post.

If a Longhand post is used no subprograms will be output.

  • Absolute Subs vs. Incremental Subs

The system will generally only output incremental sub-programs during Pattern, Mill Bore, and Thread Milling operations.

A subprogram that uses ramping or helical milling for entry moves output these moves in incremental. After the entry moves are complete, the subprogram switches back to absolute for all remaining moves.

If incremental output is selected in the Post window, all moves are incremental.

Advanced Mill

Advanced Mill is an option in GibbsCAM. An Advanced Mill post is needed when coordinate systems are defined in any part. An Advanced Mill post has the same capability as a 3-axis post. A 3-axis post is no longer needed if an Advanced Mill post is available.

Label Definitions:

There are three different letter designations for Advanced Mill Posts:

  1. B – This post style is useful for multiple setups of the same part, tombstone work and machines without automatic rotation capability.
    • The “B” style post uses a Work Fixture Offset for any machining coordinate system. All of the X-, Y-, Z-, A- and B-axis offsets must be stored in the control's Work Fixture Offsets. The output of the rotary axes will always be zero (A0 and/or B0). The X-, Y-, Z-, A- and B-axis offsets are output in the operation comments.

    Example: Fanuc 6M [FW] B001.16.pst

  2. C – This post style is useful if you have a 4th and/or 5th axis rotary table.
    • The “C” Style post also use Work Fixture Offsets for any machining coordinate system. Only the X-, Y- and Z-axis offsets must be stored in the control's Work Fixture Offsets. The A- and B-axis rotations are output in the G-code. The X-, Y- and Z-axis offsets are output in the operation comments.

    Example: Fanuc 6M [PW] C001.16.pst

  3. D – This post style is useful for 4th and/or 5th axis parts where you do not want to use Work Fixture Offsets. It is also useful if you do not like having to input data into the control's Work Fixture Offsets.
    • The “D” Style post uses one Work Fixture Offset for the entire part. This means that the X-, Y- and Z-axis values in the G-code are offset based on the machining coordinate system. The A- and B-axis rotations are output in the G-code.

    Example: Fanuc 6M [NW] D001.16.pst

Most customers use either a “B” or “C” style post. Both the “B” and “C” style posts fall back to “D” style output if they exceed the maximum number of work fixture offsets available for a particular CNC machine.

Code Issues:

Advanced Mill vs. Simple Positioning and/or Rotary Mill

An Advanced Mill post is incompatible with a Simple Positioning and/or Rotary Mill post. If you use coordinate systems to specify rotations, you need to use an Advanced Mill post.

Master Clearance Plane

The value entered into the Z clearance plane in the Document Control dialog is a fixed point in space. This position or location is not relative to the current coordinate system. In other words, this value is always local to the home coordinate system.

This value is output at the beginning of each new tool operation and at the beginning of a same tool operation if there is a new coordinate system specified.

If this value is not entered correctly, it is very possible that the system will produce unexpected negative Z rapid moves. Therefore, It is essential to make sure this value is clear of the part during all machining coordinate system rotations.

Rotate to Shortest Distance

The system calculates the shortest distance to rotate from one coordinate system to another. For example, the system will output a positive move in the clockwise direction to get from 270° to 0° degrees. The system will output a negative move in the counterclockwise direction to get from 90° to 0°. The system will output either a clockwise or a counterclockwise move to get from 180° to 0°.

4-Axis Simple Positioning

Rotation information entered in the system's Rotate Tab is output in a simple positioning post. A Simple positioning post uses either the A OR B-axis to rotate the part into position. A Simple Positioning post has the same capabilities as a 3-axis post. A 3-axis post is no longer needed if a Simple Positioning post is available.

Label Definitions:

1. P – This designates a 4th axis positioning post. A simple positioning post will output an A-axis move in the G-code. No Work Fixture Offsets will be used in the rotation of the part.

Example: Fanuc 6M [VG] PM001.19.pst

2. Y – This designates a simple positioning post which will output a B-axis move in the G-code. No Work Fixture Offsets will be used in the rotation of the part.

Example: Fanuc 6M [VG] YPM001.19.pst

3. Any Simple Positioning post can be modified into a Long Hand post.

Examples: Fanuc 6M [VG] NPM299.19.pst

Fanuc 6M [VG] NYPM299.19.pst

Code Issues:

1. Simple Positioning vs. Advanced Mill

a. A Simple Positioning post is incompatible with an Advanced Mill post. If you use coordinate systems to specify rotations, you need to use an Advanced Mill post.

2. Origin of Rotation

a. In Simple Positioning, the origin of rotation of the X-, Y- and Z-axes must be 0.

Rotary Mill

If you program Wrapped Geometry, or choose the Rotary Milling radio button in the Rotate Tab, you will need a Rotary Mill post. A Rotary Mill post uses either the A OR B-axis to rotate and machine the part simultaneously. A Rotary Mill post has the same capabilities as a 3-axis post. A 3-axis post is no longer needed if a Rotary Mill post is available.

Additionally, a Rotary Mill post has all the capabilities of a Simple Positioning post. If you order a Rotary Mill post, you will not need a Simple Positioning post.

Label Definitions:

1. R – This designates a 4th axis Rotary Mill post. A Rotary Mill post will output an A-axis move in the G-code. Cutting of wrapped arcs will be broken into linear segments. No Work Fixture Offsets will be used in the rotation of the part.

Example: Fanuc 6M [VG] RM001.19.pst

2. Y – This designates a 4th axis Rotary Mill post which will output a B-axis move in the G-code. Cutting of wrapped arcs will be broken into linear segments. No Work Fixture Offsets will be used in the rotation of the part.

Example: Fanuc 6M [VG] YRM001.19.pst

3. I – This designates a Rotary Mill post that supports Cylindrical Interpolation. A Cylindrical Interpolation Rotary Mill post will output a G2 or G3 with rotary moves.

Examples: Fanuc 6M [VG] IRM001.19.pst

Fanuc 6M [VG] YIRM001.19.pst

4. Any Rotary Mill post can be modified into a Long Hand post.

Examples: Fanuc 6M [VG] NRM299.19.pst

Fanuc 6M [VG] NYRM299.19.pst

Fanuc 6M [VG] NYIRM299.19.pst

Code Issues:

1. Rotary Mill vs. Advanced Mill

a. A Rotary Mill post is incompatible with an Advanced Mill post. If you use coordinate systems to specify rotations, you need to use an Advanced Mill post.

2. Origin of Rotation

a. In Rotary Milling, the origin of rotation of the X-, Y- and Z-axes must be 0.

3. Rotary Feedrates

a. Most rotary feedrates are calculated in Degrees Per Minute per rotary segment based on its length. Since the length of each segment is variable, the system outputs a different feedrate for each segment. The resulting rotary feedrate can be a large value based on the Degrees Per Minute calculation.

b. Certain CNCs, such as Haas and Mazak, calculate rotary feedrates using Inverse Time. Any Rotary Mill post can be modified to use Inverse Time for feedrates.


Properties ID: 000084   Views: 10292   Updated: 8 years ago
Filed under: