G50 and Zero Return

[apprentice]

Hi, everybody,

 

Could any of you please tell me what is G50 about??

 

Also, what is Zero Return?? Is this equal to G28??

 

Much Thanks.

[lathe guy]

i assume you are talking about a lathe. g50 is normally called before using constant surface feet.

ie:

g50 s2000 = 2000 max rpm

g96 s500 = 500 surface feet

 

on some fanuc g50 can give unexpected results, like movement of x or z axis. something like a reference retrn. dont remember its been a long time.

[Guest]

On many controls G50 is used to clamp the maximum RPM.

 

G50 S2000 as shown by lathe guy will clamp the machine top speed at 2000 RPM, unless it is changed again within a program.

 

On the YASNAC controls that I am familiar with, LX3 and LX5, the G50 can also be used as a reference position. You have to set it on the work offest page if you do not and call it out in a program without an S on the same line BAAAAD things will happen.

 

As far as I know a G28 without a G91 will simply returm to the programmed zero position. If you wish to send it to machine zero you must use a G91 on the same line.

 

G91 G28 Z0

 

Hope some of this helps you

[Storkman]

Oh yes, I once forgot the G91 when I was writing a manual program and tore the vise right off the 4th axis. I didn't think that Fadal had that much power. I was wrong, took a day to set it back up. Made a mental note on that one.

[LNDCAD]

Zero Return - "Homes" the machine (X, Y, Z axes). On HMC - this is usually the pallet change position. On VMC's and Turning Centers, this is machine home (usually all axes at a maximum travel position).

G28 will send a machine home, but it must be used along with other commands or the results can be disastrous.

G28 X0 Y0 Z0 - sends the machine home in the XYZ directions after FIRST moving TO the point X0, Y0, and Z0. If Z zero is the face of the fixture or chuck, the tool can be driven through the part before returning home. X0/Y0/Z0 does not cause the tool to move home, this is a point to move through prior to going home.

G91 G28 X0 Y0 Z0 - puts the machine into incremental / relative which tells the machine to first move zero in the X Y and Z direction and then go home. This zero incremental move will not crash, it just causes the tool to go directly home (the X0,Y0,Z0 is used to tell the machine which axis should be homed - a G91 G28 Z0 would ONLY home the Z axis). Turning centers often use G28 U0 W0 to send the X and Z axis home after an incremental zero move. On a HMC or VMC, G53 G28 X0 Y0 Z0 is used to send the axes directly home by using the Machine Coordinate System to tell the machine to move home after first going through the point X0 Y0 Z0 measured from the Machine Zero (Home). Finally, the G50 command is used to both clamp the maximum spindle speed on a turning center when using Constant Surface Speed, or to set the current position display. G50 S2000 clamps the maximum spindle speed at 2000 rpm. G50 X1.0 Z2.0 sets the current display to show X1.000 Z2.000. This is the same as the G92 command on some controllers (FANUC). Sorry this got so long, but it is critical that you understand this command - it can quickly CRASH. HTH

[apprentice]

Hi, Lndcad,

 

I am confused. Why when I use G28 on Haas and the spindle sent home right the way? Does that mean on that particular machine the G28 comes with G91 G28 X0 Y0 Z0 feature?? Please advice.

[MCam Newbie]

Just a G28Z0 can home the Z axis, if no Z has been set after a movement from Z home, with a G92Z(value),

because machine home is the only reference zero for Z. Z is usually brought to program, or part Z0 using and offset extention, which does not actually set a Z value in the coordinate system, because the head position will vary with each tool loaded. The offset changes the head level for each tool in turn.

Part zero for X and Y axis IS set by a value X Y distance from machine home to part zero. This position is constant (for all practical discussion, though multiple coordinate systems are frequiently used, each one will have a fixed absoute zero defined referenced to machine home from part, or program zero.

That is why, on X and Y a G28X0Y0 in G90 mode will first go to the defined part zerp,or absolute zero THEN continue on to MAchine Zero.

However, a G91G28X0Y0, puts the control in incremental mode, G00X0Y0 would not move an axis. Incremental by definition only sees distance and direction of a command, therefore has no consideration of absolute zero point.

G91G28X0Y0 = Incremental return to Reference Zero Machine Home, on the axis specified. The only reference zero IS Machine Zero. Axis goes straight home.

G90 moves references to a user set program(part) zero, and positions to that "Absolute Reference Zero" then finishes the requirement of G28 to MAchine home.

I hope this clears things up a bit, I am sure I repeated myself somehow, but even if my explanation isn't exactly correct from a systems standpoint, the concept presented is a valid explanation of what occurrs at the machine, in my experience.

**********************************************

Lathe Stuff

A G50XxxxZxxxSxxx, = Absolute Preset for the tool tip on a lathe, and sets max. spindle speed.

 

Say you start all you tools on your lathe with X and Z at Machine Home, or Zero Return position.

You index a tool into position, then before machining with it, a G50 command line sets the absolute zero at centerline of the spindle for X, and usualy the part face for Z. This is Part Zero.

If when at machine home, your G50 might be X8.0Z5.0. If you had stock in the chuck large enough, and moved X facing the part, you would find the cut face to be 5 inches away from the programed Z0 on the part. If you did not move X, and instead turned by moving Z axis, you would turn a 8.0 diameter. So a G50 presets the distance from where the tool tip is, distance and direction, from the centerline and end of your workpiece.

Gonna go to sleep now, everything is blurry, mu two typing fingers are raw. Spelling may be a victim to the blurr .... and finger spasms ....hope it is not too bad.

[MCam Newbie]

Oh, almost forgot, G28U0W0 is the same as G91G28 on a mill. U and W are incremental mode for X and Z. There is no G code for incremental, absolute. The axis character does the deed.

Way nuff said. Nighty night. Still dark, anyway ....

[tryon]

i wish incremental was as easy/obvious on a mill as it is on a lathe...

[Jack Mitchell]

Hey apprentice,

 

On a Fanuc 6T, G50 has other functions as well.

Which lathe control are you using?

I don't want to disclose and confuse unless I absolutly have to.

 

Regards, Jack

[LNDCAD]

Sorry I did not get back an answser sooner - I have been out of the office on a job (working split 3rd - 1st shift times) and only have a slow dialup internet access in my room. Work at night and sleep during the day. MCAM Newbie explained it better than I did. Any other questions, I will try to get back to you sooner. HTH

[apprentice]

Hi, everybody,

 

First of all, Thanks for all your help. it is a big help for me. Thanks again.

 

I use Mori Seikei machine with Fanuc control. Machine is about 15 years old.

 

Question: just yesterday.... bad thing happened... I cleaned one tool then hit "cycle start". However, I noticed the piece was about 1/4" shorter. The subsequent piece was short by that amount. I didn't use the MDI to write the command. However, I make sure the light on the X and Z light up before I Reset the Program. This is dangeous. Can any of you please tell me what went wrong?? Thanks

[Brendan P]

You have to be a little more specefic.

I'm going to have to use my psychic energy and guess that your part keeps coming out shorter and shorter. Right?

When something like this happens,the first thing I would check,is to make shure at the end of each tool,you are cancelling any X or Z offset.

Otherwise,it will start to multiply and your parts will keep changing in size.

 

This is done on your Mori like this:

 

Say you are using tool# 1

Then you need to put a line in after the tool goes home:

I/E

 

X-10.538 Z5.269 (tool goes home G50#)

T0100 (00 cancels out any offset)

M30 (program rewind)

%

 

quote:

---

However, I make sure the light on the X and Z light up before I Reset the Program.

---

You should have an M30 at the end of your program.

It sounds to me like you are re-setting it yourself.

Again I am just using my psychic powers and quessing.....

 

Good luck

[Charlie Pierson]

On the Fanucs we have here , G28 is a 2 step command , roughly translated , it says "Go Home but 1st go here, then go home. If executed in single block , it will take 2 presses of the start button to finish the command.

 

The crash problems come from using G28 when the control is in Absolute (G90).

G90G28Z0 says to rapid to Z0 in whatever coordinate system you are in , then rapid home.

 

The safe way is to use G91G28Z0 (incremental) which tells the machine "go nowhere, then go home"

 

Aside from "G50" being used for setting max rpm in CSS on lathes , G50 acts like a G92 and can shift your work coordinate system. Some of us here use it to shift grooving tool the thickness of the insert so's that the program coordinates match up to the print. "G50W-.125" for a 1/8 wide insert. Just gotta be careful to "G50W.125" when your done using it or the rest of the part will be in error .125 in Z.

cp