SB CG1/Reference points

From wiki.fablabtoscana.it
GCode programming
modifica
Introduction

The relationship and interactions by machine, part and tool are called reference point.

A reference point is a fixed or selected arbitrary location on the machine, on the tool and on the part.

  • Fixed reference point is a precise location along two or more axes designed during the manufacturing or setup
  • Flexible reference point are established by the programmer:
    • Machine reference point: Machine zero or Home
    • Part reference point: Program zero or Part zero
    • Tool reference point: Tool tip

The key for a successful CNC program is to make all three groups to work in a coordinated way.


Machine reference point

The machine zero point (or machine zero, home position) is the origin of the machine coordinate system.

In general terms, a CNC machine has two, three or more axes, depending on the type and model. Each axis has a maximum range of travel that is fixed by the manufacturer. This range is usually different for each axis. If the CNC operator exceed the range on either the end an error condition known as overtravel will occur. Fanuc and manu other control system prevent automatic operation of a machine tool, unless the machine zero return command has been performed at least once - when the power to the machine has been turned on.

A good safety measure


On all CNC machines that use typical coordinate system, the machine zero is located at the negative end of each axis, excluded the Z axis that will be in the positive end.


Return to machine ZERO (HOME)

In manual mode the CNC operator moves the axes to machine zero position:

  1. Check visually the endstop for debris
  2. Turn the power on (control)
  3. Turn the power on (machine)
  4. Select machine zero return mode (Ref Z, etc. or Home All)
  5. Select Z as first axis
  6. Repeat for all other axes
  7. Check the position on screen display
  8. Check the machine reference icon


Mainly for safety reason the first selected axis should be the Z axis.

Homing a machine sets up the G53 Machine Origin. As example LinuxCNC uses this information along with your limits set in your ini configuration to enforce the soft limits you have set up for your machine.

G53 G0 X0 Y0 Z0 (rapid linear move to the machine origin)

G53 X2 (rapid linear move to absolute coordinate X2)

G53 G1 X10 Y10 Z-10 F100 (feed rate linear move to coordinate)


Part reference point

A part ready for machining is located within the machine motion limits. Every parts must be mounted in a device that is safe, suitable for the required operation and does not change position. The fixed location of the device is very important for consistent result and precision. Once the setup is established the part reference point can be selected.

This vital reference point will be used in a program to establish the relationship with machine reference point. The part reference point is commonly know as a program zero or a part zero

In theory the program zero point may be selected literally anywhere but in practical terms we should consider:

  • select a point easy to take
  • safety of working conditions
  • convenience of setup

CNC machining centers allow a variety of setup methods. Depending on the type of work some most common setup are used:

  • precision vises
  • chucks
  • subplates
  • machined jaws
  • special fixture


Program zero should be present in the drawings. In any setup make sure all critical dimensions and tolerances are maintained from one part to another.

Tool reference point

Every tool loaded into the machine is a different length. In fact, if a tool is replaced due to wear or breaking, the length of its replacement will likely change because it is almost impossible to set a new tool in the holder in exactly the same place as the old one. The CNC machine needs some way of knowing how far each tool extends from the spindle to the tip.

This is accomplished using a Tool Length Offset (TLO).

In its simplest use, the TLO is found by jogging the spindle with tool from the machine home Z-position to the part Z-zero position, as shown on the far left in figure below. The tool is jogged to the part datum Z and the distance travelled is measured. This value is entered in the TLO register for that tool.

3 ways to set tlo.png


The method shown in the center is much better and used in this guide. All tools are set to a known Z-position, such the top of a precision 1-2-3 block resting on the machine table. This makes it very easy to reset tools if worn or broken.

A tool probe is very similar to the 1-2-3 block method, except the machine uses a special cycle to automatically find the TLO. It does this slowly lowering the tool until the tip touches the probe and then updates the TLO register.

This method is fast, safe and accurate but requires the machine be equipped with a tool probe. Also, tool probes are expensive so care must be taken to never crash the tool into the probe.

Both the 2nd and 3rd methods also require the distance from the tool setting position (the top of the 1-2-3 block or tool probe) to the part datum to be found and entered in the Fixture Offset Z. The machine adds the two values together to determine the total tool length offset. A method for doing this is included

In milling and related operations, the reference point of the tool is usually the intersection of the tool center line and the lowest positioned cutting tip (edge).

For tools such as drills and other point-to-point- tools used in milling the reference point is always the extreme tip of the tool as measure along Z axis.

TRP.jpg