WORK NO. (NAME SEARCH <?INP> ( )

• Key in the desired work number (program number) i.e., 2525 and press Input. It is a good idea to check the Program File prior to this step in order to identify program numbers that have been used. At this point, there is a Menu option to program in either EIA/ISO (G-Code or

MAZATROL). Note: On some older model controls (M2 – M32 – M+) the EIA/ISO selection was an option and may not be available.

• Select MAZATROL from the Menu keys You are now ready to create the Common Data Unit which will be listed on the screen as Unit #0. The first prompting question encountered is:

MATERIAL <MENU>? ( )

From the Menu options, you should select the material that most closely matches the material you are using. This selection, along with the tool file information, affects the automatic calculation of feeds and speeds later in the programming process.

• Select AL from the Menu keys and Press Input

The material choices are given above the menu keys on the control and abbreviations for materials are; : CST IRN = Cast Iron; DUCT IRN = Ductile Iron; CBN STEEL = Carbon Steel; ALY STEEL = Alloy Steel; STNLESS = Stainless Steel; AL = Aluminum; COPPER = Copper. The last Menu key on the right has arrows pointing to the right (→ → → →) for a second page of additional material selections. These can be used for user defined materials.

Note: All Cutting Condition Parameters are based from Carbon Steel (e.g. Plain Carbon Steel 1018). All other materials are a percentage factor of this. You may develop new materials specific to your application with this criteria in mind. See the section in your Mazak User Manual provided with the machine for details on assigning Cutting Condition Parameters.

INITIAL POINT- Z (CLEARANCE)? ( )

For specific details, see the preceding text in this section for a description of Initial Z Clearance question to establish the Z Plane.

• Key in 1.0 and press Input

ATC MODE ZERO RETURN <Z.X+Y:0, X+Y+Z:1>? ( ) This sets the path the spindle is to take for the Automatic Tool Change Mode. See existing text for a more detailed description of ATC MODE.

• Key in 0 to select the Z first then XY movement and Press Input MULTI MODE <Menu>?

See the existing text in this section for details regarding whether there are multiple parts on the table, or not.

• Select MULTI OFF from the Menu keys MACHINING UNIT <MENU>? ( )

The following choices are available to choose from: POINT; LINE; FACE; MANU Part

AL PROGRAM; OTHER; WPC; OFFSET; END and, SHAPE CHECK. (See Figure 8).

• Choose WPC from the Menu select keys

This is UNo.1 WPC = Workpiece Coordinate. Use this unit to identify the location for the part zero of the geometry from machine home. These values are usually measured using an edge finding device or probe system and input within the program or the offset registers. You may also set this item to use G54-G59 and additional offsets of A – K. Consult the Operation Manual of your machine for specific instructions on setting these values. A number can be assigned, in order to include multiple WPC’s within the same program.

• Press Input or use the right pointing cursor key to accept a value of 0 for our WPC number

• Press Input again to pass over the Additional Offsets

At this point, you will be prompted as follows:

WORKPIECE COORDINATE, WPC - X? ( )

WORKPIECE COORDINATE, WPC - Y? ( )

WORKPIECE COORDINATE, WPC - è? ( )

WORKPIECE COORDINATE, WPC - Z? ( )

WORKPIECE COORDINATE, WPC - 4? ( )

• Input 0 in each case for now

Setup Notes: The exact coordinate values for each of these offsets will be measured during the setup process and entered via WPC-MEASURE, WPC SEARCH. Position an edge finding device in order to find the workpiece edge along the X axis. Press the TEACH Menu key and key in a value (0) that represents the location of the spindle, in relation to the Workpicece Zero, and Press Input. Don’t forget to compensate for the radius of the edge finder. Repeat these steps for the Y axis. Input 0 for the workpiece rotation angel of Theta. All cutting tools used in the program should be installed in the magazine and measured to the tool sensor prior to workpiece coordinate setting. For the WPC – Z, position any tool that is used in the program and touch off the top most surface of the part. Remember, sometimes this top-most surface is above the finished surface zero. This is the case in our example, so once the tool is touched-off along the Z axis, Press TEACH, key in -.05 and Press Input. Input 0 for the 4th axis workpiece coordinate. When all these data are entered, a new unit (UNo.2) is started.

MACHINING UNIT <MENU>? ( )

Often, it is necessary to machine the work surface to establish a Z -0 work face. It is commonly at the beginning of the program for this reason. The following choices are available to choose from for Face Machining: FACE MIL; TOP EMIL; PCKT MT; PCKT VLY . (See Figure 8).

• Select FACE MIL from the Menu keys

Figure 19 Face Machining Menu Keys

Once the Face Machining menu key is pressed, there are columns with the following headings displayed on the screen: DEPTH, SRV-Z, BTM and FIN-Z. DIST: WPC Z0 TO FIN SURFACE? ( )

• Input 0 here because this represents our finished surface for Z

Z AXIS STOCK REMOVAL? ( )

• Input .05 here because there is that much excess material to remove

BOTTOM ROUGHNESS <MENU>? ( )

• Choose from 6 from the Menu keys

This will automatically set the Z depth of cut for the roughing (.0402) and finishing (.0098) passes. A number system of 1-9 is used here that relates to surface finish. Higher number the more fine the finish. This number affects the finish depth of cut.

• Press Input

Figure 20 Bottom and Wall Roughness Menu Keys

The following Figure identifies the approximate surface Micro Finish that is created when each of the numbers are selected. For example, selection of Menu key 6 will produce a 32 Micro Finish.

Figure 21 Surface Micro Finish Chart