dfab Laguna CNC Manual With FANUC Control 1 Introduction Throughout this manual we use different nomenclature for [HARD KEYS] and (SOFT KEYS). A [HARD KEY] is a button on the CONTROL PANEL (upper panel) or MACHINE PANEL (lower panel) which does not change; these keys have labels printed on them. The row of unlabeled keys at the top of the control panel allow the user to select various states and actions noted above the keys, these are (SOFT KEYS). 2 General Machine Safety Never step inside the painted line while the machine is in operation. Always check with operator (the individual in front of the control) prior to walking inside the painted lines or touching the machine. Everyone in the machine shop must use Safety Glasses whenever the spindle is on Hearing protection is advised for everyone in the machine shop while the CNC spindle is on Always firmly check the fixture (vacuum table hold down or other fixture devices) prior to running a job Do not make any changes to offset values Do not make any changes on the control other than what is outlined in this document (loading and deleting files) Do not use the MDI for purposes not outlined in this document (tool recovery and tool change). 3 Power up procedures 3.1 Safe Power Up Turn the switch on the machine side of the control Wait for the display screen to show the position page 3.2 Zero Return A zero return for the z-axis must be performed after power up. Press [REF] to change into reference mode, then press and hold [+Z] until the Z axis stops moving at the top of travel. When in Reference mode with [REF] key lit axis motion is restricted to the direction toward reference position, you will not be able to move the axis down toward the table. 3.3 Spindle Warm Up Running the spindle without a tool loaded will catastrophically damage the draw bar. The draw bar is the device inside the spindle that securely holds our tools. DO NOT RUN THE SPINDLE WITHOUT A TOOL LOADED.
You need not press any buttons to warm up our spindle. There is code posted in your file which will warm up the spindle if the [BLOCK SKIP] button is not pressed on the MACHINE PANEL. 4 Run your first work piece 4.1 Save a Program on the Network Drive Before posting gcode to our server, have a qualified shop technician review your toolpaths, simulation and gcode. File names must be 5 characters (not including the extension) or less. ABCDE.nc works fine, ABCDEF.nc will not work. The root of the network drive is located here: \\picasso\courses\_student Resources\dFab\Shared\ Laguna DO NOT SAVE YOUR FILE LOOSE IN THIS DIRECTORY. First create a folder, either in your class folder, or if you have been approved, make a folder in this directory that is your full last name and save your file inside that folder. 4.2 Load a Program from the Network Drive You have already posted your gcode from RhinoCAM, verified the toolpaths through the simulation screen in RhinoCAM and reviewed both your posted gcode and toolpaths in RhinoCAM with a qualified dfab technician. Press [EDIT] [PROG](OPRT)(EMBETH) and navigate to your folder using the arrow, page up down, and input keys. Navigate to your file and press (+) (+) (F INPUT) (+) (F GET) (+) (EXEC) The (+) key is the right arrow SOFT KEY Your file has now been saved to memory. To verify this, press [PROG]. You will see your gcode and will see //CNC_MEM/USER/PATH1/ at the top of the screen. 4.3 Prepare To Run Your Program for the First Time 4.3.1 Operator Position When the machine is in operation, the operator will have their left fingers covering [CYCLE START] and [CYCLE STOP]. Their left hand will be holding the FEED OVERRIDE KNOB. Practice turning that knob from 100% to zero twice at this time ensuring you are able to turn that knob quickly to zero. Your right hand will be covering [CYCLE START] and [CYCLE STOP]. Pressing [CYCLE STOP] will do the same thing as turning the FEED OVERRIDE KNOB to zero percent.
4.3.2 Spindle Warmup Press [EDIT] [PROGRAM] (CHECK) You will now see a screen that shows the four coordinate systems, all active G codes on the left and your program file on the right. Press [AUTO] on the MACHINE PANEL and the distance to go coordinate system should populate with zeros. By pressing [AUTO] The machine is active. BE CAREFUL NOT TO PRESS CYCLE START. Ensure that [SINGLE BLOCK] is DISABLED and the light above it is NOT lit Ensure that [BLOCK SKIP] is DISABLED and the light above it is NOT lit Ensure that [OPT STOP] is ENABLED and the light above it is lit While covering the FEED OVERRIDE KNOB, press [CYCLE START]. The machine should move to the tool change position and pick up your first tool. It will then make a rapid move to the top limit of Z travel and turn on the spindle. Turn the FEED OVERRIDE KNOB to 0% and insure that [OPT STOP] is enabled The spindle will automatically cycle through 3 speeds for a total of 5 min warmup. After which it will turn off the spindle. You may walk away from the control while the warmup cycle runs. 4.3.3 Verify Your Work Offset After following the previous steps in this section, we will slowly approach our starting position in XY and then follow that by slowly approaching our starting position in Z. 4.3.3.1 Verify the XY Location of Your Work Offset Set FEED OVERRIDE KNOB to 0% and enable [OPT STOP] Press [CYCLE START], look at the DIST TO GO values. You should see negative X and Y values, Z should be 0.0000. Now increase the feed override slowly and motion will occur. Turn the knob around slowly at first, under 50% and get a feel for how the knob controls motion speeds. Visualize a target location on the path of motion and practice stopping. While the machine is moving, we watch the machine in motion. After you have stopped motion by turning the knob to 0% you may look away from the machine and check your DISTANCE TO GO coordinates on the display screen. After referencing the DISTANCE TO GO values, pick a new location on the bed as your target and repeat the above process attempting to stop the machine just before your target location. Because [OPT STOP] is enabled, the machine will pause the program at the end of this move, read the highlighted commend on the display and follow directions, in this case the comment reads Turn FEED OVERRIDE KNOB to zero. Press [CYCLE START], increase feed carefully as tool approaches. This step is explained in detail in the next section. 4.3.3.2 Verify the Z Location of Your Work Offset Set FEED OVERRIDE KNOB to 0% and enable [OPT STOP]
Press [CYCLE START], look at the DIST TO GO values. X and Y should read 0.0000; Z should read a negative number, the distance between your part and the end of the tool plus one inch because we set our clearance plane to 1.000 above the surface of the material. While watching the spindle plunge toward your work piece, stop motion approximately 2 inches above the surface of your material. DISTANCE TO GO should read close to -1.000 when you stop, implying that the Z axis has another 1 inch of motion left in the current move. If you stopped 2 inches above your material and DISTANCE TO GO reads a number that is not close to 1 leave the FEED OVERRIDE KNOB at 0% and press [RESET] on the MACHINE PANEL, then figure out what went wrong. If all looks correct, you may turn the feed override back up until we complete this block of code. Because [OPT STOP] is on, motion will stop at the end of this line of code. You will see a comment in the code. Follow directions, the tool should be exactly 1 off the surface of your material. 4.3.4 Run Your File After verifying that your work offset is correct we are ready to execute the rest of your file. This is possible because we have carefully verified the program from this point forward through our software verification process in the computer. It is imperative that you carefully checked each toolpath for collisions on the computer and have not programmed any tools to cut deeper than their cutting edge length, which is saved with each tool in our library. Turn the FEED OVERRIDE KNOB to 100%. With your hand ready to crank FEED OVERRIDE KNOB back to zero, press [CYCLE START] make some sawdust! At the next tool change you will be prompted to check the tool length again. Follow instructions and then press [CYCLE START] to continue. Each time you run a new file, you must watch the entire program run with [OPT STOP] enabled while standing in front of the control, with your hand ready to stop the feed override. If anything happens which is unexpected, such as a tool cutting too deep. Turn the FEED OVERRIDE KNOB back to 0% and press [SPINDLE STOP] or press the [RESET] button. 4.3.5 Delete Program from Memory You must remove your program from the local memory after making the cut. Press [EDIT] [PROGRAM] (FILE) (OPERATE) (DEVICE) (CNCMEM) Navigate to your file then press (+) (DELETE) (EXECUTE) 4.3.6 Clean Up After the file completes running, you will get out the vacuum and clean up all the dust after removing your part from the vacuum table. We do not leave any tools in the spindle over night. T0 M6; Turn off the air at the end of the night as well.
5 Alarms and Recovery 5.1 Soft Over-Travel Alarm Soft over-travel alarms occur when an axis has traveled beyond a coordinate limit. To clear the alarm press [RESET] and jog the axis away (remember that the X axis jog buttons are transposed on the controller) It would be a good idea to re-reference any axis after a soft over travel alarm occurs see 3.2 Zero Return 5.2 Hard Over-Travel Alarm Any axis that creates a hard over-travel alarm will cause all axis to be in alarm state You must jog the axis off the switch before the alarm can be cleared. Bypass the alarm state by pressing [RESET] while holding down the [UNLABELED] button under [+X] and to the left of the [-Y] button. Continue holding the [UNLABELED] button and jog the over-traveled axis off the limit switch. 5.3 Recover a Tool Stuck On Tool Change Enter into MDI: G04 X10.0; M28; Press cycle start, walk around to tool changer (you only have 10 seconds) and support tool as tool changer carousel moves away. Be sure tool will not fall to floor. Walk back to control, press Jog, walk back to spindle and press tool release. Place tool back into carousel. Check that machine knows what tool is in spindle. [System] (PMCMNT) (DATA) Highlight D0400 Press (OPRT)(ZOOM) to see data in D0400. Verify that D0402 is set to 0 if there is no tool in spindle, or the tool number for the tool in spindle. Check that the machine knows the current tool changer carousel position. [System] (PMCMNT) (COUNTER) Check that C0000 is set to the current tool cahanger position in the current column. 6 Advanced Operations 6.1 MDI The MDI stands for Manual Data Input. It allows you to type in commands and run them at the machine. This is incredibly useful, but also quite risky because we cannot verify the commands that are typed. We ask that you not run MDI commands on our machine without first getting approval from Ryan McKibbin. You may however run the commands listed here, provided you type them EXACTLY as they are in the text. When a logical number should be added it will be revererd to as n. For example, in this text you will see Tn M6; If you wanted to pick up tool 3 you would type in T3 M6;
6.1.1 Tool Change Tn M6; (T0 M6; would leave the spindle with no tool) 6.1.2 Send machine to overnight position G53 Z0.0; G53 X30.0 Y100.0; 6.2 Search within a program Type in what you want to search for, and then press the down arrow key 6.3 Make a program already stored in memory the active program 6.4 Run a program from memory 6.5 Set new work offset 6.6 Set tool length offsets 7 Reference 7.1 I/O Channels 4 - PCMCIA (Memory Card) 17 - USB (You Know This One Dummy) 9 - EMBETH (Embedded Ethernet) 7.2 G Codes (Abridged) G00 Rapid Move G01 Linear Interpolation G02 CW circle G03 CCW circle G04 Dwell (Xnnn.nnnn) G43 Instate Tool Length Compensation (Hn) G53 Machine Coordinate System (non modal) G54-G59 - Work Offsets G81 - Drill G90 - Absolute Coordinates G91 - Relative Coordinates (don t use this)
7.3 M Codes (Abridged) M00 Program Stop M01 Optional Stop M03 Spindle on CW M05 Spindle Off M06 Tool Change M25 Servo Tuning Parameters (M25 R1. Speed, M25 R2. Balanced, M25 R3. Precision) M27 Extend Tool Changer M28 Retract Tool Changer M30 End of Program M48 Dust Hood Up M49 Dust Hood Down M401 Automatic Tool Touch Off (only for tools under 2 in length!)