Machinist Job Set Up (Making The Connection)

In Setup by Micah HoffmannLeave a Comment

Machine Home and Part Origin

  1. The machine home position is a physical location of the machine that is set by the manufacturer.
  2. Each machine will have a “work envelop” which should be maximized with the proper machine home.
  3. The part origin will ultimately be a Cartesian offset from the Machine 0,0,0. (See pic1)
  4. If datum’s are specified on the blueprint, the part origin must be the intersection of those three planes.
  5. If GD&T is not in use, then the Machinist should consider where the majority of the dimensions are coming from.

work offset xy from machine home Picture 1

Find the Edge

  1. The standard edge finder will have a .200 (two hundred thou) cylindrical body.
  2. With the edge finder loaded with the spindle turned on, first assure that the probe body is offset from center. (See Pic2)
  3. The set up worker should then jog/tram the axis in focus. We stop when the probe is realigned.
  4. The values that are displayed will be your Axis 0. Remember you must account for the .100 offset of the edge finder probe body.

Using edge finder to get x and y Picture 2

MCU Input – G92 program shift or G54 Work Offset

Absolute Zero Shift (G92)

  1. Home the Machine
  2. Machinist will find the X/Y part origin.
  3. New values will appear on the machines jog display.
    1. Always remember to account for the .100 of the edge finder.
  4. The X/Y values that were determined via the edge finder are then used to edit the G-Code program.
  5. Insert the data in line with the G92 code except ALL Signs Reversed.


N01 G90 G20 G40 G80;

N02 G91 G28 X0 Y0 Z0;

N03 G92 X-10.0 Y5.0 Z0.0;

N04 T1 M06;

Note: This method has the drawback of having to edit the program each time the part origin is to be changed.

Work Offset G54

In most modern shops this will be the preferred method.  The key factor is whether or not your MCU supports this feature.  With this method instead of storing our part data directly in the program, we instead store it in the memory of the machine, then later reference it from our program.

  1. Home the Machine
  2. Machinist will find the X/Y part origin.
  3. Write down, or some machines allow you to copy the values from the MCU that are displayed after you find your part origin.
    1. You still need to account for the .100 edge finder offset if you are using that method.
  4. These values will be used for the work offset’s in the MCU memory.
    1. Also known as G54 G55 G56 G57 …

Note: This method is clean and flexible.  The operator has no need to edits programs at the MCU.

Work Offset

No Data No Data
00 X 0.00 02 X 0.00
Y 0.00 Y 0.00
Z 0.00 Z 0.00
01 X 3.123 03 X 0.00
Y 4.233 Y 0.00
Z 0.00 Z 0.00

This following program uses the work offset 01 = G54 to drive the machine to X1.25 Y1.25 offset from the G54 work offset in the machine memory.



N01 G90 G20 G40 G80;

N02 G91 G28 X0 Y0 Z0;

N04 T1 M06;

N05 G54 G00 X1.25 Y1.25 S3000 M03;

Tool Offset – Off the top vs 1-2-3 Block

The set up operator next has to make the connection between the tip of the tool and location of work offset Z0.

Off the top method

Picture 3

Details one way to set these values – off the top of the actual part.

tool length offset top of part Picture 3

  1. Set the spindle to full retract and load a tool.
  2. Slowly jog the tool down to touch the top of the part.
    1. Use the paper method to most accurately use this manual technique.
  3. Input the Z values displayed on the controller into the Tool offset page of your MCU.
  4. This needs to be carried out separately for each tool.

Based on the Machine travel values, the MCU memory will know the relationship between your part and your tools.

But, what if…

Your tool broke mid operation and the top of your part is gone?

You need to use a tool you didn’t load before the operation?

The part doesn’t have an easy surface to touch the tool off?

1-2-3 Block method

Picture 4

Instead of off the top of the part, make the same relation between tool tip and work offset Z0, off the top of a 1-2-3 block.

picture 4 1-2-3 block tool offset

  • Z0 of the G54 work offset is still the key value.
  • Begin by finding Z delta from top of the 1-2-3 block to top of the part.
  • Make sure you note whether the 1-2-3 top is above or below the Work Offset Z0.
    • This will determine if you add or subtract from the tool length distances before inputting into the MCU.
  • Touch each tool off on top of the 1-2-3 block.

Using the tool length offset data in your Program:

  • G43 Apply tool length offset to the tool in the spindle.
  • H5 directs the MCU to look in its memory for the tool in placeholder 5.

G43 H5

Leave a Comment