Created and Maintained by the Real World Software Developers and Machinists at www.KentechInc.com ... click here to check it out !!

Wednesday, August 5, 2015

Canned Cycles in Turning - What You Need to Know - Part #2

This post is continuing with the important feature of programming canned cycles for rough turning. In Part 1 we discussed the general outline, format and command lines for the cycles ... in Part 2 we want to illustrate some examples using Fanuc ( and therefore Haas ) programming that hopefully we give an even clearer picture of the uses and commands for these cycles. We do have some Okuma Programming Notes at the bottom of this post.

The examples will use the same shape ... but will illustrate the to main Fanuc cycles for bar stock roughing ... G71 -Turning and G72 - Facing.

G71 will produce a cutting motion along the Z axis ... generally referred to as a turning motion. The G72 cycle will produce a cutting motion along the X axis ... or a facing type motion.

The way we position our Points A - B - C will also determine the motion as illustrated below. The general rule of thumb is to describe the cutting motion through the finish contour code in a motion that moves from A to B along the contour to C. This description will assist you in placing Points A - B - C in their correct location in relation to the part and the contour.

___________________________________________________________

Example #1 : 
OD Cutting Along the Z axis - Turning
(1) First we established our points A - B - C and using a clearance amount of .100 in X and .050 in Z.
(2) In our program ... the first step is to rapid to point A ... N1000 = our P call in the canned cycle block.
(3) Then command the Canned Cycle Call
(4) Then rapid to point B and proceed around the part contour to point C ... N1100 = our Q call in the canned cycle block.

G96S650M03
G00X11.0Z1.0M08
G00X10.3408Z0.05
G71P1000Q1100U0.01W0.01D0.1F0.012
N1000G00X4.8729.0Z0.05
G01X4.8729.0Z0.0F0.012
G01X4.8729Z-1.2967F0.012
G01X6.9769Z-1.998F0.012
G01X6.9769Z-3.4277F0.012
G01X10.2409Z-3.4277F0.012
N1100G00X10.3408Z-3.4277
G00X10.3408Z0.05

___________________________________________________________

Example #2 :
OD Cutting Along the X Axis - Facing

By re-arranging Points A - B - C ... and using the G72 cycle ... we can change the cutting direction from turning to facing. The basics of the format and steps in the program are the same ... move from A to B along the contour to C ... and this will help us position Points A - B - C.

G96S650M03
G00X10.1000Z1.0M08
G00X10.3408Z0.05
G72P2000Q2100U0.01W0.01D0.1F0.012
N2000G00X10.3408Z-3.4277
G01X10.2408Z-3.4277F0.012
G01X6.9769Z-3.4277F0.012
G01X6.9769Z-1.998F0.012
G01X4.8729Z-1.2967F0.012
G01X4.8729Z0.0F0.012
N2100G00X4.8729Z0.05
G00X10.34Z0.05

___________________________________________________________

Example #3 :
ID Rough Cutting Along the Z Axis Turning

Now let's turn things to focus on ID cutting. Again ... the same procedures and rules apply ... flip Points A - B - C to reflect cutting the ID rather than the OD. The same rule applies ... move from A to B along the contour to C.

G96S650M03
G00X.9717Z1.0M08
G00X0.9717Z0.05
G71P1000Q1100U-0.01W0.01D0.05F0.012
N1000G00X2.7117Z0.05
G01X2.7117Z0.0F0.012
G01X2.7117Z-0.8633F0.012
G01X1.7622Z-1.6563F0.012
G01X1.0717Z-1.6563F0.012
N1100G00X0.9717Z-1.6563
G00X0.9717Z0.05

___________________________________________________________

Example #4 :
ID Rough Cutting Along the X Axis - Facing

And again ... by re-positioning Points A - B - C and using G72 ... we can perform the rough cutting using cutting from the centerline out in a facing motion.

G96S650M03
G00X1.0Z1.0M08
G00X0.9617Z0.05
G72P2000Q2100U-0.01W0.01D0.05F0.012
N2000G00X0.9617Z-1.6563
G01X1.0717Z-1.6563F0.012
G01X1.7622Z-1.6563F0.012
G01X2.7117Z-0.8633F0.012
G01X2.7117Z0.0F0.012
N2100G00X2.7117Z0.05
G00X0.9617Z0.05

___________________________________________________________

Okuma Programming Notes :

Okuma OSP controls refer to the cycles as illustrated above as LAP cycles. The format and use is pretty basically the same as described for Fanuc / Haas controls with some modifications. If you can understand the outlines above ... the notes below should get you through the differences between the Fanuc / Haas format and that required by OSP controls.

  1. For motion for both turning and facing ... command a G85 as the canned cycle command. The variables in the G85 line are outlined in Part 1 of this series.
  2. On the line immediately following the G85 call ... command a G81 for turning or G82 for facing. This G code should appear on a line by itself with no other code on the line.
  3. The N number command on the G85 line should refer to the N number of the line where the G81 / G82 is commanded.
  4. At the end of the sequence that describes the finish contour ... command a G80 on a line by itself to signify the end of the finish profile sequence.

The Fanuc / Haas code from example #1 above has been transposed for the Okuma OSP format below :

G96S650M03
G00X11.0Z1.0M08
G00X10.3408Z0.05
G85 N1000 U0.01 W0.01 D0.1 F0.012
N1000 G81
G00X4.8729.0Z0.05
G01X4.8729.0Z0.0F0.012
G01X4.8729Z-1.2967F0.012
G01X6.9769Z-1.998F0.012
G01X6.9769Z-3.4277F0.012
G01X10.2409Z-3.4277F0.012
G00X10.3408Z-3.4277
G80
G00X10.3408Z0.05


___________________________________________________________

They say a picture is worth a thousand words ... hopefully the illustrations here will help you solidify your programming of these powerful and important canned cycles.

If anyone notices any errors in this post ... please leave a Comment below and straighten it out ... to benefit anyone stopping by ... and Thanks in advance.

Happy Chip Making in 2013 !!



Check out our Real World World machine shop software at www.KentechInc.com
Conversational CAD/CAM
Quoting & Estimating
G Code Conversion
CNC Training
.... and MORE !!!

Wednesday, June 10, 2015

Canned Cycles in Turning - What You Need To Know - Part #1

Canned cycles in CNC controls are powerful features that when used correctly can reduce programming commands and increase program efficiency dramatically. There are a variety of cycles available on most controls, the most powerful are stock removal or roughing cycles. In most of these type of cycles, the user can define the roughing process and cutting parameters, then simply describe the finish shape using G codes. The control will then auto-calculate start and end points as it removes the material to leave the workpiece with the finish shape profile.


Let's start out by explaining WHY THIS IS IMPORTANT !!!

  1. No depth of cut or point calculations required ... all you need to do it describe the finish profile and the control does all the work.
  2. Cutting conditions in the real world are dictated by the actual process of stock removal. Sure you're sitting in your office and writing the program ... everything looks great ...  inevitably when you start to actually do the cutting, things change. When using a canned cycle ... to change the depth of cut ... finish allowance ... feedrate ... they are all just edits to one variable in the canned cycle line. What could be easier !!! If you wrote the code long hand ... you have to re-generate the code each time you want to make any of these changes.
  3. ENUF said ... the CORRECT way to program any rough cutting is to use a canned cycle ... period. Whether through a CAD/CAM system or whatever. Anybody who tells you different is a poor programmer.

The cycle will will outline in this blog post is the G71 cycle in Fanuc / Haas controls ... and the G85/G81 cycle in Okuma OSP controls. This cycle will remove the material along the Z axis, taking depth of cut along the X axis. The command line will define the cutting parameters such as depth of cut, feedrate and finish material to leave as well as telling the control where to look for the finish profile of the part. Usually the command line includes (2) N numbers or some other start / end variables. The control looks between these start / end variables to see what the finished shape looks like. The user uses what amount to a standard finish cut G code program to define that finished shape and places that G code in-between those start / end variables.

For the CNC controls covered here, the same basic programming format  and programming steps should be observed. The first steps are to establish three points that are required to help describe to the CNC control the finished shape desired. These are outlined in more detail in the ANIMATION sequence for this code.

A) Pt. A  : Clearance point in the X axis
  Clearance point in the Z axis

B)  Pt. B  : Along the X plane established by Pt. A, last X diameter of the profile
  Same Z axis plane as Pt. A.

C) Pt. C : Same X plane as Pt. A.
  Along the Z plane as established by Pt. A, last Z face along the contour.



Once the three points above are calculated, the following programming sequence can be used :

a) Start the tools process as normal which means index the tool and start the spindle.

b) Rapid the tool to point A using the normal format rapid approach.

c) Command the CANNED CYCLE block as explained below.


FADAL, HAAS & Fanuc Controls ( Models 6,10,11,12,15 ) :
G71 Pxxxx Qxxxx Uxxxx Wxxxx Dxxxx Fxxxx ;
P = Sequence (N) number of the first block of the finish shape program.
Q = Sequence (N) number of the last block of the finish shape program.
U = Amount and direction of the finish allowance in the X axis ( diameter value in diameter
programming ).
W = Amount and direction of the finish allowance in the Z axis.
D = Depth of cut (radius value) - no decimal point allowed (format = xxx.xxxx) - no sign allowed.
F = Feedrate in roughing - this value overrides any feedrate commanded between P and Q.

Option : S and T commands - Good programming practice would place these commands active earlier in the programming sequence.

Fanuc Controls :
( Models 0,16,18,20,21 )
G71 Uxxxx Rxxxx ;
G71 Pxxxx Qxxxx Uxxxx Wxxxx Fxxxx ;
U = Depth of cut - radius value
R = Retract Amount - the amount the tool will retract before returning to the start for next depth
of cut.
P = Sequence (N) number of the first block of the finish shape program.
Q = Sequence (N) number of the last block of the finish shape program.
U = Amount and direction of the finish allowance in the X axis ( diameter value in diameter
programming ).
W = Amount and direction of the finish allowance in the Z axis.
F = Feedrate in roughing - this value overrides any feedrate commanded between P and Q.

Option : S and T commands - Good programming practice would place these commands active earlier in the programming sequence.

OSP Controls :
G85 Nxxxx Dxxxx Fxxxx Uxxxx Wxxxx ;
N = Sequence (N) number of the first block of the finish shape program. Last sequence is  described as the line containing the G80 command.
D = Depth of cut (radius value).
F = Feedrate in roughing - this value overrides any feedrate commanded between P and Q.
U = Amount and direction of the finish allowance in the X axis ( diameter value in diameter
programming ).
W = Amount and direction of the finish allowance in the Z axis.

Option : S and T commands - Good programming practice would place these commands active earlier in the programming sequence.

d) Continue the program by programming the finish shape starting with a rapid move from Pt. A to Pt. B.. The type of command used here (G00 or G01) will determine the roughing cycle move as it moves in this direction during the roughing process. This block must be labeled with the start sequence number specified in the call in the CANNED CYCLE block.

Fanuc control's have two types of canned cycles called TYPE I and TYPE II. The TYPE I cycle only allows for finished shapes where the axis are moving in one direction ... which basically means that no type of "pockets" can be included in the contour. TYPE II cycles are generally an option but do allow for non-continuous type contours.

Initiating a TYPE I or TYPE II cycle takes place in this block ... the move from POINT A to POINT B. If a two axis move ... both X and Z or U and W are included in this block ... than a TYPE II cycle is initiated if available. If the option is not present ... an alarm is usually generated alerting the user that the option is not available.

In the above example ... and since the Z axis plane of Point A and Point B should be the same ... an incremental move of zero in the axis is usually included just to get the cycle initiated. For example :
G00X1.250W0;
... this move will not effect the movement but since both an X and Z move are commanded ... the TYPE II cycle will be initiated.

e) Complete the program for the tool path to go all around the part contour from Pt. B around the part and ending at Pt. C. You may use G01, G02 or G03 for tool movement as long as the shape is always vertical in the X axis and horizontal in the Z axis. No pocketing is allowed in the shape (Type I only - Type II canned cycles do have this capability). This block must be labeled with the end sequence number specified in the call in the CANNED CYCLE block.

f) Finish the program with a rapid move from Pt. C back to Pt. A. The type of command used here (G00 or G01) will determine the roughing cycle move as it moves in this direction (retract) during the roughing process.

g) Return the tool, like normal, to the indexing position or, while the tool is at Pt. A, call the FINISHING CANNED CYCLE using the same P and Q sequence numbers to finish the part with the same tool.

This outline is fairly complete ... but it may take a little trying and testing for you to get the hang of it ... but the benefits are worth the effort. The ease of editing the cutting conditions and changing or altering the profile make this cycle powerful and real world. If you can master the use of this cycle ... you will reap the benefits for the rest of your programming life. If someone tells you different ... don't believe them.  And if you run across someone who never uses it or doesn't know how to use it ... consider them a poor programmer.

Until next time ... Happy Chip Making !!

At Kentech Inc. we are MACHINISTS who create Real World Machine Shop Software.
Who creates the machine shop software guiding your shop's future ??
Check out all our REAL WORLD CNC & MACHINE SHOP titles at 

Wednesday, May 27, 2015

Product Introduction : ID Clamps

Every once in a while we like to bring attention for our readers to new and innovative machining and workholding products and process that we feel are beneficial to our readers. Such is the case in the Making Chips post as we focus and bring attention to a new workholding clamp from Carr Lane Manufacturing - a leading supplier of workholding and fixture components.

Additional information and specs on the Carr Lane ID Clamps are available on their website through this link : CARR LANE MANUFACTURING

Carr Lane ID Clamps - A Brief Outline

Many of you will undoubtedly be familiar with expanding mandrels ... most commonly used to grip on the ID when turning on the OD. The new Carr Lane ID CLAMPS bring that concept to locating and workholding for milling fixtures. As the image below illustrates ... the ID CLAMP is similar to the expanding mandrel technique where the id CLAMP expands and clamps on the ID of a workpiece, leaving the outside free for machining.  Tightening the tapered center screw with a hex wrench pushes the clamping segments outward, and slightly downward, to exert force on the workpiece's internal bore. These clamps are designed to have their outside diameter finish machined by the customer to suit the bore size, because maximum diameter expansion is limited.

The flange diameter on the ID CLAMP is a machined to a close tolerance ... which allows for maximum locational accuracy. A recess can be machined in the fixture base to fit exactly with the clamp's close-tolerance flange diameter and the ID CLAMP can be mounted using flat-head mounting screws.

In the image to the right ... you can see how the larger ID is used for locating as well as clamping ... and a smaller ID CLAMP is used in the slot to provide additional locating and holding force. With this type of set-up, the entire outside contour is available for machining.

This set-up also illustrates the fact that these ID clamps need not be confined to round holes ... they can be utilized in almost an unlimited number of ID clamping roles ... use that machinist mind and explore !!

We are always on the look-out for new and innovative machining processes ... techniques .... and workholding tips. If you see one which you think would be of interest to our followers of professional machinists and engineers ... please drop us a line at Sales at KentechInc.com.

Until next time ... Happy Chip Making !!

At Kentech Inc. we are MACHINISTS who create Real World Machine Shop Software.
Who creates the machine shop software guiding your shop's future ??
Check out all our REAL WORLD CNC & MACHINE SHOP titles at 

Wednesday, April 1, 2015

Shop Efficiency - Part 8 : Gauging Your Shop Efficiency with the Magnificent Seven

We have dedicated a lot of time and brought out a lot of ideas in our Shop Efficiency series ... but most have been based "on the shop floor" and have targeted machining ... set-up ... and tooling. Quite a few clients have written us to ask about the business side ... more of the "How do I actually know if my shop is efficient" ... which is a great question. So in this post we turn our attention to the shop management and specifically ways of gauging your shop efficiency.


I have listed a few of what I consider critical areas in this Shop Efficiency post ... one's that I feel are among the easiest to gauge and important to watch ... what I call the Magnificent Seven. The points below are not in the order of most importance ... just simply a list of all the metrics. Creating a spreadsheet and taking a daily count with most of these factors will allow you to see the results as they happen ... and over time will reveal the ups and downs of the shop in general ... and allow you to make corrections. You can start your journey on the first of the month ... for example ... and take a few minutes every day or every week to fill in the numbers ... building the information in the spreadsheet as you go along. Make a graph ... and watch what these factors will reveal. If you stick with it ... you will be shocked ... maybe happily ... maybe not.

(1) Revenue Per Man Hour
Revenue per Man-hour is the annual revenue ( or do it by month ) divided by the total paid man-hours, including paid vacations and overtime. Keeping a running total of these activities and although this is a general look at the numbers ... it can be very telling.

(2) Lead Time
Customer Order Lead Time includes order-entry through production to shipment for every job. Again, start a running list from the first of the month and carry on. This stat will reveal your shop efficiency as well as give you a chance to look at the quantity of work going through the shop ... and the time frame it takes to go from order received to revenue received.

(3) Labor Turnover
Labor Turnover Rate is the number of voluntary and involuntary separations divided by the typical
number of employees. Hopefully you won't be keeping a monthly log of this stat ... but keeping a log of the turnover rate will still yield a telling tale. Although this stat has it's own revelation ... it also shows one key point regarding efficiency. When an employee leaves a company ( for any reason ) he / she also takes a piece of that company's memory and experiences with them. That loss of memory or experience can lead to efficiency and productivity loss. A company that experiences high turnover rates needs to find ways to insure that experiences and memory don't leave the building along with the employee. A low labor turnover rate ... as the inverse ... helps achieve and maintain high performance, productivity and efficiency.

(4) Completion Rate
This factor can be described as the On-Time Completion Rate. It is the percentage of goods delivered on time. This is ... obviously ... a direct result of shop efficiency. Keep a log for every job going through the shop and how it fared in the On-Time Completion Rate.

(5) Scrap and Rework
This factor is the Scrap and Rework as a percentage of shop sales. Scrap and rework cost time and
money. Some scrap and even some rework is inevitable ... but this factor may be most useful as an indicator of how well things are going out on the shop floor. An high scrap and rework percentage is an early tip-off that something ... or someone ... needs a deeper look.

(6) Machine Uptime
Total Machine Uptime is the hours of production as a percentage of the total operating hours for the shop per week. In other words, what percentage of an average shift are each of your shop's machines running. Basically put ... your employees get paid every day whether they are productive or not ... idle machines are not making that money even though the employees are getting paid. Therefore, how much a machine is up and running becomes an important factor for determining just how productive and profitable that shop is.

(7) Machine Availability
Machine Availability is the time machines are actually available for use compared to the time they are supposed to be available. Unscheduled maintenance or other problems will reduce a machine's expected availability ... and impact production schedules negatively which in turn reduce the ability of a shop to deliver product on time.

There will be some out there that utter the phrase "I know all this just by being out in the shop every day." And that may be true. But seeing the numbers on "paper" ( it might be your computer screen ) is much more telling ... and much more emphatic ... and makes the point much more clearer.

So ... there you have it ... the Magnificent Seven. Keeping a close eye on these factors or metrics will most definitely put your shop's efficiency in glaring focus ... and will most likely open your eyes and mind to whole list of other metrics that may be pertinent to your particular shop and operation. Taking the time to develop and review your information as it develops will prove to be more than worth the effort ... and keeping the faith will insure your shop is on the straight and steady track.

Please come back for our next installment in our series on Shop Efficiency.
Until next time ... Happy Chip Making !!

At Kentech Inc. we are MACHINISTS who create Real World Machine Shop Software.
Who creates the machine shop software guiding your shop's future ??
Check out all our REAL WORLD CNC & MACHINE SHOP titles at 

Tuesday, March 10, 2015

Shop Efficiency Part 7 - CNC Programming

Our Shop Efficiency series has really taken off ... and we would like to take a few lines to say Thank You to all our readers for your email comments and support. We are very pleased that we have been able to take some of our real world machining and machine shop experiences and turn them into valuable tips and pointers and pass them on to so many of you. Thanks so much for your support.

First - A little background on this Post
At first glance ... since Kentech Inc. develops and sells CNC programming software ... this post might look like straight marketing and a sales pitch for our Kipware® conversational CNC programming software. Actually ... it's a story of just the opposite. Most of our software titles have been designed and developed based on what we saw was lacking in our many years on the shop floor. Our Kipware® conversational CNC programming software is a product of that experience.

One of my most telling personal experiences was working in a shop here in Masachusetts as a CNC machinist. The shop was your typical job shop with all kinds of work coming through the door. Most of it was fairly simple ... with a few plastic injection mold type jobs every once in a while. The CNC programming was supposed to be done by the shop floor machinists ... using a CAM plug-in for Solidworks ... which was a bit complex. No CAD/CAM training more than a simple tutorial was offered or provided. As a result ... since most shop floor machinists were great at cutting chips but lacked intense CAD/CAM experience ... and the jobs were fairly simple ... they often resorted to manual programming. The result was programs loaded with mistakes ... from typo-errors to incorrect toolpaths ... and the result from that was scrap, broken tools and sometimes worse ... but the overall effect was complete shop floor inefficiency.

The frustration level on the floor ... needless to say ... was very high. The machinists were basically unable to do their job ... because no one trained them on the complex CAD/CAM system ... and there were no other tools to help them ... other than an editor.

In this environment ... our conversational CNC programming concept and design was born. It was plain to see that the CAD/CAM and a CAD/CAM programmer was required for the mold work ... but clearly for the 95% of programming we did on the shop floor it was NOT required. In fact ... having the CAD/CAM option as the only option ... actually made things worse.

video

CNC Programming and the LINK to Shop Efficiency
Which brings us to this post and the subject of CNC programming as it pertains to shop efficiency. Obviously ... if the program isn't created in an efficient and correct manner ... the parts don't get made and the money doesn't flow. But just as important as tooling and fixturing ... the program creation process must have options also. You wouldn't think of placing a simple rectangular piece of stock in a custom made fixture ... you would use a vise. In the same way ... you shouldn't think of programming a simple part with a round pocket and bolt circle through a complex CAD/CAM system. The real key to efficient shop floor programming is having an ARSENAL of tools at your disposal. Thinking about your CNC programming as more of a tool ... with multiple choices for various situations ... will help your shop floor reach a higher level of efficiency.

CNC Programming Tools Available
We've listed what we consider to be the realistic options for CNC programming available to anyone creating CNC programs in a "job shop" environment ... the environment where our readers predominately are working ... and the options up for discussion in this post.
  1. CAD/CAM
  2. Off-Line Conversational CNC Programming Software
  3. Conversational CNC Controls
  4. G Code "wizards"
  5. Manual Programming through an Editor
"Wizards" and Manual Programming
To narrow the discussion a bit ... let's remove the two options that are really not realistic in a professional machine shop environment. So called G code wizards are way too simplistic and act
more as hindrance and weight than any kind of efficient tool. Full conversational programming software makes much more sense both from a financial and capabilities perspective. Full, quality conversational software is a programming system ... not a simplistic crutch.

Manual G code programming should only be considered for the simplest of parts. Human error plays too great of a role in any other scenario and really renders this option a last resort choice for a professional programming environment.

That's not to minimize manual CNC programming knowledge and experience. Any CNC programming option used is made VASTLY more efficient and productive when operated through the hands of an experienced manual CNC programmer. A good Editor should always be available to allow that experienced CNC programmer the tool to alter or edit auto-created G code. The point here is that creating programs from scratch manually is not a good choice. Even for simpler programming ... a tool that will auto-generate the code provides stability ... and the manual tweaking of the code can enhance that output greatly.

CONVERSATIONAL and CAD/CAM
Efficient CNC Programming Requires an ARSENAL of Tools
It's more about OPTIONS than OPTION
In a professional environment ... really the two main options are CAD and / or CAM and full, quality conversational programming software. The CAD/CAM option can really be broken down into two options. First the CAD option is a must for any design environment ... even when that is just supporting the shop floor with fixture design. Professional CAD can range from the simple to the complex ... and from the FREE to megabucks. Each shops design and CAD needs would drive that discussion. However ... going from the CAD drawing to a G code program does not necessarily have to through the expensive and complete CAD/CAM system.

Using conversational software ... that CAD drawing can also be turned into a G code program. DXF import can be used in quality conversational software and a variety of other applications to go from a CAD drawing to a G code program.  And of course ... the integrated CAM option can be used to go from that CAD drawing to a G code program.

The main point is that no two workpieces are exactly alike ... and the right programming option for one will most likely not be the right programming option for another. From our experiences ... the best programming method for any job involves (2) main factors :
  • Who is the best choice to create that program? Shop floor? Dedicated programmer?
  • What is the best tool for that individual to use to create that program quickly and accurately?
Letting the correct answers to these questions guide the process ... rather than forcing the path because of limited options ... will increase your shop efficiency when it comes to programming your CNC's. Some thoughts :
  • Maybe the best person to create the program is not full CAD/CAM proficient but would be the best chip-maker for the job ... a shop floor conversational programming option might be the best solution. 
  • Perhaps the job is very complex ... and the only solution for an accurate and efficient toolpath is the CAD/CAM alternative. 
The point to make is that with an arsenal of tools available ... the experience of your personnel and the complexity of the workpiece / programming can dictate the most efficient path to take for the program creation. This allows for the free flow of efficiency ... rather than ramming the square process through a round hole.

Machine Tools with conversational CNC controls
Conversational CNC controls mounted directly to a CNC machine appear to be the perfect solution ... but actually have some important points to consider. The alternative of purchasing a laptop or Windows based tablet ... loading it with conversational software ... is more often than not the better alternative. Here are our major reasons to support this claim :
  1. CHEAPER ... conversational CNC controls can be quite expensive. A tablet with conversational software will cost less than $1200.
  2. PORTABILITY ... having the ability to do the programming on the shop floor, in the office, at home ... makes a portable alternative very attractive.
  3. PROGRAM MULTIPLE MACHINES ... the ability to simply move the laptop around or pass it off to someone else gives you the ability to use the "conversational control" on multiple machines. Other machines can also be purchased without the conversational option ... you already have a "conversational control".
  4. PROGRAMMING AT THE MACHINE ... even though most modern conversational controls have basically (2) modes ... the conversational programming mode and the machine operation mode ... they can often result in headaches and frustration. Either the machine is not runnning waiting for a program to be created ... or the machinist is programming the next job while trying to run production. Not the best environment to say the least.
  5. CNC CONTROLS ARE NOT COMPUTERS ... most industrial grade CNC controls do not have the power or capability of a desktop or laptop PC ... they are simply not constructed from the same components. And if they are a PC ... they are most likely NOT an industrial grade PC and not fit for the harsh machine shop environment.
  6. CONVERSATIONAL SOFTWARE IS MORE POWERFUL ... backed by the power and capabilities of a PC ... conversational SOFTWARE is more powerful and has more options than conversational software operating on a CNC control.
Some Closing Thoughts ... 
The main reason for combining this post into our Shop Efficiency series is to get shops thinking about all the potential programming tools available. Our experience shows that the most efficient CNC programming is accomplished when an ARSENAL of good tools are made available. Inevitably users might find and use their favorite tools ... but the key is that they have the ability to choose from an assortment. Also ... that the other tools remain available when the need arises ... providing choices. Also ... when an assortment of tools is available ... shops can increase the number of people who can create those programs ... and that is a huge jump in shop efficiency. Creating CNC programs faster ... using more people ... means more spindles turning and that means more profits being generated. And isn't that the true test of Shop Efficiency?

Please come back for our next installment in our series on Shop Efficiency.
Until next time ... Happy Chip Making !!

At Kentech Inc. we are MACHINISTS who create Real World Machine Shop Software.
Who creates the machine shop software guiding your shop's future ??
Check out all our REAL WORLD CNC & MACHINE SHOP titles at 

Wednesday, February 18, 2015

Shop Efficiency - Part 6 : 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

-----------------------------------------------------------------

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

-----------------------------------------------------------------

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

-----------------------------------------------------------------

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.
Until next time ... Happy Chip Making !!

At Kentech Inc. we are MACHINISTS who create Real World Machine Shop Software.
Who creates the machine shop software guiding your shop's future ??
Check out all our REAL WORLD CNC & MACHINE SHOP titles at 

Monday, February 2, 2015

Shop Efficiency Part 5 : 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 5 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.

Please come back for our next installment in our series on Shop Efficiency.
Until next time ... Happy Chip Making !!

At Kentech Inc. we are MACHINISTS who create Real World Machine Shop Software.
Who creates the machine shop software guiding your shop's future ??
Check out all our REAL WORLD CNC & MACHINE SHOP titles at 

Tuesday, January 20, 2015

Shop Efficiency Part 4 : Re-Thinking Your Lathe Tooling

We've always been a big fan of Sandvik Coromant and their tooling ... not just because they are a member of the Kipware® family ... but we have always found their tooling, inserts, support and design to be cutting edge and of the best quality. On the shop floor ... they were our tooling manufacturer of choice and never let us down whether in standard type production or when we were looking for that new and innovative tool to get us through the toughest job or materials.

One of my personal best purchases was in converting our CNC lathe tool turret from standard lathe tooling to the Sandvik CAPTO system. I can compare this transformation to the points I outlined in Part #1 of this Shop Efficiency series ... click here to read that article ... and the transformation that takes place when you bring your VMC table into the 21st century. A CAPTO system will bring your CNC lathe turret into the 21st century.

First - What is CAPTO?
The CAPTO system is basically a quick-change, modular tooling system for CNC lathes and turning centers. Instead of mounting tooling directly into the turret ... tools are mounted to quick-change clamping units that are mounted onto the turret. Tools are then easily interchanged by simply changing the "head" mounted onto the clamping unit. Need to change from an 80 degree turning tool to a 55 degree ... just simple swap the "head". Need to change from a .750 insert drill to a 1.250 ... simply change the "head". For live tool turning centers ... need to change from a 1" drill to a face mill ... simply change the "head".

Second - Why Use CAPTO?
This type of modular tooling system comes with tons of advantages. Here are just a few of the more important ones pertaining to the Shop Efficiency factors which are the main focus of this series.
  • Quick tool change which keeps the spindle running and the machine making chips / money. Not only in changing the complete tool type ... but insert changes can take place off-line while the head is replaced at the turret involving less time than an insert change.
  • Greatly reduced set-up and changeover times because of the cutting edge repeatability when re-mounted in the clamping unit.
  • Greater tool stability leads to improved cutting and cycletimes.
  • Greater flexibility in tool selection and tool type.
  • Same tooling can be used throughout the shop ... reduced tooling costs and inventory.
  • Greater options for through-tool coolant delivery ... again, improved cutting and cycletimes.
  • Turning Centers with Live Tools can see the biggest impact. By simply swapping heads that tool station can go from a face mill to a drill to an end mill in seconds. With greater repeatability meaning less set-up / touch off times. In addition ... turning that face mill station into a turning tool station can also be accomplished ... quickly and easily.
I could go on and on ... but I'm sure you're machinist mind sees the point.

Third - Cost vs Features
Like anything in life ... the system does require an initial investment. How much can be spread out over time as you integrate the system into the machine and the shop over time. I will say from
experience that the long term savings are there ... in quicker change overs, increased cycletimes and reduced tooling inventory ... especially if you integrate the system into multiple machines. The beauty part here is that once you have the clamping units on all your machines ... all machine will now utilize the same tooling. That is a huge advantage including reduced tooling costs and inventory all around.

RESULT - Increased Shop Efficiency
As you can see from the points outlined here ... there are a ton of features that can lead your CNC turning department to increased shop floor efficiency with the transformation through a CAPTO system. By integrating the system into your shop bit by bit you can defer the initial investment a bit and still reap the long term advantages and savings as you build the system into your shop floor. From faster insert changes ... to faster tool change-overs ... to faster set-up ... to improved cutting and cycletimes ... your shop floor can certainly reap improved shop efficiency with a CAPTO system.

LINKS for ADDITIONAL INFORMATION 
  1. For a more in-depth look ... take a peek at the Sandvik Coromant video by CLICKING HERE.
  2. For more information on CAPTO in general ... download the informational PDF by CLICKING HERE
Please come back for our next installment in our series on Shop Efficiency.
Until next time ... Happy Chip Making !!

At Kentech Inc. we are MACHINISTS who create Real World Machine Shop Software.
Who creates the machine shop software guiding your shop's future ??
Check out all our REAL WORLD CNC & MACHINE SHOP titles at 

Monday, January 5, 2015

Shop Efficiency Part 3 : The Infamous Milling Vise

Part 3 in our Shop Efficiency Series will expand a little on Part 1 ... and key in on one of the most common workholding options used in the milling world ... the vise. Some of the ideas we will present might be old hat for the more professionals in the group ... but it's never a bad idea to refresh and re-look at this subject. For me ... something new always clicked when I looked at my vise set-up or holding configuration. Ideas usually led to different set-up ideas ... how to position the vise or vises ... as well as jaw ideas ... material, change-over and others. So we thought it was a good plan to outline some of the newer options available ... and to get your idea machine cranked up.

FIRST - Dump the Knee Mill Vise
We still see a lot of shops using an old style knee mill vise ... or some revised configuration of one ... on their new and modern CNC machine. Ya ... you know the ones ....
If these look all too familiar to you ... the first step in improving your workholding and basically your whole shop floor efficiency is to dump these vises and step up to today. Sure in a pinch ... they are OK ... but you should really think about putting 'em on Ebay and stick some "hobby machinist" ( whatever the hell that is ) with these toys. If you have a CNC machine and want to be a pro ... here are your new alternatives.


Here a just couple of important reasons to dump your 1950's vise for a new CNC vise :
  1. SIZE and SPACE : Without the "wings" sticking our from the sides, these types of vises are slimmer and trimmer ( not to mention lighter ) and will take up less room on your table or fixture plate. That allows for more efficient use of your machine travels and table capacity. 
  2. MULTI PART MACHINING : configurations can include double vise jaws ... again, multiple part machining. The whole concept of efficiency is to perform the most machining while the tool is in the spindle. That may entail multiples of the same part or combining different parts during the tools cycle.
  3. QUICK CLAMP : The ever present annoyance of rapping your fingers while turning the handle to clamp can also easily be eliminated by incorporating a power clamping system such as a pneumatic wrench instead of the handle ... or if you want to "crank it up a notch" ... check out the CHIC video below :

SECOND - Jaws for the Modern World
Now that you have upgraded the vise itself ... it's time to incorporate new holding options into the vise. Almost every shop with a CNC vise uses some sort of aluminum vise jaw that has been machined to accept the stock to be machined. It's a basic ... it's a staple ... if you don't do it it's time to step into the 70's. 

So the most basic step is to create a CNC program that will machine a blank aluminum vise jaw to fit your CNC vise. That way anytime you need some jaws ... call up that proven program and machine some jaws for stock ... or keep some on the shelf. Done.

But hold on ... now there's an even better method. We have talked about these jaws before in Making Chips and we are high on their use and rewards. No cap screws ... 2 min changeover ... and tons of configurations make quick change vise jaws the new go-to vise jaws. Here's a sample video from Carvesmart ... one of our favorites :


THIRD - Don't forget the TABLE
Part 1 in our series dealt with how to bring your VMC machine table into the 21st century. Combining your new table configuration with these new vise and jaw options can really expand your efficiency. This is a really important read ... if you missed that post ... here's the link : 

FOURTH - Don't forget to MOVE THAT VISE !!
Always placing the vise so it looks nice in the middle of the table causes a lot more harm than you might think. Here's a past Making Chips post dealing with that subject in detail ... http://kipware.blogspot.com/2013/01/move-that-vise.html ... required reading if you use a vise ( and seriously, who doesn't ?? ).

RESULT - New Shop Floor Efficiency ... 
with the sky as the limit.
As you can see ... these are some fairly simple but really important changes that will greatly effect your shop floor efficiency. From faster set-up changeovers ... to more advanced configurations ... to faster part load / unload ... to simply better cycletimes ... these tried and proven changes mean more profits ... a happier workforce ... with the sky as the limit. We are also confident that as you implement these changes ... your "machinist" mind will think of even bigger and better changes now able to be implemented with the upgrades that come with the ones outlined here.

Please come back for our next installment in our series on Shop Efficiency.
Until next time ... Happy Chip Making !!

At Kentech Inc. we are MACHINISTS who create Real World Machine Shop Software.
Who creates the machine shop software guiding your shop's future ??
Check out all our REAL WORLD CNC & MACHINE SHOP titles at