This manual describes the concepts, programming commands, and CNC programming formats used to program ANILAM 5000M CNC products. Use the Contents and Index to locate topics of interest. In general, topics are presented in order of complexity. For example, “Section 1” describes basic CNC topics while later sections describe CAM programming and special programming features that require a firm grasp of CNC programming.
Some sections of this manual apply only to specific configurations of the 5000M CNCs. In these sections, icons in the left margin identify the configurations to which the information applies. Table 1-1 lists the icons for each CNC configuration and the number of axes supported by each.
5000M Three Axes System 3
5000M Four Axes System 4
5000M Five Axes System 5
NOTE: All systems also support one spindle axis.
The main difference between the configurations is the number of axes supported. Generally, this manual describes the 5000M three axes configurations. The four and five axes configurations operate exactly as the three axes configuration except for features that include the additional axes.
Before you start to write a program, determine the work-holding device and the location of Part Zero (the point to which all movement is referenced). Since absolute positions are defined from Part Zero, try to select a location that directly corresponds to dimensions provided on the part print, such as the lower left corner of the work. Then, you can develop a program using a procedure similar to the one that follows:
1. To enter the Program Directory from the Manual screen, press PROGRAM (F2). Create a program name for the part.
2. Enter the Program Editor (Edit F8) to open the new program and start writing blocks.
3. The first block of any program is usually a safe start position and toolchange position (a position away from the work where the axes can return for safe tool changing). The first block is normally also used to specify the units of measurement (Inch/MM), mode of operation (Absolute), and move type (Rapid) and to cancel all auxiliary functions (Tool Offsets, Spindle, and Coolant).
Typical first block: G70 G90 G0 X0 Z0 T0 M5
4. Subsequent blocks in the program set Spindle information, call Tool number, turn on Coolant, and make the initial move toward the work.
5. The remaining blocks in the program describe the required moves, Canned Cycles, and Tool changes to complete the machining.
6. The next to the last block in the program returns the axes to the Tool change position, turning off any auxiliary functions (Tool Offsets, Spindle, and Coolant). The last block (M2) ends the program.
Typical final blocks: M5
G0 T0 X0 Y0 Z0 M9
7. After you write a program, verify it. Run it in Draw Graphics Mode to troubleshoot for errors. Verify that all programmed moves are safe and accurate to the part print dimensions.
8. Now, load the stock material into the selected work-holding device.
9. Set the Tool Offsets for each tool in the Tool Page.
10. Before running the part in the Auto Mode, run it in Single-Step Mode to verify that both the program and the setting of Tool Offsets have been correctly completed. Single-Step Mode allows you to execute the program block-by-block.
11. After you test the program, make any necessary corrections.
12. When the finished program is ready for production, back it up on a floppy disk.
This section contains programming concepts for the beginning programmer. You must master these concepts and be familiar with the terminology in order to write programs.
A program is the set of instructions that the CNC uses to direct the machine movements. Each line of instructions is called a block. Each block runs independently, thus allowing the program to be stepped along, one block at a time.
The machine moves along its axes of motion. All movements along an axis are either in a positive or negative direction. Not all machines use the same system to identify axes. The descriptions used in this manual are commonly used to identify 3-axis mills.
Table movement along the X-axis is to the left and right. Positive motion is table movement to the left; negative motion is table movement to the right.
Table movement along the Y-axis is inward and outward. Positive motion is table movement outward; negative motion is table movement inward.
Spindle movement along the Z-axis is upward and downward. Positive motion is tool movement upward (away from the workpiece); negative motion is tool movement downward (into the workpiece).
The intersection of the X-, Y-, and Z-axes is the reference point from which to define most positions. This point is the X0, Y0, and Z0 position.
Most positions are identified by their X, Y, and Z coordinates. A position two inches left, three inches back, and four inches up has an X coordinate of X -2.0, a Y coordinate of Y3.0, and a Z coordinate of Z4.0.