This part will have some profiling on the OD (Outside Diameter).
- Select MODE to get to the control’s Main Menu.
To make the part, we are going to load the DXF file from the common drive or using a flash drive. We’ll then create a cycle program and machine the part manually or using CNC mode.
The following are steps for loading the DXF program and machining the part.
Step 1 – Uploading DXF
Press MODE – PROG IN/OUT – OPEN
Use TAB, DATA DWD, and DATA BACK soft keys to access the DXF file from M Drive or D Drive if using a flash drive. You may need to change the file extension tab to .DXF or .PT4 in order to locate the file.
Select the file named LathePractice.Part and press OPEN FILE.
Press CONTINUE to move to the next step.
Press YES to close lines gaps to the specified tolerance.
To select the absolute zero position, select C and select the front arc to place the origin at the center of this arc. A red square will be indicated as shown below.
- Press CONTINUE.
- Press X POS to show the drawing line view corresponding to the side the tool will track along. This removes half the drawing. Press CONTINUE.
- Press HIDE LINE to remove the vertical lines across the part profile. Click on the line to highlight and click again to delete line.
- Press CONTINUE.
- Select CYCLE and click YES to chain events. Click on the arc to set the cycle start position, then on the next line to create the chain as shown below. All the lines will be highlighted.
- Click on the event icon shown on the top right corner of the controls window. A drop down menu of cycle event #1 appears as shown below.
- Enter the following specifications: For X Stock, enter 1.2; Depth of Pass enter 0.03; Z approach; RPM/Surface Speed enter 200 sfm; Feed per Min or Rev enter 0.01 IPR; Tool #1; Fin Cut enter 0.005; Fin RPM/Surf Speed enter 300 sfm; Fin Feed Min/Rev enter 0.003 IPR; Fin Tool #1.
- Event #2 window indicating ALL OK at the top right corner appears as shown below.
- Click EVENT icon to hide the event windows. Press END DXF – YES. You’ve finished importing the DXF and setting parameters for CNC program.
Step 2 – Setting Raw Material
- Obtain 1” diameter aluminium stock from stock area, about 3” long.
- Hold stock in 1” collet and secure collet on chuck using ratchet. About 2.3” stock should stick out from collet/chuck. Use a chuck key to secure collet firmly.
- Select tool #1 by pressing tool # soft key then enter  and press Abs Set.
- Press Spin Speed, enter , and press Inc Set to set the spindle speed to 1000 revolutions per minute (RPM).
- Turn on spindle and face part as demonstrated in Setting Up Tools Tutorial and set Z = 0 on faced side.
- Move tool away from part and turn off spindle
Now we need to enter or confirm the current information in the tool library. Refer to Setting Up Tools Tutorial.
- Press MODE to return to control main menu
- Press SETUP
- Press REF POSN to confirm tool reference position is set to X = 4.000, Z = 4.000. NOTE: It’s very important that the reference position is set to avoid crashing tool into part and/or chuck.
- Press RETURN to exit REF POSN.
- Press MODE – PROG – GO TO BEGIN to confirm the information on the program. You can press look to display the cycle events profile. Note: The cycle position events are automatically added by the machine.
- Press TOOL PATH to view the tool path graphic. If there is a program error it will be displayed now.
- If everything is OK, press MODE to return to the Main Menu.
Step 3 – Running Program
- Press RUN to enter run mode.
- Press START to cue up the program from the beginning.
- Note – the prompt invites you to press GO when you are ready to execute the program. If you press GO now – the machine will move in rapid speed up to the part and will enthusiastically begin to execute the commands you have entered. But what if you have made a mistake? You could have a crackup and damage the tool, the part, or yourself. So let’s be safe – here is a mode you should use the first time you run a new program:
- Press TRAKING. This will allow you control the rate of program execution by moving the hand wheels.
- Follow the screen prompts;
- Put in TOOL #1.
- Turn the spindle on.
- Press TRAKING
- Z- Axis hand wheel is used for aggressive feed.
- X- Axis hand wheel is used for fine feed.
- Turn the x hand wheel to machine the part. Continue turning until the program runs over and the tool retreats to the home reference position.
- Inspect the part dimensions.
Your part is ready.