Hurco
VM10U Mill
Tutorial
What
is the Hurco?
The Hurco is a 5-axis CNC milling machine. It has a 24-tool automatic tool changer. It can move its axes with a resolution of 0.0001 inch. (2.5 micron) Like the waterjet or laser cutter, the Hurco has no manual control capability other than jogging; to make a part with it you need a program.
How do
you program
the Hurco?
The Hurco can run two types of programs: Hurco conversational programs and G-code programs.
If you want to make a part from a print or a sketched drawing, entering a conversational program is a quick, easy way to do that. You can create and edit conversational programs directly on the machine's console.
A G-code program is a text file containing a list of commands for the machine to follow to make a part. A G-code program is a list of codes that are executed in sequence, line-by-line. There are two ways to get a G-code program.
The first is to use
The second approach is to write the G-code
yourself, either
in a text editor or by writing a program to output G-code. This is a great way to
learn about how G-code
works, and will provide you with invaluable knowledge when
trying to debug
G-code programs generated by
The Hurco has a hard disk drive and runs Windows. The easiest way to get programs on and off of it with with a USB thumbdrive.
Be
Careful to Avoid
Machine Crashes
With any program, whether it be conversational, G-code from CAM software, or G-code you have written yourself, it is possible for the program to crash the machine into the vise or the work, doing severe damage to our $150,000 machine. Therefore, you have to have a very careful attitude when writing and testing programs for the Hurco. On the other hand, we take bigger risks (e.g. driving, crossing the street) all the time; you just need to be careful, go slowly, and always have your finger on the "Feed Hold" button. Run your programs for the first time in single-step mode with the speed turned all the way down, and watch the machine closely; if it starts to do anything even slightly unexpected, press "Feed Hold" and check to see if there is an error in your program, tooling, or setup.
Where to get
Information
The Hurco mill has an excellent online help system built in that can guide you through any task. To access it, press the "Help" button on the console.
The Hurco mill has a 482 page manual, which we have placed online at the link below. It includes, among other things, a complete G-Code reference.
Another great source of information is the website http://www.hurconotes.com. This website includes step-by-step tutorials on basic operations such as jogging, setting machine zeros, and zeroing tools.
Step-By-Step
Tutorial
1. Turn the Machine On
a. Turn on power using red switch at rear.
b. Follow on-screen instructions to enable servo drive.
c. Press the soft-key to calibrate axes. Calibration rotates the axes through their full range; make sure whatever is mounted on the table is small enough to go through a full rotation; otherwise the machine will crash during calibration.
2. Create or load your program
Switching from NC mode to conversational mode (or vice/versa) will clear all of the tool and machine zeros. If you want, at any time you can save the zeros to a file (called an NC state file) and then load it later. But because switching modes clears the zeros, it is a good idea to load your NC or conversational program from disk, or to create a new conversational program, before setting zeros.
To load an existing program from the machine’s internal hard drive or from your USB stick, press the “Input” button and then the “Program Manager” softkey. To create a new program, then press the “New” softkey.
To edit your program (conversational or G-code) press “Input” and then the “Part Programming” softkey.
3. Install and zero tools
We keep a whiteboard next to the machine with a list of all of the currently installed tools and their tool-holder. In general, it is good etiquette to:
To jog
the machine
For many setup operations, you need to manually jog the machine. Jog capability is accessible from many of the screens, including Manual, Tool Review, and tool setup.
To jog the machine, switch the knob to the desired axis. (X/Y/Z/A/C) The “O” setting turns off the jog function. Set the jog speed by pressing one of the buttons. The speeds available are 0.0001 inch per click, 0.001 inch per click, or 0.01 inch per click. Turn the jog wheel to jog the machine. The fastest speed is good for gross positioning, the medium speed for fine positioning, and the slowest speed for bumping the tool against an electronic gauge block.
To
change tools
Press “Input”, then the “Tool Review,” softkey, then “Setup” softkey. Type in tool number into the box and press the ENTER key. Press the tool changer “Auto” button. Close the doors and make sure there is nothing obstructing a tool change, especially any of your body parts. Press the “Cycle Start” button to initiate a tool change.
To
install a new tool in
the machine
Obtain a CAT V-40 tool holder for your tool. There are end mill holders in the shop, as well as collet chucks and a drill chuck. Make sure the tool holder you use has one of the Hurco machine’s retention nuts screwed into the top.
If you use the collet chucks, MAKE SURE you snap the collet into the collet nut before installing the tool (get help if you don’t know how) otherwise it will be much harder or impossible to remove the tool from the collet chuck.
If you need to, you can purchase a variety of CAT V-40 tool holders from MSC direct or McMaster. There are all kinds of tool-holding products and adapters out there to choose from off-the-shelf.
There is a button on the spindle carriage to release the tool. Make sure you are holding the tool when you remove or re-install, to keep it from dropping. Above all, make sure you are holding the tool or tool holder below the lip that makes contact with the machine --- otherwise when the machine pulls the tool back in it will crush your fingers. If you are not SURE that you understand where to hold the tool, get John to show you.
To zero
a tool
It is good practice to zero tools off the table, rather than off the top of the work. This is essential for 5-axis programs, so the machine knows the actual height of the tool, and is good practice otherwise because it allows re-using the tool zero over multiple parts.
To zero a tool, press “Input,” the “Tool Review” softkey, and then the “Setup” softkey. Place the electronic gauge block on the table. Jog the tool down until its tip just touches the gauge block and causes the light on the gauge block to illuminate. Press the “Store Position” button. To compensate for the 2 inch height of the gauge block, click on the tool position box, then press 2.0 + Enter.
At this time, you can go through and set the other parameters, like the tool diameter, surface feed, and feed per tooth. For aluminum, 300 FPM is a good surface feed and the tool diameter divided by 200 is a good feed per tooth. These parameters are important for conversational programs, but not used for G-code programs.
4. Set Part Zeros
Tool 20 is an electronic edge finder. It has an elastically-mounted ball on the end, and lights up when the ball touches a metallic part. Do not run the spindle with the electronic edge finder; it is meant to be used with the spindle stopped. Also, be aware that the electronic edge finder requires a complete circuit between its shaft and ball to light up. If you are cutting metal and using metal fixturing, ordinarily you will have this; but if you are using wax to hold your parts, you may need to use an alligator clip to complete the circuit. With plastic parts, you could use a piece of copper tape as a metallic surface, or use a different edge finder.
Switch to tool 20.
Press “Input” and then the “Part Setup” softkey.
Bump the edge finder off the left side of the part. Press “Store Position.” If you want the zero at the left edge of the part, press 0.2 + Enter to compensate for the 0.2 inch radius of the ball.
If you want the zero in the center of the part, after pressing store position, bump the edge finder off the right side of the part. Then press XXX / 2 + Enter, where XXX is the part X position indicated at the right side of the part.
Use the same procedure to zero the Y axis.
To zero the Z axis to the top of the work, place the electronic gauge block on top of the work, then run the edge finder down so the ball just touches the gauge block and both light up. Press store position on the “Offset Z” box to record the Z position, then press 2.0 + Enter to compensate for the gauge block thickness.
5. Run the program
To run a program, press the “Auto” key, then press the “Run Program” softkey. When running a program for the first time, you can press the “Single” key to single-step the program.
In any case, it is a good idea to run with the rapid federate and axis federate at low levels, and to “cut air” first by applying an additional Z offset first, to make sure your program is doing what you think it should.
While you are running a new program for the first time, be extra careful to make sure that the machine does not crash into or machine through itself, the vise, or the table. This is very expensive to repair.
6. Turn the Machine Off
Break down your setup. Using the manual coolant nozzle and air hose, clean all chips off the table and machine axes. You can jog the machine around to help you reach parts of the machine. Be sure to switch the jog function off by switching the knob to the “O” position, and set the jog speed to the lowest speed, before reaching into the machine to clean it. Otherwise accidentally knocking the jog dial could cause the machine to move and crush some part of your body.
Thoroughly clean and dry the machine, and spray down with WD-40 to prevent rusting.
To turn the machine off, press the “Aux/Menu” key, then the “Utility Screen” icon. Press the Shutdown softkey. Press “Yes.” After the machine confirms that it is safe to shutdown the computer, turn off the red switch at the back.
Have fun and be safe!