G28 G53 Zero Return
G28 G53 Zero Return
CNC Training (Call 07834 858 407)
G28 is used to send a machine to Zero return for a tool change or at the end of a program.
G28 G91 Z0 (Z axis moves up to tool-change)
G28 G91 X0 Y0 Z0 (All three axis move to their respective zero return positions)
I know some of you don’t like three axis moves like the one above. If it don’t hit anything it’s just fine “Get Over It”
Below are the two ways of doing this.
Ignore This If You Get Bored Easily
G28 actually means return to the zero point via a reference point.
If you programmed
G28 G90 Z0 or you forgot the G91 this means return to zero point via a reference point. The reference point is Z0 so the spindle would rapid to Z0 (Bang) and then move up to reference return point.
Therefore if we use G28 G91 Z0 the first press will take it to the reference point which is incrementally zero form where you are (no move) the second press move to zero (no collision)
Some older machines won’t have this so try not to get over excited.
G53 uses your absolute machine position (Machine) this means all moves are from home position and are not affected by datums (G54 etc) or tool length offsets.
It is one of the very few non modal commands so you can’t write
X0 Y0 (this will use works offset not G53)
You need to write
G53 X0 Y0
Advantages Disadvantages (G28 G53 Zero Return)
G28 uses G91 incremental so you must remember to write G90 (absolute) for your next command. In fact many a collision is caused by misuse of G28.
G53 is best if you have it just remember it is non modal.
So you write it in each time you need it.
Some machines have return to tool change built into the tool change line.
On a Haas machine for example where the return command is built in you would not need to send the Z axis home.
I recommend that you always put one in.
If you are in single block you can stop before the tool-change if you wish.
Also I know someone who got into the habit of doing this and crashed a Fanuc Controlled machine that needed the command. (If you read this you know who you are)
G53 has another really good use and that is if you want the machine table (on a vertical machining centre) to move to a standard position to do things like changing the parts. It will always put the table in the same place regardless of work offset.
Bare in mind that if you put a position in that is relative to your work offset and not use G53 then the next time you set the fixture up your machine may over-travel because the fixture is in a different place.
If you read this article you will see how it could be used to set a vice in a known position regardless of datum.
Remember G53 is a position from the machine zero, it does not take into account the tool length offset or the datum. The other important thing is that it is non modal. That means you will need it on every line that you wish to use it for.
On Machines Like The BMC 800 from Toshiba
This machine has the Tosnuc 888 control.
For this control use G73 instead of G53.
If you have any questions about G28 G53 Zero Return or you are affected or have been affected by any of the issues in this post please contact me 07834 858 407
- CNC programming training.
- Want to learn CNC programming.
- Fanuc control training.
- Yasnac programming training.
- Any type of CNC course.
- Fanuc training courses
- CNC lathe training
- CNC Vertical Machining Centre training
Services offered at CNC Training Centre
Mazak Training Fanuc Training
Don’t forget we offer training on all types of Mazak Machines and all Fanuc Controls 6m to 31i Oi old to young.