I'm new to running a turning center style cnc lathe with a turret, my question is, if I touch off all the tools to the part do I need to set a work shift? What exactly and how does the work shift work? I'm having trouble understanding how the tools, work shift and program correspond with each other. I understand why and how the tools need to be touched off, but what exactly does the work shift do? I touch all my tools off set my zeros and then set my work shift and my tools are are over the place in the z axis, x axis is good. It's always the z axis that is out. Any help would be much appreciated.
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
setting up turning center tools
- Thread starter gehodgin3
- Start date
- Replies 27
- Views 5,358
EmGo
Diamond
- Joined
- Apr 14, 2018
Work shift ? wtf is that ? Try tool offsets.
Programs are written for a tool that is in a certain place. In the real world, the tool is seldom in that actual place. They used to have to be - the turret was removed and tools set up on a fixture or surface plate, in case you are curious.
Then the builders figured out that you could add or subtract numbers from where the tool was supposed to be, to where the tool really was. That's tool offsets.
And that's all there is to it.
I dont know how the new work shifts work on newer machines. so I am assuming they all work the same.
My lathes I use work shift so I dont have to reset tools again off the part.
for example all tools offsets are set off the face of my part, so that means Z0 is set.
now lets say I run another part I call up tool 1 touch the face of my part and use shift work offset to call that Z0 . I dont have to reset my tool offsets(unless I put new tools in).
Basically its keeps you from setting you tool offsets on every new part. On a 2 axis lathe you dont need to worry about the x workshift offset.
Again thats how I do it for the older machines fanuc and yasnac controls
My lathes I use work shift so I dont have to reset tools again off the part.
for example all tools offsets are set off the face of my part, so that means Z0 is set.
now lets say I run another part I call up tool 1 touch the face of my part and use shift work offset to call that Z0 . I dont have to reset my tool offsets(unless I put new tools in).
Basically its keeps you from setting you tool offsets on every new part. On a 2 axis lathe you dont need to worry about the x workshift offset.
Again thats how I do it for the older machines fanuc and yasnac controls
Kallam
Cast Iron
- Joined
- Feb 11, 2006
- Location
- South Carolina
some people use for a lack of a better word g54 for a home ( haas uses a g54. my kia call it cordanance shift if I remember correctly) and use the cut face on tool number 1 as Z zero. the benefit of doing this is that if you have a short piece of material you can shift all your tools with 1 adjustment. some people just do the individual tools by themselves. I was taught the first way due to I worked in a large quantity production company. it also comes in handy if you have a probe, because you need to know the difference between your touch off of ur probe, and the face of your part.
First thing first... what machine is it and what control? Narrow this down and you'll get more precise answers to your exact question because everyone sets their tools differently. it's user preference.
EmGo
Diamond
- Joined
- Apr 14, 2018
Shee-it. You guys never heard of G92 ?
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
All of us that have been around for more than 5 minutes know about G92. But we've all moved on where the control has Work Offset Coordinate System programming available.
G92 is the alternative to G50 used for setting the Work Coordinate System; The overwhelming number of Lathe Controls use G50, with G92 predominately used with Machining Centre controls. Fanuc controls can select the G Code System that uses either G50, or G92 for Coordinate System setting via parameter; the default is G Code System A that uses G50.
rick-b
Aluminum
- Joined
- Jan 1, 2013
- Location
- Queensland
OK, tell me more about using G92. I have a lathe that seams to use it in place of G50.
If G50 is G-Code system A what system is G92?
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
Hello Rick,
If your control is a Fanuc, then G Code System B and C (settable via parameter) use G92 instead of G50 to set the Work Coordinate System and Clamp the Maximum Spindle RPM when using Constant Surface Speed control.
If the Control has Workshift Offset Programming available, its a big backward step to be using G50. or G92 to set the Work Coordinate System. With controls that have Workshift Offsets available and a Measure Function (such as many Fanuc Controls at the discretion of the MTB), its normally the Common Workshift Offset (G52) that is set via the Measure Function. Any value that is set in G52 is applied (added) to all other Workshift Offsets. As apposed to a Machining Centre. its rather uncommon to use numerous Workshift Offsets in the one program, unless there is a repeat of a feature, using a lot of code, at numerous locations along the shaft. But even then, there are other ways around that scenario than using multiple Workshift Offsets. Therefore, when shifting from one job to another, only the Z value for G52 needs to be set. This can be set by a Measure Function (if the machine is so equipped), by G10 from within the program, or by a Custom Macro to mimic the Measure Function that is supplied with many machines.
Regards,
Bill
angelw
Correct me if I am wrong but using a g50 on lathes that home to the extents of there travel away from the chuck is more of a pain in the butt than a lathe that homes to the (closest to the chuck) front of its z travel
for example on most lathes a g50 you use after sending your machine HOME away from your chuck,
My citizen z home position is closest to the chuck. so when I have lets say a 1" long part I just jog out to z1.1 type in G50z0.0 input then cycle start.(added .100 extra so it doesnt bump home switch)
on the normal lathes you just need to do a little math to get the same effect from the part 0
Whats nice about g50 on my citizen is all I need is a OAL of the part plus some extra and I dont have to do any math.,
Does that make sense? I am curious how others with older citizens and funac controls set there machines up was teh reason I am asking.
Thanks
Correct me if I am wrong but using a g50 on lathes that home to the extents of there travel away from the chuck is more of a pain in the butt than a lathe that homes to the (closest to the chuck) front of its z travel
for example on most lathes a g50 you use after sending your machine HOME away from your chuck,
My citizen z home position is closest to the chuck. so when I have lets say a 1" long part I just jog out to z1.1 type in G50z0.0 input then cycle start.(added .100 extra so it doesnt bump home switch)
on the normal lathes you just need to do a little math to get the same effect from the part 0
Whats nice about g50 on my citizen is all I need is a OAL of the part plus some extra and I dont have to do any math.,
Does that make sense? I am curious how others with older citizens and funac controls set there machines up was teh reason I am asking.
Thanks
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
Hello Delw,
Its not much, if any more difficult if the Reference Return Position is in the plus direction from the chuck. If the G50 is to be made at the Reference Return position:
1. Perform a Reference Return
2. Set the Relative Display in Z to Zero
3. Move the Setting Tool to the Z Zero of the Workpiece.
4. The G50 will be the Absolute Value (+ value) of the negative value displayed.
However, having the Reference Return at the Negative Extreme of the Z Travel will be harder to crash the machine if the G50 is executed when the axis slide is in the wrong position. For example, it would be less probable that the G50 will inadvertently be executed with the tool in a negative position from the workpiece Z Zero, when the Reference Return Position is in the Negative direction.
Regards,
Bill
Ox
Diamond
- Joined
- Aug 27, 2002
- Location
- Northwest Ohio
I have posted this a few times, but since you are asking:
I was taught by Hardinge when I bought my first lathe and my first Fanuc to use G10 in the program header to activate the WORKSHIFT.
I love it, and hate to go to other machines that I need to use G54.
If your machine has G10 capability, you just put in your header:
G10 P0 X0 Z-(whatever)
For starters, you wunna run a tool set-up run through MDI, so:
G10 P0 X0 Z0
That makes sure that your WORKSHIFT is set to zero.
Now set your tools to the surface of your chuck, collet, or ......
Now - in your case - you want to set your G50 @ 1.1", in this case, you would just put:
G10 P0 X0 Z-1.1
in your header, and when it reads it - it will update your WORKSHIFT file automatically. (is that G53 maybe? I don't need to get into the offset files, so ...)
While I like to not have to worry about editing the G53 (?) each time, a couple more benefits to using this as opposed to G50 or G54 are:
A) If your G10 line is near the top of your program, you can always see it on the CRT.
So - if you forget how far to stick your bar out - all you doo is look at that line, and you know for sure.
B) When touching off new tools to your faced off surface, WORKSHIFT keeps the Z values up all the time, unlike losing your G54 when you hit RESET.
This way you don't need to subtract the G54 value when updating the OFFSET register. (Not a G50 issue, but is for G54)
This is an even bigger issue when you have dual paths or subspindles, as when you come back to the program, it's all there and ready.
If you were to G50 1/2" off this time from the last, it could mess up your subspindle actions at times, so ...
-------------------
Think Snow Eh!
Ox
Booze Daily
Titanium
- Joined
- Sep 18, 2015
- Location
- Ohio
I do exactly what Bill mentioned on my Okuma. I used to do the whole touch off the face of the part thing but I wanted something similar to setting tools on the machining centers.
Specifically:
I touch the face of the turret on a 1-2-3 block off the face of the chuck. This is the program zero.
I set it in the control and it never changes.
Then touch all the tools off the 1-2-3 block. This will give all +Z offsets.("gage length method" on MC's) Easy to double check with a scale.
Caliper from the face of the stock to the 1-2-3 block and shift that amount.
Specifically:
I touch the face of the turret on a 1-2-3 block off the face of the chuck. This is the program zero.
I set it in the control and it never changes.
Then touch all the tools off the 1-2-3 block. This will give all +Z offsets.("gage length method" on MC's) Easy to double check with a scale.
Caliper from the face of the stock to the 1-2-3 block and shift that amount.
Mike1974
Diamond
- Joined
- Nov 5, 2014
- Location
- Tampa area
I think everything has been covered. Just wanted to comment that it is interesting all the ways mentioned. So I guess it is as much personal preference as right/wrong.
Sidenote, get a lathe with a toolsetter and you're all done.
Sidenote, get a lathe with a toolsetter and you're all done.
rick-b
Aluminum
- Joined
- Jan 1, 2013
- Location
- Queensland
It's funny, I never found the VMC as hard to learn to use as the lathe has been.
Kallam
Cast Iron
- Joined
- Feb 11, 2006
- Location
- South Carolina
I bet this guy is very confused now.
EmGo
Diamond
- Joined
- Apr 14, 2018
If all you know is Fanuc, I guess so. But if you want to talk real controls, G92 is just as common with lathes as it is with machining centers. And it's more basic and reliable. There's not really any need to add more and more and more crap on top of something that works fine. KISS.
Vancbiker
Diamond
- Joined
- Jan 5, 2014
- Location
- Vancouver, WA. USA
Mistakes in using G50 and G92 are probably the #1 cause of crashes or scrap parts on machines that do not have work coordinate offset capability.
That's normal. It's called Machine Shop "Maturity". Puberty is like using a VMC, growing up is using Turning Centres, Maturity is running multi axis Turning Centres, and old age is the same hopefully--not doing shit until I want to.
R
