CNC working units

Working units may be determined by the number of decimal places seen on the CNC display panel.
Metric: 3 decimal places.
Imperial: 4 decimal places.

CNC feed rate units (F<n>)

Metric: mm/min
Imperial: in/min

CNC Spindle speed setting (S<n>)

Spindle speed is set manually on the mill itself and is not controlled by the CNC. The mill has two spindle-speed ranges: The LO range covers 60 to 500 RPM inclusive, whereas the HI range covers above 500 to 4200 RPM inclusive. The operating range is selected by a HI-NEUTRAL-LO lever on the right-hand side of the machine head. The lever places the head either in direct drive, for the LO speed range, or in backgear drive, for HI speed range. The backgear drive causes reversal in spindle spin direction. Though the CNC does not need to be told the actual spindle speed, it does need to know the operating range (i.e., the lever position) so that it can compensate for the backgear and maintain proper spindle rotation. (The CNC flips two phases of the power lines driving the spindle motor, when required, to keep spindle rotation consistent regardless of the speed range.)

Example: If you will be milling at 1000 RPM, you may use S<n> to program the CNC with a spindle speed anywhere between 501 and 4200, inclusive.

Stopping the Spindle

• If the spindle cannot be manually stopped when a cycle is interrupted press RESET. You should then be able to stop the spindle. This seems to be a problem when one is running a cycle by itself. If the cycle is part of a part program it is possible to stop the spindle when the program is interrupted.
• To stop the spindle at the end of a program place an M30 command at the end. (The CNC stops the spindle after it terminates a single cycle run in conversational mode. However, if you run a program consisting of an ensemble of cycles then you have to explicitly shut off the spindle in the program.)

Tool Change

• The spindle must be fully retracted so that the air wrench can engage the drawbar.
  - The CNC tool-change command T<n> positions the spindle at the proper height for the task.
  - To manually change tools, use the Z+ key to raise the spindle until the soft-limit is reached.
  
  Note: Support the tool while releasing it, otherwise it will fall to the ground!
  听
• To use the X-Y coordinates shown in the "change position" window issue the M20 modal command. Note that M30 cancels M20.

The cardinal rule in machining is to remove as much material as possible within the limits of machine capability. That is, to machine as quickly as possible. It is not so much a question of minimizing time wasted machining, but one of maximizing cutting tool life.

• Feed rates that are too low produce excessive heat which may cause premature failure of the cutting edge.
• Feed rates that are too high may cause the cutting edges to fracture or cause more catastrophic failure.
• Cutter speeds outside the recommended range may cause the cutting edges to experience buildup, wear excessively, crater, chip, or produce poor workpiece surface finish.

Cutting speed is the term used to express the velocity of the outside edge of the milling cutter (SFPM = surface feet per minute) as it cuts a specific material. Each material has an optimum range for its machinability with each cutting tool material (i.e. H.S.S., Carbide, etc.) Recommended cutting speeds are given in charts, usually as a range.

Feed rate (IPM = inches per minute) is the rate at which the cutting tool advances into the work. The allowable feed rate is governed by the cutter rotation speed (RPM), the number of cutting teeth on the cutter (called "flutes"), and by the size of the chip that the cutter can withstand (the chip load.)

Chip load (IPT = inches per tooth) is a measure of the chip thickness that one tooth can carve off of the workpiece. The recommended values for chip load are based on the cutting tool material, the cutting tool size, and the hardness of the workpiece material. The recommended values for feed per tooth are given in charts, usually as a range.

The formulae shown in the table bellow are used to compute the feed rate and cutter speed. The cut is assumed to be a slot of width equal to the tool diameter. The depth of the cut is specified in the tables that provide the SFPM and IPT values. As a rule-of-thumb do not bore deeper than the tool radius when making slots.

Alternatively, . (Note: This program returns different feed and speed values than those computed by hand using information on this page. The M-file uses a different set of tables for SFPM and IPT. This goes to show the variability of the RPM and IPM values.)

While the recommended feed rates found in charts represent good fundamental machining practice, they are however only recommended starting values. SFPM and IPT vary by material machined, material of the cutter, sharpness of cutter, type/amount of coolant used, depth of cut, milling machine horsepower, etc. Circumstances usually require deviation from these recommended values.

For instance,

• The feed rate used on small or thin work may need reducing.
• The work holding technique has a great deal to do with the feed rate. Setups lacking rigidity may require a lower feed rate.

Remember that using a chip load that is too small will cause excessive tool wear. Do not just set the feed rate low and think this is correct. A good rule of thumb is to start out at the low or mid range of chip load and increase the feed rate to the capacity of the machine tool, the setup, and the desired surface finish. Selecting the speed and feed for a job is an art and some judgment must be made based on common sense. For instance,

• Does the chip formation look good?
• Does the milling machine sound as if it is struggling?
• Does the finish look bad?

Approximate Cutting Speeds (SFPM)

Approximate Chip Load

Stopping the Machine

More important than knowing how to run your program is knowing how to stop the milling process.

• The <Cycle Stop> button stops program execution but does not stop the spindle from turning. (Machining resumes when <Cycle Start> is pressed. A typical use is pause machining to inspect the workpiece.)
• The Emergency Stop button stops the machine and is used to prevent catastrophes (it cancels any program execution and powers down the spindle and X-Y-Z axis motors.)

Know where these buttons are located on the CNC console. When something goes awry it can happen fast. Until you are confident of your part program keep your hand near these buttons and have an action plan.

Finding the Edge of a Part

Tool Calibration

Tool calibration is carried out with the icon shown above. The process consists of lowering a tool until its bottom reaches a fixed reference point and then having the CNC memorize the Z-coordinate. This reference point must be the same for all tools used to make a specific part. Since no universal vertical reference point has been setup on the mill one has to be improvised. Often a flat surface on the part being machined is selected. This surface then becomes the point defining Z=0.

Here are practical pointers:

• Turn on the spindle during the calibration process. In this way, should the tool be accidentally driven into the workpiece it will hopefully machine away the material and pose a lesser risk of damaging the tool or the machine.
• Step in the Z-direction with low speed. (Practice manipulating the tool with the tool away from objects so as to avoid collisions. Lower the table if necessary to create clearance.)
• Control step size using the jog control and use smaller discrete steps when nearing the reference surface.
• The tool height is noted when the tool just scratches the reference surface.

Check each tool's Z-zero level before machining!

After each tool is calibrated check that its length is properly defined in the CNC tool offset tables:

• Move the tool off of the workpiece so that it is in air.
• Issue Z 0 <Cycle Start> and confirm that the tool descends to the same height as the reference surface.
• Keep you finger on the <Cycle Stop> button to interrupt the command should the tool head for a collision.

听

Your Dry Run

You may graphically simulate the machining of your workpiece. Though the graphics are primitive they can indicate obvious programming errors. Even if you simulate your part, the first run of your part program should be executed with caution. Graphical simulation does not include such items as the equipment used to hold your workpiece and in a real program execution the mill may crash the tool into a clamp or a vise. Here are a few suggestions:

• Try a dry run in the air or on a scrap piece of stock (metal, wood, Styrofoam, etc.) just to see how the mill moves.
• While your program is executing - be it as a dry run or in production - keep your hand on the FEED dial. During questionable segments of execution, slow down execution speed by lowering the feed %. You can pause program execution by dialing in 0% feed.
• Always be aware of the <Cycle Stop> button and use it to stop program execution if something goes wrong. (Use the Emergency Stop button for catastrophes.)