Roughing Canned Cycle in Turning - Everything 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.

Happy Chip Making !!

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 !!!

Anatomy of a Cutting Tool

Living in the "real world", chipmakers are living in the labratory conditions where most ideal cutting parameters are achieved. Real world chipmakers are confronted with necessary changes to their cutting conditions that may involve a machine problem, a cutting tool material problem or can be as simple as a change in the cutting tool geometry.

Understanding the terminology and nomenclature of cutting tools is key to the ability to decide and use specific cutting tool geometry for specific applications. Using the proper geometry for specific applications will greatly aide in both tool life and machining sucess.

To understand cutting tool geometry, one must understand the basic cutting tools ... the single point tool used in turning. The effects the related angles have on a single point tool are also basic to understanding to milling cutters, end mills, drills, taps and most other cutting tools. This blog post outlines the important areas of cutting tool geometry as they relate to the single point turning tool and briefly as they relate to other cutting tools.

Cutting Tool Terminology

Shank
The shank is the main body of the tool. If the tool contains inserted cutters, the shank supports the cutter bit.

Face 
The surface against which the chips bear as they are severed.

Nose Radius
This term generally means the rounded tip of the cutting end. This strengthens the cutting edge, improves finish and tool life. Too large a radius increases radial forces and induces chatter. Too small a radius may result in chipping or prevent proper distribution of the heat and thus break down the properties of the cutting tool material.

Chipbreaker
A groove formed in or on the shoulder of the face of the tool for the purpose of breaking up the chip. A chipbreaker of the shoulder type may be formed directly on the tool face or may consist of a separate piece that is held by brazing or clamping.

Rake
A tool is said to have rake when the tool face or surface against which the chips bear as they are severed is inclined for the purpose of either increasing or decreasing the bluntness of the edge. The amount of the rake is measured by two angles called the "back rake" and the "side rake". Rake may be "positive" ( more blunt ) or "negative" ( less blunt ) depending on the inclination angle.

Functions of the Various Angles in Cutting Tool Geometry :

Radial Rake Angle ( Milling ) -- Side Rake Angle ( Single Point Turning Tool )
This angle has a major effect on power efficiency and tool life.

Axial Rake Angle ( Milling ) -- Back Rake Angle ( Single Point Turning Tool )
This angle controls the chip flow and the strength of the cutting edges.

Corner ( Chamfer ) ( Milling ) -- Side Cutting Edge Angle ( Single Point Turning Tool )
This angle reduces the thickness of the chip.

True Rake Angle ( Milling ) ( Single Point Turning Tool )
True rake angle is considered the most significant angle on the cutting tool for metal removing.
The combination of radial rake, axial rake and corner angle determines the shear angle thus power requirements, tool force and temperature at the cut. The higher the positive true rake angle, the lower the cutting force, the power requirements and heat generated at the cut. The rake angle is most often determined by the cutting tool material and the rigidity of the machine tool.

Inclination Angle ( Milling and Turning )
The inclination angle most significantly effects the direction the cutting chip will flow. A posiitive inclination angle directs the chip outward and a negative angle directs the chip toward the center of the cutter. Also, any change in the axial rake angle, radial rake angle or chamfer angle will also change the direction of chip flow.

Dish Angle ( Milling ) -- End Cutting Edge Angle ( Single Point Turning Tool )
This angle provides clearance between the cutter and the finished surface. An angle close to zero does provide strength, but also causes rubbing, generates heat and can thus negatively effect surface finish. Too large an angle weakens the tool. Flats parallel to the finished surface can often be added to the end cutting edge or dish angle to assist in improving the surface finish.

Clearance Angles ( Milling and Single Point Turning Tool )
Primary clearance is directly below the cutting edge and prevents the cutter or tool from rubbing on the workpiece. The secondary clearance is on the tool form of the cutter or the shank of the single point turning tool. This clearance must be large enough to clear the workpiece and permit the chips to escape. Too large of a secondary angle may result in the weakening of the cutter or the tool.

NOTE :
One of the most important variables in machining is rigidity. Rigidity applies to many areas including the set-up and workholding, the machine tool itself, the cutting tool and the workpiece. Even though many other guidelines have been adhered to, where a lack of rigidity exists in any of these areas, a change in cutter geometry, cutting tool material, cutting conditions or a combination of these factors may be required.

Information in this article was taken from Kentech's KipwareEDU® - Mechanical Engineering Version. If you found this information helpful ... we invite you to explore all our versions of KipwareEDU® ... just click here.

Cutting Fluids ... Do you REALLY think about them?

Another major factor to be considered with good Chip Making is the cutting fluids employed. In this post ... we are dedicating some facts and ideas to probably one of the least considered factors in Making Chips.

Cutting fluids typically perform numerous functions simultaneously, including cooling the workpiece and cutting tool, lubricating, minimizing the effects of built-up edge, protecting the workpiece from corrosion, and flushing away chips. The success of cutting fluids is dependant on a combination of interacting parameters, such as cutting fluid formulation, workpiece material, tool material and tool geometry, surrounding atmosphere and cutting speed. Machine design is also of increasing importance.

Cooling Mechanism

Two requirements must be met in order for a cutting fluid to function effectively as a coolant . The fluid must gain access to the course of heat, and the fluid must have the capability of removing the heat.

Lubricating Mechanism

High pressures and temperatures in most cutting operations make it impossible for a cutting fluid to sustain a complete liquid film between the cutting tool and workpiece material. Instead, the conditions in a typical metalcutting operation favor the use of the fluid primarily as a boundary lubricant. In boundary lubrication, additives in the fluid react chemically with the workpiece material and tool material to form compounds on the metal surfaces. One theory suggest that lubrication in cutting occurs by a reduction in severity of shear strain at the cutting tool. Two schools of thought exist to support this theory. First, the lubricant absorbs into the chip surface and restricts the adhesion of chip material to the tool. Second, the reactive components of the fluid combine chemically with the freshly generated metal surface of the chip to produce a film which has a lower shear strength than that of the chip material, thus reducing friction, cutting forces, and temperature.

Corrosion Protection Mechanism

Corrosion protection of the machine tool and workpiece is important when machining operations employ the use of a cutting fluid. Some lubrication charecteristics to consider when looking at the composition of cutting fluids :

Soda Ash -- increases the alkalinity of the fluid and reduced the tendency to cause rust.

Mineral Oils -- provide a major deterrent to rust formation using an ability to coat the surfaces of the machine tool and workpiece to form a physical barrier to prevent chemical reaction from taking place.

Chip Removal Mechanism

In machining operations that generate large amounts of metal chips, an important function of a cutting fluid is to flush chips away from the cutting zones. The flushing action removes the chips from the cutting zone and keeps them from scratching the machined surfaces. This action is especially useful in deep-hole drilling, trepanning, and gundrilling operations, in which fluid is used to force the chips out of the hole. One major consideration in these applications is the pressure under which the fluid is supplied to the cut. However, with these applications can come excessive foam generation which can weaken the effects of the cutting fluid. Proper selection of cutting fluid is important to avoid this condition which can interrupt the machining and cutting fluid filtering process.

Information in this article was taken from Kentech's KipwareEDU® - Mechanical Engineering Version. If you found this information helpful ... we invite you to explore all our versions of KipwareEDU® ... just click here.

Let's Talk Chips

Well ... it's the name we have chosen for the blog ... so let's start the talk with that subject. I would like to devote this first article to the highlighting of some of the key points about chips ... what they mean ... how they are made ... because a deep understanding of these points is essential to good chip making.

Lets start with the Types of Chips :

• Discontinuous Chips : Discontinuous chips are small broken chips and may form when cutting at low speeds or when cutting a material containing points of stress concentration, such as cast iron that contains graphite flakes or free-machining steel. These chips are a series of chip segments that have broken at areas of stress concentrations in the workpiece material.
• Continuous Chips : At speeds at which the temperature at the chip / tool interface is relatively low, the chip being created can split and a portion of the chip is left behind. This portion of the chip attaches itself to the to the face of the cutting tool and is commonly referred to as the "built up edge" or BUE. This left-over material then acts as a cutting edge and will usually continue to grow until it reaches a size where it then passes off with the chip. This process repeats itself many times during the cutting process producing a variety of continuous chips. This process is a major factor in surface finish since the BUE varies in size and depth and effects the depth of cut at the cutting tool edge and thus the surface finish produced during removal.
• Seconday Shear in Chipmaking : As the metal is being removed and the chip created, the chip rides up the face of the cutting tool. When the sticking stress of the chip on the cutting tool face equals the stress of the chip removal at the material, additional stress is transformed internally into the chip being created. This is commonly referred to as secondary shear. Since secondary shear is due to high stress on the tool face, it is always accompanied by an increase in cutting forces. The remedy for secondary shear is normally an increase in the shear angle of the cutting tool.

General Considerations in Chipmaking

• Chipbreakers : Chipbreakers are often added to the face of a cutting tool to insure that the chip is broken periodically. The distance the chipbreaker is away from the cutting edge and the style of chipbreaker determine the length of the chip produced and the frequency of those breaks. Chipbreakers can be seperate from the cutting tool or insert or built directly into the tool or insert.
• Chip Color : Contrary to popular belief, the color of the chip is not a direct reference to the heat of the chip or the heat present at the time the chip was produced. Rather, the color of the chip is a reflection of the oxide coating of the chip and only a minor reflection of the cutting temperature involved in the creation of the chip. The amount of oxide coating can be effected by the use or non-use of coolant ( more oxygen is present at the cut ), feedrate ( chips produced under a high feedrate remain hot longer ), as well as the materials ability to oxidize. 
• Cutting Forces : 
• Cutting forces are less with discontinuous chips than with continuous chips.
• A built-up edge may decrease or increase cutting forces
• The greater the secondary shear zone on the face of the tool the greater the cutting forces.
• Cutting forces are decreased by reducing the chip thickness.
• Surface Finish : 
• The main components that effect surface finish are built-up edge, feed marks caused by a secondary cutting edge (BUE) and tool instability or chatter. 
• Feed marks are often eliminated by a reduction in feedrate and an increase in the tool nose radius of the tool.
• BUE can often be reduced by increasing the cutting speed, reducing the tool face friction or through the use of coolant containing free machining additives. 
• Chip Control : 
• Long, unbroken chip are a danger both to the operator and to the workpiece.
• Broken chips allow for easier removal from the machine both in terms of maintenance and in cutting.
• Chipbreakers should be employed where necessary to force the breaking of chips.

So there you have it ... what I consider some of the essentials of Making Chips ... I hope you will find these ideas helpful and informative.

Information in this article was taken from Kentech's KipwareEDU® - Mechanical Engineering Version. If you found this information helpful ... we invite you to explore all our versions of KipwareEDU® in more detail ... just click here.

Start Me Up

It's November 5,2012 and we are starting a new BLOG that will include news, tips and tricks pertaining to CNC machining ... chipmaking ... and manufacturing and metalworking in general.

Based on our 25+ years in metalworking industries ... we now create Real World Machine Shop Software applications marketed under our Kipware® trademark. Our applications include business software ... quoting and estimating ... and conversational CNC programming software for milling and turning ... our pioneering G code conversion software ... and CNC programming training & reference titles.

Please visit our website ... www.KentechInc.com ... and check them out !!!

If CNC ... CNC programming ... metalworking ... and manufacturing in general is your cup of tea ... please visit us here often and hopefully we will provide some CHIP MAKING stimuli !!

See ya soon !!