G96 & G97 on lathe.

[AMCNitro]

I've been programming lathes for abut 10 years, so I feel stupid asking this, but here it goes...

I've only programmed Haas lathes and I've always gotten the following code:

 

G97 S881 M03

G0 G54 X.867 Z.01

G50 S1600

G96 S200

 

 

I know what the G50 and and G97 are(or do), but I've never been sure about what the G96 does.  I've always just gotten it to work to my liking by messing with the 3 numbers, but can anyone tell me exactly what changes when the G96 changes?

 

Thanks.

[Guest]

Constant surface Speed

 

If you set your CSS at 400 SFM say.......you will get a speed that will match at whatever diameter you are cutting up to your G50 mas spindle speed

[The Cathedral]

I made a video a while ago to explain CSS. I use it when I teach a class on the basic principles of machining. It's meant to be played in the background as I stop and verbally explain the concept, but there is enough wording to give someone a good idea. Check it out if you want. 

 

[Reko]

Nice video Cathedral.

 

<out of likes>

[slyym]

How does someone who's been programming for 10 years not know what constant surface speed is?

[Mike@Lustre]

reality is trades are filled with skilled people who don't know every aspect or code , some programmers never set-up or run a machine so all the codes are just letters and numbers they see on a screen .

[AMCNitro]

How does someone who's been programming for 10 years not know what constant surface speed is?

I know what it is, and I have always understood the concept.  I just wasnt sure what G96 did.  Theres a difference, dont put words in my mouth. 

[AMCNitro]

reality is trades are filled with skilled people who don't know every aspect or code , some programmers never set-up or run a machine so all the codes are just letters and numbers they see on a screen .

I started making molds with my dad in the mid 90s.  I started with manual machines, my 1st CNC was a bridgeport Series 2 with a Hidenhein TNC 145.  I had my own shop after that for 6 years, went to work for other shops for the last 4 years and now Im back on my own again.  The 1st time I programmed a lathe was when I started my own shop in 05, before that I had never programmed a lathe.  So I know how to setup, run and program...

 

I find it peculiar that someone asks a question and suddenly his knowledge is questioned, as if everybody here knows everything and was born knowing..smh...

 

Thanks JParis and Cathedral, we need more people like you guys.

[slyym]

I started making molds with my dad in the mid 90s.  I started with manual machines, my 1st CNC was a bridgeport Series 2 with a Hidenhein TNC 145.  I had my own shop after that for 6 years, went to work for other shops for the last 4 years and now Im back on my own again.  The 1st time I programmed a lathe was when I started my own shop in 05, before that I had never programmed a lathe.  So I know how to setup, run and program...

 

I find it peculiar that someone asks a question and suddenly his knowledge is questioned, as if everybody here knows everything and was born knowing..smh...

 

Thanks JParis and Cathedral, we need more people like you guys.

Sorry. Guess my question can be taken a few different ways. Wasn't trying to take a shot at you. Guess we're all different and learn things at different times.

[Mike@Lustre]

I started making molds with my dad in the mid 90s.  I started with manual machines, my 1st CNC was a bridgeport Series 2 with a Hidenhein TNC 145.  I had my own shop after that for 6 years, went to work for other shops for the last 4 years and now Im back on my own again.  The 1st time I programmed a lathe was when I started my own shop in 05, before that I had never programmed a lathe.  So I know how to setup, run and program...

 

I find it peculiar that someone asks a question and suddenly his knowledge is questioned, as if everybody here knows everything and was born knowing..smh...

 

Thanks JParis and Cathedral, we need more people like you guys.

It was not a jab at  your skill level , just pointing out that there are lots of highly skilled guys who don't know everything about what they are doing , not a negative thing just a fact about today  .

 

I run and set-up twin spindle turning centers , and have only been in the CNC end of things fulltime for 2+ yrs , prior to that(25+yrs) I was a manual guy in a jobbing shop bouncing from machine to machine getting stuff done .

 

Last shop I was working at, had guys that could draw , program and set-up machines yet had no skills on trimming the fat off a program and making the most out of it .

[Roger]

G96 (constant surface speed control) according to the list of G codes.  Meaning the lathe RPM will correspond to the diameter the tool is at, up to the max RPM which you programed (G50).

 

885 SFM X 3.82 / DIAMETER =RPM @ THAT DIAMETER (G97)

 

Is this helpful?

[AMCNitro]

G96 (constant surface speed control) according to the list of G codes.  Meaning the lathe RPM will correspond to the diameter the tool is at, up to the max RPM which you programed (G50).

 

885 SFM X 3.82 / DIAMETER =RPM @ THAT DIAMETER (G97)

 

Is this helpful?

That helps, but it makes me realize that I should also have asked about the G97.  MC asks for a Spindle Speed, which it uses as G96 and a Max Spindle Speed, which it uses as G50.  My next question is, how does it determine G97?  ANd what does G97 control?  

Is it correct for me to assume that G97 is the starting RPM?

[Reko]

That helps, but it makes me realize that I should also have asked about the G97.  MC asks for a Spindle Speed, which it uses as G96 and a Max Spindle Speed, which it uses as G50.  My next question is, how does it determine G97?  ANd what does G97 control?  

Is it correct for me to assume that G97 is the starting RPM?

G96 and G97 are modal... you can only be in one mode or the other.

 

G97 is just a direct RPM... the spindle never changes RPM when in this mode.

 

The formula for figuring RPM is:

 

            SFM x 3.82

RPM=  ---------------

              Diameter

 

So... say you are programming 6" Diameter... you want to rapid to safe distance away... say... X6.1 Z0.1

 

If you program G96 S400 ...when you look at your actual spindle speed when your tool arrives at X6.1 the spindle speed will be 250 RPM's

 

because:

 

            400 x 3.82

RPM=  ---------------  = 250

                 6.1

 

 

Now, you could program G97 S250 ...and you get the same result at X6.1 Z0.1 ...an actual spindle speed of 250 RPM's

 

The difference is when you are roughing and changing diameters:

-in G97 mode... the spindle STAYS at an actual spindle speed of S250 RPM's

-in G96 mode... the spindle speeds up the RPM as it gets closer to X0 (staying at the proper SFM)

 

Now, a typical post processor might be designed to kick out a G97 S250 first... and then when it arrives at X6.1 Z0.1 it will change over to G96 S400... that way you don't get the radical speed change when it rapids from home position to X6.1

 

JM2C

[The Cathedral]

G97 is a constant, unchanging RPM. You can use G97 and have the RPM stay the same, no matter what the cutting diameter. Think of facing: if you use G97 S1500, the rpm will be 1500 as it starts the cut at the OD, will be 1500 as it moves down, and will be 1500 as it moves to X0. No matter what, it's 1500. 

 

When you use G96, it changes. It will be slow at the OD, and as it moves closer to X0, it will speed up until it hits the max spindle speed. G50 sets the max speed, and that's important because, as the cutting tool gets closer to X0, it theoretically has to spin up to a bajillion RPMS in order to keep the constant surface speed you program. So G50 keeps the machine from spinning too fast for safe cutting conditions.

 

However, when you program to use G96 in Mastercam, you will see an initial G97 move at the toolchange. This is put there because if you were to start in G96 mode, while your turret is in home position, the spindle would have to start spinning at 1 RPM or so. Having your spindle constant ramp up to max then down to 1, then up and down again isn't really the best practice. So it kicks out a steady RPM at the beginning. This RPM is calculated using the formula listed above, using your cutting start point as the diameter. That's why it's such a random number (like 1137 RPM). Once it gets into position and G96 kicks on, you shouldn't see any spindle speed fluctuation and it will go right into the cut at the appropriate speed.

 

G96 and G97 are mutually exclusive: you can only use one or the other, never both at the same time.

[jlw™]

Me thinks from your other posts that you are more than capable of "getting" G96/G97 and you're over-thinking.

 

Make 2 simple programs and go watch it run, soon as you see the 2nd program run you'll have that "aha" moment I guarantee!

[AMCNitro]

Me thinks from your other posts that you are more than capable of "getting" G96/G97 and you're over-thinking.

 

Make 2 simple programs and go watch it run, soon as you see the 2nd program run you'll have that "aha" moment I guarantee!

You're correct.  I know what it does, and why.  I wasn't clear on what to change, I thought that changing G97 had an effect on the way it works.  Now, thanks to all the people that answered my question, I have a much better understanding of what to change.

 

Thank you!