Category Archives: Machinist Tips and Tricks

This category contains a variety of machining and machinist tips and tricks derive from our 25+ years of real world chipmaking.

Powering ON / OFF Your CNC — The RIGHT WAY !!

Believe it or not … there is a RIGHT and WRONG way to turn the power on and off to your CNC equipment at the start and end of the day. And the difference can mean increased life for a lot of the electrical components at the heart of your equipment.

During my 20+ years as a field service engineer for Mori Seiki and Yamazen USA … the first thing I taught clients when they received their new CNC machine was the correct way to power up and power off. I knew from my experience that even this little lesson would bring big dividends over the long haul.

The main idea is to dissipate power or bring power on line in an orderly and limited manner. Big power boosts or cuts can damage delicate electrical components over the long haul and can even mean damage in the short run that will eventually lead to big failure.

Let’s start with the power OFF routine …

We’ll start with the power OFF because power on is the exact opposite. So we want to get this done right first off.

The WORST thing to do is to simply cut the power using the breaker on the machine. This creates a huge power vacuum all at once … not a good thing for delicate CNC electrical components. That breaker or switch  usually look something like this …

At POWER OFF … my recommended process is :

  1. Hit the big RED button … E-STOP is #1. This will kill the power to the motors and lock the axis movement preventing any axis jumps due to a bigger power cut. The E-STOP circuit is designed specifically for this type of power cut.
  2. #2 — CONTROL POWER OFF. Next up press the power off button for the CNC control. This will now kill the power to the CNC control components and control panel in an orderly manner. Again … that’s what the control off circuit is designed for.
  3. LAST — turn off the circuit breaker on the machine. Not the panel on the power box at the wall of the shop … the one at the machine. This will be the final power kill but at this point on limited items are still powered up and running.
(1) E-Stop
(2) Power Off
(3) Main Breaker

This is an orderly process that will turn the power off and dissipate power from the components in an orderly and minimum manner.

 POWER ON … the exact opposite :

  3. UNLOCK the E-STOP (which was depressed at power off) … once that is unlocked the power will automatically return … although on some circuits you may need to  press the CONTROL POWER ON again once the E-STOP is released.

Should I Even Bother To Power Off My Machine ?

I know a lot users don’t even bother to turn the machine off … they just keep it powered on continuously.  I also know a lot of thinking here is that the power surge to the components is worse. Yes … that’s true if you just kill the BREAKER as your power off routine … but if you use the process I outlined here you will not adversely effect your electronics with power off … and you’ll save a TON on your electricity bill !!

Hope you found this article useful …
Happy LONG and PROSPEROUS Chipmaking !!

Kenney Skonieczny – President
Kentech Inc.

G Code Circle Milling – Like a PROFESSIONAL !!

Milling a counterbore or doing other circle cutting using an end mill or similar tool can be a powerful and creative machining process. Most times replacing the need for a reamer, boring bar or other sizing tool. This type of cutting, when combined with cutter compensation gives the operator much more flexibility in adjusting the size of the finished hole.

However, the main drawback is usually created using simple programs and is usually found at the entry and exit points where a small tool mark can be created due to the tool pressure caused at the entry of the cut. With a little creative programming technique and some simple calculations, a much more efficient and “professional” program can be created.

In this post, we’re going to take you step by step through a program creation to mill a circle using the “loop in – loop out” method which takes the cutter from the center into the side of the hole using an arc move – then cuts completely around the hole – then loops back to the center using another arc move. This type of cutting gives a real nice finish in the hole, helps maintain size a little better and leaves no tool mark at entry or exit points.

In our example, finish milling an inside round pocket using G02 or G03, a cutter mark will remain from tool pressure at the entrance and exit point of the arc. In order to create a smooth entrance and exit, some “tricky” machining technique must be employed because most machines do not have a “canned cycle” for the type of cutting explained here. Although this employs nothing more than simple G02 or G03 commands, the manner in which the codes are used and the type of process that results, makes efficient use of the simple codes and makes a more attractive and accurate workpiece.

The objective with the example below is to create a smooth transition into and out of the cut. In the example below, we are attempting to machine a 2 in. radius circle with a 1 in. radius cutter.

STEP #1 : We calculate the arc needed to move the cutter from the center of the pocket to the finish wall edge. In the example below, we use the following formula :

2.00 (pocket radius) – 1.00 (cutter radius) = 1.00

This is the distance needed to move from the pocket center to the wall edge, allowing for the cutter radius.

STEP #2 : Next divide the total distance in half to obtain the radius needed to swing an arc from the center to the outer edge as calculated above.

1.00 / 2 = .500

If you like this concept … we invite you to take a look at our Kipware® Conversational CNC Programming Software …it auto-creates G code from fill-in-the-blank forms … NO CAD experience required !!! CLICK HERE for MORE

Cutter  Compensation  Note : 

Some controls will allow for the activation of CUTTER COMPENSATION on the example program block #1. In that case, you can calculate the same as above but do not compensate for the cutter radius, instead call the cutter compensation G Code and compensation offset number on the program block. In our example, the program block would be :

G02 G91 G42 X2.00 Y0 R.500 D12 

In this block, we are using G42 (cutter compensation right) and storing the radius of the cutter in offset #12. Using cutter comp as above will allow for the easy adjustment of the pocket size by adjusting the value in offset #12. Don’t forget to cancel the cutter comp with G40 after the tools cutting is complete.

 Creating a “CYCLE” : 

Using a simple combination of sub-programming, you can take the example above a step further and create a simple Z axis step-down cycle resulting in the roughing of the above example with little effort.

In the program example below, we are taking the circle cutting routine created above and storing it in a sub program. The main program will step the Z axis down – call the sub-program to machine the hole at that depth, then return to the main program which will in turn move the Z axis to another depth and start the process again. This “cycle” repeats until the total depth is achieved.

Main Program : 

{ start and position the tool to the hole center as normal }

G01 G90 Z-.100 F15.0 ; — move to the depth of the first cut

M98 P1111 —————- call Sub Program O1111 which does the cutting as above

G01 G90 Z-.200 F15.0 ; — move to the next depth of cut

M98 P1111 —————- call Sub Program O1111 again at the new depth

G01 G90 Z-.300 F15.0 ; — move to the next depth of cut

M98 P1111 —————- call Sub Program O1111 again

G01 G90 Z-.400 F15.0 ; — move to the next depth of cut

…. etc. till the desired depth is realized

Sub Program : 


G02 G91 X1.00 Y0 R.500 F10.0 ; — circle to the hole edge

G02 I-1.00 ; ——————— cut the complete circle

G02 X-1.00 Y0 R.500 ; ———— circle back to the center

M99 ; —————————- return to the main program

This is just one example of the combination use of the sub-programming feature and “simple” programming codes to create a user cycle. You can always use your initiative and create some other ideas. Maybe think about these  :

How can you put the Z axis move in the sub-program as well ?

Call the sub program and repeat a set number of times ?

… any others ?

Kenney Skonieczny – President
Kentech Inc.

G62 – Automatic Corner Override – Brief Overview

When milling, have you ever experienced chatter and poor surface finish when you are attempting to machine an inside corner radius using the same feedrate as the rest of the workpiece?

Oftentimes, this results in the programmer having to decrease the cutting feedrate in the blocks where the tool cuts in the corner areas. Is there another way to have this done automatically ?

The most common situation above occurs when cutter compensation (G41 or G42) is active and you are attempting to cut in a corner where the toolpath inside radius and the TNR offset value are of similar size. You can use the machine to calculate an automatic decrease in feedrate using the G62 – Automatic Corner Override command ( This is a Fanuc G code … check your programming manual if you are programming a non-fanuc compatible machine … there is probably a similar command.) When G62 is commanded, the machine adjusts the feedrate automatically to maintain the cutting quantity per unit time in the corner. This often results in improved surface finish without the intervention or alteration of the programmed feedrate.

A couple of notes for G62 use :

  1. Once commanded, G62 becomes MODAL and must be cancelled by commanding G64 (normal cutting mode) or by Power Off as G64 is usually the normal power on mode.
  2. G62 can only be used effectively in conjunction with Cutter Compensation – G41 / G42.

Kenney Skonieczny – President
Kentech Inc.

G01 — Use ME for RAPID Movement Too !!

To experienced G code programmers … we might be stating the obvious here … but for the novice, this blog post may reveal a valuable programming trick that may come in handy during your CNC programming life.

When learning G code programming … one of the first codes taught are G00 and G01. G00 is used for rapid movement … making the axis move at their top speeds … while G01 is used for moving at a feedrate in a straight line. If we take a look at some of the details of these codes … we will also reveal a few hints into how they can be manipulated beyond their basic design.

A couple of notes on G00 :

  • As stated G00 executes axis movement at their top speed … so we can get to the destination as quickly as possible.
  • Oftentimes … the two axis are not created with the same rapid traverse speed … for example the X axis may be able to travel 1200 IPM while the Y axis is only capable of 850 IPM. This is often due to the design of the machine … size of the ball screw, etc..
  • When two axis are involved in the G00 move … the distance each axis has to travel is the determining factor as to which axis reaches it’s destination first … resulting in a move that is not a straight line.
  • Oftentimes … the machine is equipped with a RAPID OVERRIDE switch / dial that allows the user to slow down the rapid movement by some percentage … 25% – 50% – 100%. BUT … there is usually no a variable setting … so the rapid movements are hard to control when working in tight corners during program prove out.

A couple of notes on G01 :

  • G01 executes axis movement at a programmed feedrate … the axis moves at a rate that we determine via the F command.
  • When two axis are involved in the G01 move … the machine’s CNC controller calcuates the speed at which each axis will move so that each axis arrives at the end point at the same time … always resulting in a move that is a straight line.
  • Oftentimes … the machine is equipped with a FEEDRATE OVERRIDE switch / dial that allows the user to slow down the feed movement by percentages … there is usually a variable setting … and allows for extensive flexibility during program prove out … even to pause the movement completely.

SOooo What??

The points outlined above lend themselves to some “bending and twisting” and result in some nice features that can be employed in our CNC programming … such as :
  • We often think of G01 movement as cutting feed or cutting movement … but using a faster feed of 200-300 IPM or higher … when not cutting can turn a G01 move into a “rapid” move.

The two main advantages of programming G01 for rapid include :

  • Programming a fast feed into a G01 block will always result in a straight line move … comes in handy sometimes when moving around the part and avoiding possible collisions that a non-linear move like G00 may cause.
  • The FEEDRATE OVERRIDE switch allows us greater flexibility during programming prove out than the RAPID OVERRIDE … but yet when running at 100% the fast feedrate doesn’t have to effect our cycletime.

Thinking Outside the Box … always produces interesting results. In this case … we can bend the intended use of G01 to assist us creating an un-intended yet beneficial cutter movement.

 Got Ya Think’in ??
Any Other Ideas ??

Shop Floor Programming … Why It’s Different and Why It Matters

If you have ever worked and lived on the shop floor … as we did for over 30+ years … you know there is a difference between programming in a job shop type environment  … what we call every day programming / shop floor programming … and complex “die and mold” programming which is the true essence of CAD/CAM and CAD/CAM programming.

It’s a fact … it’s real … and it can DEFINITELY mean the difference between profit and loss. 

This post is dedicated to exploring exactly what we mean …. because there is a HUGE difference in employing a SHOP FLOOR PROGRAMMING model vs. a CAD/CAM PROGRAMMING model. 


Our definition of shop floor programming is the programming of the simpler, everyday type workpieces on the shop floor … perhaps directly at the machine … by the shop floor personnel using simpler G code creation tools like Kipware® conversational. It is in contrast to the CAD/CAM programming model where CAD/CAM software … with the start of everything dependent on a CAD drawing … is used by dedicated “CAD/CAM” guy(s) to create G code programs. Our 30+ years of shop floor experience have proven to us that everyday operations like simple milling … drilling … tapping … turning … grooving … boring … for the everyday type parts machined in 95% of job shops around the world every day … can be created more efficiently using the  shop floor programming model.

In a job shop and / or production environment … shop floor programming can especially pay big dividends when the statement “the more the merrier” is employed. The more personnel that are involved in the creation of G code programs … the better the efficiency and the better the output. And of course, allowing shop floor personnel to create the simpler, everyday CNC programs using tools like our Kipware® conversational means increased profits along with that increased efficiency and output.

In most cases … being a good chipmaker is the key experience requirement. Someone who can cut chips … knows material removal and all that that encompasses … and knows fixturing and workholding. While the knowledge of G code in any CNC environment is always essential … tools like Kipware® conversational can assist those chipmakers with limited G code knowledge create fast and efficient  G code programs from scratch. Many chipmakers have a handle on G code but creating a G code program from scratch can be a daunting, cumbersome and sometimes slow task. The reverse is also true … CAD/CAM / computer operators often lack the chipmaking and fixturing expertise of the shop floor personnel resulting in non-efficient CAD/CAM programs or constant re-programming because of real world consequences.


Is contrast to the points outlined above … the programming of complex … what we’ll call “die and mold programming” … should be the main prerequisite  behind a CAD/CAM programming model. CAD is an essential tool for design and engineering … and while the the CAM portion of the CAD/CAM model can be disputed … for complex, 3D programming die and mold programming … it to is essential.

However, using a complex CAD/CAM system and requiring CAD/CAM trained personnel to create G code programs for the simpler, everyday type workpieces can mean the exclusion of valuable chipmakers from the programming process. It can oftentimes lead to slow program creation and thus decreased efficiency, productivity and output. The fact is … CAD/CAM was never designed for EVERYDAY programming. It was created to handle complex design and the programming of complex aircraft and die / mold components. It was always an afterthought to adept it to production programming. The mere fact that everything starts with a drawing inherently makes it more complex and cumbersome for this task.

 Debating the CAM in CAD/CAM

Even when utilizing a CAD application for design … still not every workpiece should be or needs to be programmed through the CAM module nor by the “CAD/CAM programmer”. The point we want to make here is that CAD can be different than CAD/CAM. While having a drawing and design application … a CAD program … can be and oftentimes is essential … the CAM part is up for discussion. Handing off a drawing and having the simpler workpieces … the everyday type workpieces … programmed on the shop floor can free up additional programming resources to concentrate on the more complex programming required for the more complex components. Shop floor programming can be the key that unlocks increased efficiency and productivity … even when using a CAD ( and / or CAD/CAM ) programming model.

And home and hobby shops?

One man, small shops and hobby makers can also reap the rewards of NOT programming every workpiece through a CAD/CAM system and using a shop floor programming application. The quick and efficient programming made possible through tools like Kipware® conversational can assist in realizing the quick and accurate production of workpieces … whether a single component, multiple components or in production. Spending time creating drawings … because every CAD/CAM program starts with a CAD model … for even the simplest of operations … can slow down, bog down, and waste time that home and hobby shops can’t afford to waste.

Although usually a CAD system is required in these environments … mainly because small shops and one man shops also do their own design … shop floor programming and tools like Kipware® conversational can also be an essential part of their efficiency.

Bottom line …

CAD/CAM is a great tool. But it can be overkill … can often bog down a programming environment … and can remove good chipmakers from the programming process. These chipmakers are more often than not the keys to unlocking a good SHOP FLOOR PROGRAMMING SYSTEM and the benefits that can come from that.

Don’t be fooled by the CAD/CAM marketing.
Don’t get caught in CAD/CAM overkill.

We invite you to explore Kipware conversational and see how shop floor programming can set you and your shop floor free !!

Kenney Skonieczny – President
Kentech Inc.

When is a CNC Program More Than JUST G Code?

… when it’s a set-up sheet as well.

Most people are familiar with the ability of most CNC controls to include COMMENTS in the CNC G code program itself. Comments are designated in a variety of ways from :

  1. ( THIS IS A FANUC AND OKUMA COMMENT ) … any text inside (  ) is considered a comment.
  2. ! THIS IS AN ACRAMATIC COMMENT … any text following the ! is considered a comment.
  3. ; THIS IS A FAGOR COMMENT … any text following the ; is considered a comment.
  4. and on and on we could go.

Comments can be a real help when they include operator messages … such as :


… but comments can go well beyond operator messages and can turn your G code program into a complete set-up doc as well that includes tool information, part zero locations and even stock descriptions.

Most people will create either a paper or digital tool sheet / list and / or set-up sheet / list that is stored and re-called when the corresponding G code program is going to be run again. The set-up personnel refer to these docs to set the machine up … loading required tools and setting height offsets and work offsets. Works great … no problems. But is there a better alternative? The answer is a “could be” yes. By storing this information directly in the G code program using the COMMENT capability of your CNC control. For example … something like this :

( PART #1234 )
( PROVEN PROGRAM : 7/2/2014 )
( T1 / H1 = #3 CENTER DRILL )
( T2 / H22  = 1/2 DRILL )
( T3 / H3 = .500 CARBIDE END MILL )

So what is the advantage of keeping this info directly in the G code program using the COMMENTS capability of the CNC control?

  1. Harder to misplace … if you’re going to run the program, you need the program … and all the set-up info is right there stored right inside the G code program.
  2. Complete info is there for all to see at any time … no rummaging for loose paperwork or docs.
  3. Any edits or changes can be made directly in the program … when the running program is saved after execution … all the current set-up info is changed and saved as well including all updated data.

We often get asked … “Won’t this slow down my program execution speed?” The truth is that it will … but it will also be so minimal that usually the cost savings of having comments and all the convenience that comes with it far outweigh any reduction in program execution time. Rummaging around for lost documentation or re-creating lost documentation would be the real money waster.

Just a little something to think about if you haven’t considered COMMENTS already in your CNC programming. We touched on only a few points here … but we’re sure you can find many more benefits depending on the capabilities or lack thereof pertaining to your particular CNC programming operation. The fact is that expanding the use of COMMENTS in your CNC programming could be a real time and money saving alternative to digital or paper documentation.

Until next time … Happy Chip Making !!
Kenney Skonieczny – President
Kentech Inc.

Why Use Cutter Compensation In Your CNC Programming ?

The story has been circulating here about a support issue that was raised recently where a Kipware® conversational customer inquired about how to have KipwareT® output program coordinates using the tool center vs. using G41/G42 cutter compensation and the imaginary tool tip on the control. The conversation went something like this :

Support Staff : “Why would you want to do that? That’s really not a good programming practice.”

Client : “Well all our programs are written like that.”

Support Staff : “OK … but that’s not a good programming practice. When we created Kipware® conversational we wanted to include best programming practice so KipwareT® outputs G41 / G42 and does all the calculations and automatically includes all start-up and cancel blocks and code … so it creates a better program. No worries … even if you don’t know how to program it KipwareT® does it all for you.”

Client : “Yes but nobody programs like that.”

Really? Nobody out there programs like that? We find that hard to believe.

So … we decided to post some of our main reasoning for considering the use of cutter compensation on the control as “Best Programming Practice”. If you agree with our points … we hope that you will consider making the change … getting educated … and to start creating your G code programs using G41 / G42 cutter compensation.


  1. Program Coordinates … programming to the tool tip center means that coordinates in the program do not reflect actual part print coordinates. Coordinates are based on the tool tip center rather than on the part dimensions. You can imagine the trouble and confusion that happens when edits need to be made.
  2. Tool Interchange – Turning … since the G code was written for a specific tool radius … the program will only function correctly for that tool radius. Decide to use a 1/64 radius for finish when the program was written for a 1/32 radius … re-program or re-generate the toolpath.
  3. Tool Interchange – Milling … I think this point probably comes into play more for milling G code than turning G code. Does your shop always have perfect .500 end mills? If so … WHY ???? Re-grinding end mills is quite a cost saver … but it means your end mills might be .485 or something odd. If you use G41 / G42 … who cares? Just enter the correct offset value.
  4. Dimensional Adjustments … Come on, this is the real world. There is no reason to keep running back and forth to the CAD/CAM guy or programming office when dimensional adjustments need to be made during production … and they will be because cutting conditions are not theoretical, they’re real !!. Cutter compensation and part / tool offsets can handle probably 99.99% of all dimensional adjustments. Use the power of the control !!

Some of the main reasons we hear for why clients don’t use cutter compensation ( and none of them are valid by the way ) …

  1. Nobody taught me. Come on … grab a hold of your future and do some “playing” at the machine … or read for yourself. This is a truly important programming tool … you need to know hoe to use it if you want to go anywhere.
  2. Nobody uses it.  Like our scenario above … just keeping following the crowd … over the cliff. If I ran that shop … the guy that comes to me and says “I think we need to change the way we think about cutter compensation” would have more of my respect than the guy who gives me the excuse “That’s the way we always did it.”

“I’m not stubborn … 

it’s just that doing things your way is stupid.”

After having spent more than 30+ years creating … editing … teaching … G code and running shops on a day-to-day basis … cutter compensation is one of the most mis-understood and mis-used programming feature. And also the most important tool a programmer and operator and shop foreman has at his/her disposal.

If you agree … want to learn more … or just want some additional reading … below is a link to one of our previous posts that dealt with this issue also … CLICK HERE for that article.

Unfortunately CAD/CAM systems have made it so easy to program with tool tip radius … but in the real world, on the shop floor, it can be a real detriment to productivity and efficiency. We urge any CNC programmer out there who is not using cutter compensation on the control to step up and take control of your future … get educated on cutter compensation … and use cutter compensation in your G code. Your future will be a lot brighter … and profitable.

Kenney Skonieczny – President
Kentech Inc.

Deciphering M CODES for Your CNC Machine

Recently we have been working with some Kipware® conversational clients assisting them in setting up their Kipware® post processor blocks for their G code output. With the addition of our EIA MENU option … users now have greater flexibility in using machine functions ( M ) functions in their G code to accomplish specific tasks. One example might be … parts catcher UP or DOWN to catch a part being parted-off … or chuck OPEN and CLOSE during a bar feed operation … or 4th axis CLAMP and UNCLAMP for CNC mill.

During these sessions we are coming across the situation where the end user doesn’t know the specific M for their machine to accomplish some of these tasks. And for whatever reason … manuals lost or misplaced … machine was purchased used and no manuals were included … or whatever … the end user does not have any Operator or Programmer manuals for their machine which would normally outline the M codes and their function. Without the manuals … they have no way of finding out what M functions control what. OR DO THEY ??

Let’s start this journey with a brief explanation of the HOW’s and WHY’s of CNC M functions. 

  1. First … there is no “industry” standard for M functions. Although you might find that M08 and M09 or M03 and M04 work for most CNC machines … there is not an industry standard that says they must meet a certain criteria.
  2. M functions are designed by the machine tool builder … not the control manufacturer. So you may have (5) Fanuc controlled machines in your shop … some Mori Seiki’s some Hitachi some Leadwell … all with different M functions. Because the M function circuits are designed by the machine tool builder and not Fanuc.

With those basic facts … when you ask your buddy “What’s the M function to open the chuck?” … and he says “M11” … and it doesn’t work on your machine … now you know why.

So how can you find out the M functions for your machine WITHOUT an Operators or Programming manual?

One of the best ways is to use either the electrical or ladder diagram for the machine. Although most Operator or Programming manuals get lost along the way … mostly because they are not kept with the machine but rather float around the office or shop … electrical diagrams ( which outline the electrical circuitry of the machine ) and ladder diagrams ( which outline the logic of the machine ) are most often kept inside the machines electrical cabinet. Open up the doors and you will usually find one or the other or both.

Even if you’re not electrical savvy … the circuits are pretty clearly labelled and you can find say the CHUCK OPEN circuit and trace things back to find the appropriate M function. Again … because they are built and designed by the machine tool builder and their electrical outline is outside the realm of the control … these circuits are contained in the machines electrical documentation … not the docs for the control.



Above is a pic of an electrical diagram for a Shizuoka CNC vertical mill … with an exploded view on the bottom. You can see fairly easily even without any electrical savvy that the M10 command will control the 4th axis clamping function. 

With today’s more sophisticated controls … oftentimes the ladder diagram is available directly on the machine controls CRT. You can pull up the ladder and even search for the appropriate function command … but in other cases the “old fashioned” printed ladder can also usually be found in the machines electrical cabinet.

Taking a look at either the electrical diagram or ladder will usually result in some additional road or path to travel to find the appropriate M function on your machine. A simple execution of an MDI command is a good test to see what happens. The old Trial and Error method will open up additional doors or produce the desired results.

M functions are powerful options on your CNC machine that can help automate many tasks and make your manufacturing more efficient. Know that you know the trick to discovering the M functions on your CNC machine … why not peruse your electrical or ladder diagram and see if there are any you might be missing in your programming?

Like what you see?
Please visit us at

Kenney Skonieczny – President
Kentech Inc.

Shop Efficiency Series Part 5 : Multi-Function Tools

Multi-function tools have been around for quite a while but oftentimes are overlooked for a variety of reasons ranging from lack of understanding to shop inventory. But the truth is that in many situations, multi-function tools can be a key to reduced cycletime … more efficient machining … better workflow … and that ultimate prize … increased shop efficiency.

In this installment of our Shop Efficiency Series … will take a quick look at some of the more common multi-functions tools … outline some of their features and benefits … to hopefully bring about a better understanding and start that “machinist mind” thinking about how these types of tools might be able to benefit your particular shop efficiency.

Milling : Multi-Function End Mill
Multi-function end mills are designed with two main features … low cutting resistance and good chip evacuation when center cutting / drilling and milling at an angle. These two features give these tools the ability to perform both drilling and milling … which makes them an indispensable part of your tooling inventory. Imagine being able to select either plunge milling or side milling when machining … or employing a combination of both because the tool has that capability. The image below gives the whole range of machining op’s that are available with this tool type … it illustrates well their flexibility and capability … and speaks volumes about why they should be one of your go-to tools. As you can see there are a variety of operations where they can make an impact.


Additional Information / Recommendation :

Tool Name / Manufacturer : Kyocera MEY – Ultra Drill Mill
Catalog / Brochure Link :


Milling : Thriller – Drill / C’Sink / Tap
If you have never utilized a combination drill / thread mill … this tools will really blow your mind. Center drilling … drilling … countersinking … thread milling or tapping as means of creating a tapped hole is SOOOO NOT KOOL !! 4 tools combined with the tool changes … stopping and starting … tool costs … etc. … make this method of creating threaded holes simply NOT ACCEPTABLE when discussing shop efficiency. You may have held off on these thinking that they are really for specific types of threaded holes … but the more you look the more they make sense as the go-to-tool .. with tapping and other standard operations as the secondary option. Our favorite tool comes from Emuge Corp. … which also has outstanding field support BTW … and combines drilling, countersinking and thread milling in one tool … quickly illustrated below.


But rather than yapping about all the benefits …we suggest watching the video link below … it tells the story way better than words.

Additional Information / Recommendation :

Tool Name / Manufacturer : Emuge Corporation – Thriller
Catalog / Brochure Link :

Video Link :

Video Link :


Turning : Groove / Turn Tools

For machining operations that include both turning and grooving … it oftentimes makes sense to combine those operations with one tool. Of course the type of material and type of groove machining play an important role here … but when possible, using a combination groove-turn tool can be very beneficial and efficient. Eliminating the tool change and related non-cutting time can improve cycletime … but the flexibility of the tool opens up a wide variety of machining options as well … beyond just grooving operations.


As the illustration above shows … machining operations such as PARTING OFF … GROOVING … BACK TURNING … and STANDARD TURNING are all possible with this tool type.

Additional Information / Recommendation :

Tool Name / Manufacturer : ISCAR – Groove-Turn

Catalog / Brochure Link :

Video Link :


 Turning : Boring with an Indexable Drill

In certain non-turning tool applications … it is possible to utilize the same indexable drill used to drill a hole as a boring bar to open up the hole diameter. Benefits of course include decreased cycletime and the use of less tools … but this should be considered carefully and success involves many factors. As stated many times in our blog … we recommend Sandvik tooling quite often … and they have a great online resources that delves into this type of machining and the options to consider before giving it a go in the link below … just click the image to open up their information page :



Of course there are thousands of ways to use standard type tooling as a multi-function tool … and we are sure that your machinist mind has come up with some novel ones along the way. But we felt the need to include at least some of the more “common” options in any conversation about shop efficiency. So there you have it. Some food for thought … and some multi-function tooling options you may not have been aware of or considered.


Please come back for our next installment in our series on Shop Efficiency.

Kenney Skonieczny – President
Kentech Inc.

Shop Efficiency Series Part 4 : Re-Thinking Your HEIGHT OFFSET Strategy

As we have been stressing throughout this Shop Efficiency Series … keeping your spindle running and the green cycle light lit is one of the main keys to making money and profits. In Part 4 we’re going to shift our attention back to the VMC and HMC world and send out some thoughts regarding Tool Height Offsets … “touching off” tools … and how to get that inevitable task done quickly, easily and efficiently … so that the spindle stays running and the tools gets in the chip.

Tool breakage or the need to replace dull or ineffective tools can cause huge loss of cutting times and spindle on time. With the implementation of the simple system we outline below … you can insure that replacing or setting up your tools for machining can be done quickly and efficiently with as little disruption to cutting time as possible. There are some initial costs involved … but the ROI is fast and you’ll see the results immediately.

We’ll take you through the Set-Up and Process first to show you how it works … then highlight some of the Features and Benefits that can achieved by utilizing this system. The basic idea is to utilize a MASTER TOOL to set the part Z0 position … and use the HEIGHT OFFSETS to calibrate the distance difference from the MASTER TOOL and EACH CUTTING TOOL. This system leaves us only the MASTER TOOL to re-calibrate for each workpiece … and allows us to leave the cutting tools unchanged no matter what part we’re running. Setting up ONE tool is obviously faster than setting up multiple tools.

What You’ll Need :

  1. Height Gauge … digital gauge will obviously function the best.
  2. Master Tool ( more details below )
  3. Tool Holder Adapter or Setting Fixture


The Master Tool :

In order to utilize the features of this system, you’ll need to create a MASTER TOOL. What we refer to as a master tool would be a piece of stock, say a piece of turned, ground and polished stock or drill rod loaded and secured into a tool holder. It should be secure in the holder … the best way is with a shoulder butting against the tool holder face so it has a positive stop. Another feature is to make this master tool close to the length of the machine specs longest tool. This way you’ll know that no cutting tool can be longer than this master tool.

Tool Holder Adapter or Setting Fixture :

Once you have created your stable Master Tool … the next stable component should be your setting fixture. With a little thought and work you can turn a standard tool tightening fixture … such as the ones pictured below … into something suitable for this purpose … with the main criteria being the stable repeatability of the tool holder positioning.


The Process :

On a surface plate, set up your height gauge and tool holder adapter to allow for the measuring of your tools. To measure a tool :

  • Place the MASTER TOOL in the setting fixture and set zero at the top of the master tool.


  • Place a cutting tool to be measured in the setting fixture and record the reading at the top of the tool’s cutting edge. This is the distance from the master tool tip to the cutting tool tip. This dimension is the value that is to be entered in the machines height offset table for the measured tool.


  • Repeat the second step above for each tool to be measured, recording the value on the height gauge for each tool.
  • Load the tools in the magazine and enter the measured height offset values from Step #2 above into their respective height offset table positions.
  • Using the MASTER TOOL, touch the Z0 surface of the workpiece and record the value from the home position to the Z0 location. This value should be entered in the Z table for the work offset (G54 – G59) to be used in the program.

That’s it. 

Your program is ready to run. Your program will call up the G54 – G59 work offset or similar and will know the distance from the master tool to the Z0 location. Using the H value call in the program, the machine will calculate the difference between the master tool and the measured tool and adjust as required.

Now that we’ve set the thoughts and ideas in your mind … feel free to deviate and expand on the basics outlined here.

 Some Features and Benefits :

  1. Let’s suppose you’re going to set up a new job next but will utilize some of the tooling from the previous job. The only set-up required is to use the Master Tool to touch the new Z0 surface, changing the value in the work offsets with this new value. Your cutting tools and their height offsets can remain the same. Save time by touching off one tool instead of many.
  2. You can set-up a spare tool or replacement tool off the machine using the master tool and the height gauge … insuring that your spindle will be back in the cut faster.
  3. You can load say a nice cutting carbide mill in the magazine and use it for a variety of different jobs. No need to touch it off all the time, just use the master tool to get your work offset in Z.
  4. Measuring tools becomes easier, allowing more people to assist with the tool setting . Setters don’t need to know how to operate the machine.

From experience, once you try this method you’ll find it saves you all kinds of time. The best advantage is being able to call out set tools that stay in the magazine. This really speeds up the set-up and changeover process.

Stay tuned for more posts in our Shop Efficiency Series.
Next up we’ll take a look at MULTI-FUNCTION tools that can perform multiple types of cutting and save your shop a ton of time in the process.


Kenney Skonieczny – President
Kentech Inc.