G-Wizard Calculator:
Fast, Easy, Reliable Feeds and Speeds


Join 100,000+ CNC'ers!  Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:

  • Our Big List of over 200 CNC Tips and Techniques
  • Our Free GCode Programming Basics Course
  • And more!


GCode is Complicated
G-Wizard Makes it Easy

G75 and Peck Parting Off For Lathes

Feb 17, 2016   //   by Bob Warfield   //   Beginner, Blog, GCode, Techniques  //  7 Comments

PartingOffFor whatever reason, parting off seems to be the operation on lathes that causes the most people trouble.  Perhaps deep boring operations where the bar is really hung out there is a close second.

Parting off is definitely a challenging operation when you look at it mechanically.  You’re going to take a fairly tiny cutter and plunge it deep into the material.  That cutter has to be hung out quite a ways relative to its width, although we do have the luxury that the parting blade under the tip is fairly substantial.  If you lathe is lightweight, this just means lots of strong lever to try to make the whole thing flex downward and potentially dig in.  The geometry is such that parting tools seem to be more sensitive than many others about how they’re set up relative to the lathe’s centerline.  Get it too far off and it’ll tell you in a hurry.  Once the tool tip is deep down in the parting groove of the material, getting chips out and lubrication in becomes problematic as well.  Lastly, parting seems tailor made for generating chatter, which brings a whole other set of problems into play.

Beginners are advised to feed hard, although their inclination is to take it easy and back off with every squeak and squawk they hear.  What a mess!

It takes some experience, a good parting tool that is well set up, and a lathe with good rigidity to make parting any easier, but sometimes even more is needed, particularly in CNC applications where the “touch” of manual machining is absent.  Enter the idea of “Peck Parting”.

Most machinists will be familiar with peck drilling cycles where the drill bit is retracted a little to break a chip or a lot to help extract chips from a deep hole over and over again as it makes its way down the hole.  Turns out we can benefit from the same sort of thing when parting off.  We shouldn’t be surprised–the groove width to depth ratios are not unlike the twist drill diameter to depth ratios that cause us to need peck cycles there too.

Many controls have a peck option on the G75 grooving code, which is also used for parting off.  If the control has a conversational CNC mode, it will often have a “parting off with peck” option as well.

How and When to Use Peck Parting Off

In terms of the “when”, it’s all about the chips.

If you’re getting long stringy chips and bird nesting while parting off, try the peck cycle.  In this case, you just want to back off every so often to break the chip.  Backing off 0.002″ or so should do it.  If you don’t have a parting off or grooving cycle that does peck,  you’ll have to hand code it.  If you’re hand coding, try pulling back 0.002″ and dwelling for 2 revolutions to make sure the chip is broken.

If the problem is that the chips are breaking properly, but they’re really piling up (one more argument for slant bed lathes, eh?), you may have to retract further to provide some clearance for the chips to drop through and the coolant to flush the area out.  Unlike peck drilling, where you don’t want to retract clear of the hole and wash chips back down the hole, the only detriment when parting to too much retraction is that it will slow you down.

Typically, you won’t have these problems unless you get to parting larger diameters, but they’re common at some point to everyone.

A good recommendation when parting is to slow way down and turn off CSS as you get very close to the middle.  Slowing down will reduce the likelihood of the part flying around inside the machine when it finally breaks loose.  You can even do the last little bit of parting as a G01 move without bothering with a cycle of any kind.  Alternatively, some machinists will just set a G50 spindle clamp of around 1000 rpm.  It really depends on the material’s requirements though.  You may well want to be going a lot faster than 1000 rpm up until you’re close to being done parting.

Fanuc’s G75 in newer controls uses a two-line format:

G75 R0.002
G75 X1.0 P0.125 F10

R is the amount of retraction after each peck.

(X1.0, Z-10.0) is the lower left corner of the groove.  That’s assuming that the lower left corner of the grooving tool is its reference point, and the grooving is being done from right to left.

P is the depth of cut for each peck at a feedrate of F.  So, each peck cuts a distance of P, retracts a distance of R, then re-engages the material and does another peck of distance P.  This cycle continues until the bottom is reach, and the last peck is often less than a full P depth.  When the cycle completes, the tool retracts to the X value that was present when the G75 cycle began.

Now here is a nifty trick.  If you specify a Q value and a Z value, it means you want a groove wider than the tool width (Q), which runs from the starting Z position when the cycle is entered to the ending Z specified in the cycle.

One warning about all this:  Peter Smid says it doesn’t produce precision grooves, so it probably shouldn’t be used where there are tight tolerances.

There is also a one line version on many controls, which won’t allow you to specify as many parameters.  For example, an “R” on the second line is used to describe how much relief to leave for the tool on the final cut, perhaps so you can slow down the spindle before cutting the last little bit.  In a one line format, you only get one “R” and it is used to specify the peck retract amount.

Make Peck Parting Super-Easy With Conversational CNC

If you don’t want to bother learning and remembering how to use G75 for peck parting, or if your machine doesn’t have G75, it’s can still be very easy to set up for peck parting.  The easiest way I know is to use a Conversational CNC capability like G-Wizard Editor’s to do the programming for you.  Here is what the screen looks like in G-Wizard Editor:


It’s easy to set up peck parting in a Conversational CNC program like G-Wizard Editor…

I’ve circled the peck option in red.  There’s a “Peck Z” parameter block to the right that gives you full control.  Peck Z determines how far to cut in Z before pecking.  Retract is how much to retract–just a little will break the chip.  And Dwell is how long to wait while retracted to give the chips a chance to be carried away.  Very simple and straightforward.

The Conversational CNC function programs a complete peck cycle.  There’s even an option for a finish allowance and a slowdown at the end so the part will fall of nice and easy and not be flung into the enclosure wall, possibly dinging up your part.

If you’ve never tried Conversational CNC or G-Wizard Editor, give them a try with our Free 30-day Trial.  You’ll find a ton of useful functions there.


Like what you read on CNCCookbook?

Join 100,000+ CNC'ers!  Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:

  • Our Big List of over 200 CNC Tips and Techniques
  • Our Free GCode Programming Basics Course
  • And more!

Just enter your name and email address below:

Full Name
Email *
100% Privacy: We will never Spam you!

G75 and Peck Parting Off For Lathes
Rate this post


  • Hi Bob, If I can offer a couple of guaranteed aids to parting. Forget about those old HSS blades, they are a pain in the bum. Change to the ISCAR pattern small insert tip and blade with custom holder. Set the overhang to be adequate, and go for it! Those inserts are black magic and witchcraft combined! I had a tool rep in the shop some 34 years ago, prattling about these fantastic miracle tools, so I said, lets prove it! Well, after one and a half mild steel bar, then a two inch 4140, a 2 inch brass bar, and a two inch Aluminium alloy bar all had slices taken off f them, and at higher speeds and feeds than I would have dared, and a cut off in 4140 under feed;

    left me open mouthed, and telling him that it was staying in my lathe! One tip geometry did everything, which still blows me away. They need to run wet though, but not at supersonic speed. The critical thing is that they form and swage the width of the chip down somewhat and just slice through like a knife through butter. For what it is worth, I have parted numerous blanks of Aluminium up to 6 inch diameter without any great dramas. I am talking about my Colchester Triumph 7.5 inch center height lathe. To cut big bars up, you need to do a few things differently. A deep center in the opposite end of bar, and the three point roller steady up near the cut off area, but more to contain the bar from going wacko when it cuts off.

    The secret lies in being as close to the chuck as possible, and not running overly fast,, and keeping the coolant flowing. I have cut many quite long bars into short pieces without any problem. You can stop before getting under say 3/8″ or a bit less, and hacksaw if nervous. The bar will just stop revolving when it parts off. Do not have high pressure on the center preferably a live center. When doing large diameters, you need to do it in several stages, and do a cut that is fairly wide to allow additional chip clearance. It can be exciting if the swarf jams down the side of a well extended blade! With big bars, I tend to do maybe a double width cut down to about half diameter or a bit more, then cut in the center, which gives clearance on each side. Yes, it sounds dramatic, but I was shown this trick over twenty years ago by a man who I have the greatest respect for, and was amazed just how easy it made the virtually impossible. Another good dodge is to mount the tool upside down in a rear holder if you have one, and use gravity to assist with clearing the chips out. It also pulls the spindle down into the solid part of the headstock, and is normal practice on a capstan lathe.

    I have never regretted buying that magic formed insert parting tool all those years ago, and have NEVER had any of those oh so frequent troubles since. One of the other problems is that most parting tools have zero back rake, and that also increases cutting forces.
    On the CNC lathe we usually work with pre sawn billets rather than part in the machine. I have done a few specials, by judicious use of the hand-wheel and electronically hand feeding the tool. I think it is likely that parting some jobs on a CNC is likely to be a source of more problems than it is worth, unless you are running a large quantity and truly optimise the process to the material, the tool and the machine.

    Bob, this is one of the problems with many CNC machinists; they have not had near enough if any manual center lathe and even capstan lathe work, which is the greatest way to learn about the incantations and magic that occurs at the cutting tool edge and workpiece interface. The skilled manual man has a great advantage when it comes to optimising the speeds and feeds listening to the action, and knowing how it is really performing. The same on a machining center. The CNC can beat the human ten to one in normal operations, sand repeatable accurate work, but it lacks the nouse of the human, because the machine lacks two ears with a brain between them, and two eyes to observe what is happening.

    But for trouble free parting, just try one of those magic formed cutoff inserts, and ponder on how it works for so many different metals. It seems that many tip makers have them these days. They may seem expensive to buy but they are worth every cent.

    • Stephen, thank you for the tips. I also like my insertable parting tool. It uses the GTN inserts. Sometimes I will use an HSS blade. When I do, I find it is often helpful to just dish the top to create a little positive rake there. Makes for happier parting with many materials, especially brass and aluminum.

      If you can feed bar at all in your CNC lathe, you’re going to find parting is essential. There’s a lot of sneaky things you can do with a good parting tool as well. More on that in a future post.



  • Hi Bob. Parting off is surely a touchy issue for some. HSS blades are great for smaller lathes and hobby type machines. One of the main problems is centre height AND squareness. The squareness issue is because there is no clearance behind the cutting edge (front to back). If you are off square then the result may be that you get some deflection which leads to the back face of your component not being flat. That would apply if you are penetrating only a short distance. However if you are moving in a fair distance then other issues arise. Generally the side of a HSS parting tool will only rub, which may reduce the quality of the surface finish, but it may also deflect the blade so much that you run the risk of it shattering. This rubbing also causes friction. Friction causes heat. A real enemy to HSS tools. Coolant will help carry the heat away, but it will not take away the side stress on the HSS blade.
    I have always said to my students, that you can get away with being very slightly(read a few thou) below centre when parting off, providing you are NOT going to the centre of the part. But you can never get away with being above. There is always exceptions to the rule. But you will discover those while you work. You will never find those in a book.

  • Thanks for further tips, Peter. I can see parting off strikes a chord. Others have suffered through it, LOL. Perhaps I should’ve written a more general parting off article to pick up more of these points, buy you guys are doing a good job of adding the information right to the comments.

    On the topic of squareness, I agree, it is critically important and can be compromised if the setup flexes at all. I will typically use the chuck face for a quick squaring up of the parting tool if it is available. sometimes a 1-2-3 block against the face is helpful in gaining better access.

    Otherwise, I’ll sweep an indicator and tram the parting tool just as you would a mill vise.

  • Hi Bob, Just a thought on this..I am not a machinist just a hobby machinist,my trade is completely different.A guy I worked with is a toolmaker with about 40 years experience,and he has shown me quite a lot of different things and I am very grateful for what he has shown me,and also some of the things he has told me I had trouble understanding due to never being involved in machining.

    I asked him about parting off after seeing a lot of people on u-tube being somewhat hesitant, so he came around and set up a parting blade that I had bought, the insert type,told me to set it right on centre, never above centre, and make sure it was at 90 degrees to the part,asked me what speed to run the lathe at,to which I replied, how would I know…lol.

    So he had a look at the insert packet and showed me how to work out the rpm and sfm, started the lathe,turned the coolant on, and said let’s go, as soon as I started to cut there was a bit of a noise and I backed off, he laughed a bit and said, no keep going don’t back off, I had just made a common mistake.

    Anyway after a few goes I started to become more confident,and a lot of times now when I part off, I use the auto cross feed I seldom wind in by hand,not that I am saying I am an expert at parting off as there are a lot of different steels around.But he said don’t be scared of parting off, the more you do the better you will learn.

  • In cutting threads on a manual lathe are there any mathematical formulas or tables to determine how far the cross slide should be advance for each thread pass.

Leave a comment


Do you want to be a better CNC'er in 37 Seconds?

Get Better Tool Life, Surface Finish, and Material Removal Rates Fast.

It's that easy. You can install and get results in a matter of minutes.


Start Now, It's Free!



  GW Calculator

  GW Editor



  Deals and Steals

CNC Blog








     Feeds and Speeds

     G-Code Tutorial

     CNC Machining & Manufacturing

     DIY CNC Cookbook

     CNC Dictionary

CNC Projects


     Machinist's Search


     Online Groups


     Reference Data


     CNC Dictionary


     Tool Brands


     Hall of Fame

     Organization: Soon!





     Our History

     Privacy Policy

All material © 2016, CNCCookbook, Inc.