G28 - Do you REALLY Know What It Does?

Most programmers use the FANUC G28 command to return an axis to the ZERO RETURN or REFERENCE RETURN position for a variety of reasons. Because this position is normally the position of the axis almost at one end of the stroke, those reasons range from tool change considerations to clearance considerations to safety considerations.

On a CNC lathe, REFERENCE RETURN or ZERO RETURN is the normally the axis at the farthest position away from the chuck - used mostly for safety and clearance reasons. On a vertical machining center, the Z axis is normally required to be at this position for a tool change sequence to start - an alignment issue here.. On a horizontal machining center, both Z and Y may be required to be there for a tool change alignment.

The How's & Why's of ZERO RETURN ?

The ZERO RETURN position is a very important position to the machine tool because this position never changes, even after POWER OFF. Basically, the ZERO RETURN position is a fixed position in which the machine tool builder uses a physical limit switch to obtain. The normal mode of operation when finding ZERO RETURN is that the axis rapids in the zero return direction looking for the signal from the limit switch that the dog has made contact. At that point, the axis slows to a feedrate set within the control and feeds until the dog feeds off the switch. At this point, the axis will begin to feed at a slower rate, a set number of pulses of the motor or set number of turns of the ballscrew. This final distance is called the GRID SHIFT and is usually adjustable through the machine parameters.

This type of system assures that the ZERO RETURN position will be arrived at even after power off and will be the same position, within tenths, all the time. For this reason, the ZERO RETURN position is very important to the machine tool and the programmer. It is the only position on the machine that can be found again and again after power off - because of the use of the "hard wired" limit switch. For this reason, most work coordinate systems (G54-G59) and PART ZERO locations are measured from the ZERO RETURN position.

In the newer machines and newer controls (referencing FANUC controlled machines with "red cap" axis drive motors), the zero return position is memorized within the control. Although the "hard wired" limit switch is used to set the position initially and after a CNC failure, once the position is found it is memorized in the control. This allows for a much faster movement to ZERO RETURN either through the program or in the manual mode. This system is commonly referred to as DOGLESS ZERO RETURN.

Usually on older machines, after POWER OFF, it becomes necessary to re-establish the ZERO RETURN position before operation can begin. Therefore, the first act upon power on of the machine should be to return the machine to the ZERO RETURN either by the manual method or thru the programmed G28 command. Oftentimes, machines are set up and will not allow automatic operation until manual reference point return is completed. This type of machine set up restricts the initial reference point return to manual operation only.

The Program and Zero Return ?

As mentioned above, it often becomes necessary in a program to send one or all of the axis to the ZERO RETURN position for any of the reasons outlined above. This can be accomplished in the program through the G28 - Return to Reference Point command. Although most programmers use this command, I have encountered many instances when I ask them why and how they use it, they simply say, "I don't know, that's the way we do it and it works?"

Like all movement commands, G28 can be made in either the ABSOLUTE mode (G90) or INCREMENTAL mode (G91). In either case, the movement is always made through an INTERMEDIATE POINT in the G28 command. The intermediate point is a point the tool will go through before proceeding to the ZERO RETURN position.

If G28 is commanded in the ABSOLUTE mode, that is with an absolute dimension after the G28, this absolute dimension is regarded as the INTERMEDIATE POINT and the machine tool will first go to this point before moving to reference return. For example, used in a machining center, one might command :

Machining Center Ref. : G00 G90 G28 X4.00 Y2.00 ;

Lathe Ref. : G00 G28 X4.00 Z2.00 ;

The above command would move the tool from the current position to the absolute position of X4.00 and Y2.00, then to the X and Y axis reference point return position. This is movement through an absolute INTERMEDIATE POINT. This can be used for safety or clearance reasons and eliminates the need for a seperate move to the clearance point than another command to the zero return position.

When used in the INCREMENTAL mode, the G28 can produce a move directly to the zero return position. For example, the machining center command of :

Machining Center Ref. :G00 G91 G28 X0 Y0 ;

Lathe Ref. : G00 G28 U0 W0 ;

The above command actually establishes an intermediate point of with an incremental distance in X and Y of 0. Therefore the tool moves to the intermediate point (no movement) then to the reference point. The end result is a direct move to the reference point. This is commonly used in programming.

As stated in the above examples, the Return to Reference Point is performed using the modal G movement command (G00 or G01) if not commanded in the same line as the G28 command. Therefore, good programming practice is to include the G00 or G01 on the same line as the G28 command.

Happy Chip Making !!

Check out our Real World World machine shop software at www.KentechInc.com

Conversational CAD/CAM

Quoting & Estimating

G Code Conversion

CNC Training

.... and MORE !!!