Newbie- G50 Shift?

[RC-CNC]

Hi,

I am struggling with understanding exactly what is going on when doing a G50 shift. Here is an example of the code I am looking at the beginning of the program:

$1
M118
M9
G99M52M97M6
G50Z-.015
G0Z-.05X.285


So am I to believe that when G50 Z-.015 is called, that is setting the Z Axis at 0 at -.015 over the part or away from the part?

Then when I do a Z-.05 move, where is the tool? Where is the steel?

Thanks a lot, still learning these swiss machines.

[HuFlungDung]

If this is standard usage of G50 and you are running in absolute mode, the line:
G50 Z-.015
implies that a new Z0 datum was set .015" in front of the current position.
So, the next line
G0 Z-.05
will cause the tool to move the incremental remaining distance, Z-.035 further towards the chuck. This will satisfy the new Z0 datum that was set with the G50.

[tobyaxis]

Originally Posted by RC-CNC Hi, I am struggling with understanding exactly what is going on when doing a G50 shift. Here is an example of the code I am looking at the beginning of the program: $1 M118 M9 G99M52M97M6 G50Z-.015 G0Z-.05X.285 So am I to believe that when G50 Z-.015 is called, that is setting the Z Axis at 0 at -.015 over the part or away from the part? Then when I do a Z-.05 move, where is the tool? Where is the steel? Thanks a lot, still learning these swiss machines.

All Cuts in the Stock are going to be Z+ while Z- is the opposite, (away from the tool).

Think about where the Z Axis Spindle is in relationship to the Cartesian Coordinate Table.

[cogsman1]

The G50 in THAT case is defining where the STOCK is as you start the program. There is a "theoretical" ZERO in your machine, the location of the the tool holder in the gang tool plate, and the cutoff tool you have in the machine has an insert that has an edge closer to the guide bushing by .010". You also need to have some material to face off, usually .005", so that is where the -.015" comes from. Now after this is read you will retract the cutoff tool and call the face tool into position. When you command "G0Z0" the stock will move OUT that .015" there by giving you .005" to remove during the facing operation. You should also note that at the END of the program after the cutoff you will see a line of code that sends the Main spindle BACK to that position WITH THE COLLET OPEN, "M6", "G0Z-.015". This is how you are able to run bar stock.

[RC-CNC]

Thanks for all replies!

Let me get this straight,

G50Z-.015 will do a GRID SHIFT (coordinate system set) setting the GRID 0 at .015 in the Z- direction. The machine will think that the end of the part (machine 0) is .015 away from the tool.

Z+ Z-
<- ->

Calling G0Z0 would then move the stock that .015 to make the shifted grid 0 be the same as the machine 0 thereby having the stock actually stick out .015 past the edge of the tool.

Doing a facing operation at Z0 would face .015 off the end of the part and establish the end of the part at machine 0.

The G0Z-.05 call moves the stock .050 away from the tool to allow for the tool to be retracted.



If I were to do a G50Z.015 (positive direction) shift, and then subsequently doing a G0Z0 call, the stock would actually retract .015 away from the tool and establish machine 0 as .015 AWAY from the tool (in space). Correct?

[cogsman1]

You are correct. This method although it seems rather insane to a "non" swiss person, allows a much cleaner program result than using offsets for tool geometry.
Attached is a pdf that explains more.

[UK-Engineer]

Hi

All the answers regarding your G50 query are correct but in case you were unaware (you did say you were a newbie) the M118 command is cancelling the collision detection at the start of the program. Although you often have to do this on the machines, (particularly when working close to the subspindle nut) you should be aware that you could potentially have a collision as the machine is not checking for this throughout the program.

I often thinks its best to cancel the alarm only when you need it. I find that depending on tool setup you can run programs on most Citizens (I assume your machine is probably a C16 or L20 machine?) without having to cancel the alarm at all.

Anyway good luck!

[tobyaxis]

Originally Posted by RC-CNC Thanks for all replies! Let me get this straight, G50Z-.015 will do a GRID SHIFT (coordinate system set) setting the GRID 0 at .015 in the Z- direction. The machine will think that the end of the part (machine 0) is .015 away from the tool. Z+ Z- <- -> Calling G0Z0 would then move the stock that .015 to make the shifted grid 0 be the same as the machine 0 thereby having the stock actually stick out .015 past the edge of the tool. Doing a facing operation at Z0 would face .015 off the end of the part and establish the end of the part at machine 0. The G0Z-.05 call moves the stock .050 away from the tool to allow for the tool to be retracted. If I were to do a G50Z.015 (positive direction) shift, and then subsequently doing a G0Z0 call, the stock would actually retract .015 away from the tool and establish machine 0 as .015 AWAY from the tool (in space). Correct?

YES!! Just remember that you can set a G50 (Coordinate Zero Anywhere in the Stroke of an Axis)

In theory you can set the A or B Axis Gang Slides for End Mills, Drills etc. If you do not want to use the Offset or Geometry Machine Positions.
You can do this when doubling and tripling operations using the same tool.

[tobyaxis]

Oh, also remember that it is the Bar Stock your Moving in the Z Axis not a Turret, unless your using one of the newer configurations. They have the Turrets I wanted, but the Boss didn't want to spend the extra $$$.

[HSPMInc]

Originally Posted by cogsman1 The G50 in THAT case is defining where the STOCK is as you start the program. There is a "theoretical" ZERO in your machine, the location of the the tool holder in the gang tool plate, and the cutoff tool you have in the machine has an insert that has an edge closer to the guide bushing by .010". You also need to have some material to face off, usually .005", so that is where the -.015" comes from. Now after this is read you will retract the cutoff tool and call the face tool into position. When you command "G0Z0" the stock will move OUT that .015" there by giving you .005" to remove during the facing operation. You should also note that at the END of the program after the cutoff you will see a line of code that sends the Main spindle BACK to that position WITH THE COLLET OPEN, "M6", "G0Z-.015". This is how you are able to run bar stock.

Why would you G50 the whole program for the part-off width? Why not Just G50 the part off tool.

For instance

T100
G50 W-.01

cutoff

G50 W.01
M99

[cogsman1]

When you first turn on the machine the "work coordinate" for the "Z" axis would be some huge number like -8.4567 so when you start the cycle and tell the stock to go to "0" it would shoot out 8.4567. You MUST define your starting location which is different depending on the cutoff tool that is in front of the stock at starting.
FYI, the "G50" does NOT move anything just changes the work coordinate system numbers.

[HSPMInc]

Originally Posted by cogsman1 When you first turn on the machine the "work coordinate" for the "Z" axis would be some huge number like -8.4567 so when you start the cycle and tell the stock to go to "0" it would shoot out 8.4567. You MUST define your starting location which is different depending on the cutoff tool that is in front of the stock at starting. FYI, the "G50" does NOT move anything just changes the work coordinate system numbers.

understood. So then just put a G121 or a G50Z0 in your header.