I am working on a new article and am looking for success stories about the success of women  as CNC machinists, operators, programmers, supervisors.

If you have a good story or comments on the subject, comment on this post- I will review for content and if applicable use anecdotally within the article.

Suitable posts will be approved for posting on this blog “as is.”

Of interest are things like:

1. How did you get into the trade
2. do you like it
3. Do you feel your pay and treatment are consistent with male colleagues
4. would you recommend the trade to other women
5. what were your barriers to entering the business of CNC
6. what training do you feel women should seek to succeed
7. success stories (what did you overcome, achieve, etc)

To be a good NC/CNC programmer you must understand how the radius of a tool affects your programming points.  The radius may be on the end of a lathe tool or the radius of a milling cutter.

The following is excerpted from the FAQ section of 7 Easy Steps to CNC Programming: Book II, Beyond the Beginning.

CNC Tool Nose Radius

Lathe tools rarely have a perfectly sharp corner at the tool nose.  As a result, when you program lathes, it is important to compensate for the tool nose radius.
 
As you look at the tool nose radius example below, imagine these two situations.  Assume you are using a tool with a .031 nose radius.  As you cut down the face of the part, if you stop at X0, the tool, the actual cut will be .031 above the center of the part, leaving a .062 nub at the center of the part.  Then if you want to drill a hole in the center of the part, the drill walks off center because of the nub.

 

In another situation, assume you are using the same tool to cut a profile.  If the program does not compensate for the tool nose radius the part will be cut under / over size.  
 
The solution is to program the desired tool path relative to the center of the cutter.  This is true for lathes as well as mills. 
 
When programming a lathe, use the center of the tool nose radius.  This is particularly important when manually programming machines.  If you are generating G-code using a Computer Aided Manufacturing (CAM) system this is less critical.
 
Programming to the center of the cutter is essential for correctly applying the math to generate accurate machine control data.
 

 Fig. 13  (from 7 Easy Steps to CNC Programming: Book II, Beyond the Beginning) above shows how a 1.00” cutter must be programmed so that there is 5” between parallel cuts if you need the part 4” wide. 
 
Examine the previous Tool Nose Radius example. Notice that if you program using the center of the tool nose radius, programming an X0 will move the tool so that its center stops at the center of the part.  That’s the good news.  The bad news is that the tool would then cut with the center of the tool on the profile, thus making the part too small.
 
You must compensate the tool path for the tool nose radius by adding the tool nose radius to the part diameter.  For example assume the following: 

• The the small diameter of the finished part is 1.000
• The Tool Nose Radius is .031
• The machine is programmed in the radius mode
• The program is written for the center of the tool nose radius

In this case, the center of part would be programmed as X.0 Z.031. The X dimension to turn the diameter would be X.531. 
 
Many lathes let you enter diameters instead of radii.  In this case, the center of part would be programmed as X.0 Z.031. The X dimension to turn the diameter would be X1.062, the diametrical result of changing the cutting radius by .031.
 
So, when facing to the center of a work piece with a .031” radius tool, you can actually program the cutter to go to X0

Note:  The above descriptions are “old school” in that most machines on the shop floor today have offsets for tool nose radius.  Using offsets allows you to program right to the dimensions of the part.  But goodCNC programmers know that, just because the machine can do something, does not excuse them for knowing how it works or how to do it manually.

 

Canned Cycles used in NC programming are great time savers, but often don’t do exactly what we want them to.

Gopal posted a great question today about the limitations of the G83 canned cycle.  Here is what he had to say after reading Proven Tips and Tactics: Understanding Canned Cycles.

[ I need to drill 200 holes of Diameter 4.0mm to a depth of 50mm (Z-50.0) and then continue Diameter 3.0mm to a depth of 110.0mm (Z-110.0).

There is no problem for drilling Dia 4.0 upto Z-50.0 wirh a G83 code. But the Diameter 3.0mm hole, I want to go rapid upto Z-50.0 (because already drilled Dia 4.0 upto this depth) and then peck 2mm and clear the chip at Z3.0 and continue 2mm peck and clear chips at Z3.0 until Z-110. reaches. Is there any way I can do this in Fanuc or Sinumerik? If I give the R value 3.0, The drilling cycle starts from Z3 and lot of time wastage. If I give the R value -50.0, The chip is clearing at z-50 and not Z3. Any solution for this? ] – Gopal

    That is an interesting situation and one that can be solved, not with canned cycles, but with sub programming.

Sub programming techniques allow us to creat our own CNC canned cycles.  While they may take a little effort to create in the beginning, once created they can be use over and over. 

So what are CNC sub programs and how do you use them?

Sub-program are similar to any other NC / CNC program except they are usually more simple.  Generally, sub-programs will only be a series of moves or positions.

The significant difference in a sub-program is that the end code will be an M99.  The M99 commands the control to return to program from which the sub-program was called.

When you want to call up a sub-program, use the command M98P(xxxx).  M98 commands the control to leave the current program and complete the instructions in the sub program specified by the P-code.

THE FOLLOWING IS A DIAGRAM OF THE SUB-PROGRAM PROCESS

From 7 Easy Steps to CNC Programming P.48

To interpret this diagram start at the beginning.  As you read down you see at line n30 the program calls, with an M98, the sub program 80.  Moving through program 80 at line n15 the sub-program 85 is called.  Program 85 runs down to the M99 which returns control to program 80.  Program 80 continues processing until it reaches its M99 command.  This M99 returns control to the main program. 

From here the main program continues until it gets to line n70 where the control is once again passed to programs 80 and 85.  After programs 80 and 85 finish their processing the control is returned to the main program which continues until it reaches the end of the program at the M30.

You see from the example above, CNC controls allow sub programs to be nested.   This can be very useful too.

So how could we use CNC sub programming to address Gopal’s Question?

Starting the main program, it could be structured something like this?

MAIN CNC PROGRAM   750

NOTE: THIS CODE IS FOR REFERENCE ONLY!  IT HAS NOT BEEN TESTED FOR ERRORS

O750 (main program)
N005 (these are the )
N010 (typical start up)
N015 (blocks you normally)
N020 (to prepare the machine)
N025 G0 X  Y (position to first hole)
N030 G43/G44 Z3.0 (rapid to Z using your offset mode)
N035 M98 P751 (call sub program 751)
N040 G0 X Y (move to new position)
N045 M98 P751 (call sub program 751 again)
N050 G0 X Y (repeat until all holes complete)
N055 ……..
N060 ………
N065 G0 G28 G91 Z0 M9 (safely return to Z home)
N070 G28 X0 Y0 M5 (return to tool change position)
N075 M0 M1 / M30 / M2 – (however you want to terminate the process)

Notice this Main CNC program only sets the machine in motion and moves to the location of the first hole.  The main program does not do any drilling in this example.  The actual drilling will be accomplished by the sub program shown below.  

It’s a little long, but in a few lines you will see the pattern of what the CNC sub program doing.   After the first few lines, you will see that the only change is in the drilling depth of each pass.

CNC SUB PROGRAM 751  

NOTE: THIS CODE IS FOR REFERENCE ONLY!  IT HAS NOT BEEN TESTED FOR ERRORS

O751 (sub program to do drilling)
Z-50. (rapids to Z-50.0 to save time)
G1 Z-52.0 Fxxx  (Drills to depth at desired feed rate)
G0 Z3.0  (rapids to Z3.0 to clear chips)
Z-50.0  (rapids to Z-50.0 to save time)
G1 Z-54.0
G0 Z3.0
Z-50.0
G1 Z-56.0
G0 Z3.0
Z-50.0
G1 Z-58.0
G0 Z3.0
Z-50.0
G1 Z-60.0
G0 Z3.0
Z-50.0
G1 Z-62.0
G0 Z3.0
Z-50.0
G1 Z-64.0
G0 Z3.0
Z-50.0
G1 Z-66.0
G0 Z3.0

NOTE: THIS CODE IS FOR REFERENCE ONLY!  IT HAS NOT BEEN TESTED FOR ERRORS
Z-50.0
G1 Z-68.0
G0 Z3.0
Z-50.0
G1 Z-70.0
G0 Z3.0
Z-50.0
G1 Z-72.0
G0 Z3.0
Z-50.0
G1 Z-74.0
G0 Z3.0
Z-50.0
G1 Z-76.0
G0 Z3.0
Z-50.0
G1 Z-78.0
G0 Z3.0
Z-50.0
G1 Z-78.0
G0 Z3.0
Z-50.0
G1 Z-80.0
G0 Z3.0
Z-50.0
G1 Z-82.0
G0 Z3.0
Z-50.0
G1 Z-84.0
G0 Z3.0
Z-50.0
G1 Z-86.0
G0 Z3.0
Z-50.0
G1 Z-88.0
G0 Z3.0
Z-50.0
G1 Z-90.0
G0 Z3.0
Z-50.0
G1 Z-92.0
G0 Z3.0
Z-50.0
G1 Z-94.0
G0 Z3.0
Z-50.0
G1 Z-96.0
G0 Z3.0
Z-50.0
G1 Z-98.0
G0 Z3.0
Z-50.0
G1 Z-100.0
G0 Z3.0
Z-50.0
G1 Z-102.0
G0 Z3.0
Z-50.0
G1 Z-104.0
G0 Z3.0
Z-50.0
G1 Z-106.0
G0 Z3.0
Z-50.0
G1 Z-108.0
G0 Z3.0
Z-50.0
G1 Z-110.0
G0 Z3.0
M99 (retuns control to the main program where it left off)

 The CNC sub program may look a little intimidating to write but it wasn’t.  Once I had the structure correct for the first few lines, I cut-n-paste the rest of the program.   All I had to do after that was to edit the lines for the drilling depth.  All other lines stayed the same.

So How is the CNC sub program reusable like canned cycles?

If your CNC control is capable of sub programming, and most controls are these days, any NC program can call any available sub program.  So, in this case, any program that has the line
    M98 P751
will call this exact sub program.

But wait, isn’t this useful only if I want to drill these exact holes in some other part?

Yes and no.  That is true if you don’t edit the code.   But once you have made a template for a sub program, you can reuse the structure but change the start, stop, clearance points and so on.  Once you have made the new sub program simply save it as a different number.

A good strategy is to reserve a set of numbers for your sub programs.   For example, you might store all your sub programs in the 5000 series of numbers.  Your first sub program would be 5000, the next 5001 and so on.

You can even get more creative with your numbering.   Sub programs 5000-5099 could be drilling sub programs.   Sub programs 5100-5199 could be sub programs to mill pockets.  Sub programs 5200-5299 could be sub programs for some other repetitive features, and so on.

Sub programs are not just for drilling.

You probably realized from the creative numbering examples above, that sub programs are not limited to drilling routines.   Sub programs can be used for any feature or shape, or for changing pallets, indexing table, or whatever.   Any repetitive CNC commands you do can be put in a sub program.

Great question Gopal, thanks for asking.

After reading the previous article on the importance of feedrates,  DAVE DAVIDSON (SOCIETY OF MANUFACTURING ENGINEERS, Co-Chair:MMR Tech Comm | Advisor: DESC Deburring/Surface Conditioning Tech Group)  provided a  link to a very informative article published by SME – Check it out.

http://dryfinish.wordpress.com/2011/07/14/microfinishing-and-surface-textures/

http://dryfinish.wordpress.com/2011/07/28/microfinishing-and-surface-textures-part-2/

One of the most important calculations you need to understand as a machinist or CNC programmer is the feedrate calculation.

Why are feedrate calculations so important?

Feedrate, the speed at which the cutting tool engages the part, is directly related to safety, productivity, tool life, surface finish, part quality and so on.  Let’s look at these individually.

• Safety - Feedrates determine cutting forces.  The faster you attempt to remove the material the greater the cutting forces.   So, the faster you cut the part, the more rigid you set up needs to be.  Anyone who has ever been around a machine when a cutting tool crashed into a part at rapid travel knows the damage that can be cause by excessive feedrates.
   
  Also, combined with tool geometry, the feedrate you use affects the chips that are made during the cutting process.   If the feedrate is too slow the cut material will not break into small chips and will create long stringers that whip around the spindle.   Stringers are very dangerous and can severely cut people, remove limbs, and so on.
    
• Productivity- obviously for production machining you want to cut the part as fast as possible without endangering people or machines or diminishing the quality of the part.  Some may disagree, but the fact is few things cost more spindle time.  
     
  For round numbers imagine you borrowed$100,000 for a machine at 10% interest. Just the interest on the machine is costing you $1.60 per hour.   If you only run the machine 1 shift per day, the cost is really $4.80 per hour. . . just to pay the interest.   Now if you want a 5 year pay back on the machine, that adds another $9.60 to the cost.
    
  To break even on the $100,000 machine loan at 10% interest, that machine needs to earn $14.42 per hour or about a quarter per minute.   And that does not even include wages, benefits, profit, G&A, marketing etc.Are you starting to get the picture.
   
• Tool Life - But what about tool life you ask?  Don’t aggressive feedrates reduce tool life? They can and the tooling cost is a consideration, but compared to inefficient spindle time, the cost is minor.
    
  The faster you cut the more pressure you put on the tool cutting edges and those forces tend to wear the tool more.   By the same token, cutting some materials too slow will work harden the material in front of the tool causing very rapid tool wear because of having to cut hard material.
    
• Surface Finish - Surface finish is directly related to feedrate and tool geometry.  Cut too fast with a tool nose radius that is too small and you will get a course finish.  A perfect example is threading on a lathe.   The tool is moving very fast in relationship to the spindle speed.   A face mill moving too fast in relation to spindle speed tends to leave a grooved pattern.
      
  Surface finish is also directly related to cost.   If the customer requirement allows for a 125 finish and your cutting process is giving them a 32 or 60 finish, you may be cutting too slow, wasting machine time, and increasing your cost of production.
    
• Part Quality - Customers don’t usually want low quality parts.  But what does that mean?  If a customer requirement is for a 125 surface finish, is a part with a 32 finish higher quality?  Print tolerances and surface finishes, when stated correctly, give the customer exactly what they need at the best possible price.   If the requirement is for a 125 finish, the customer is saying they don’t want to pay for the additional cost to achieve a 32 finish.  Now they may prefer a 32 finish, they just don’t really need it or want to pay extra to get it.
    
  So cut as aggressively as you can to meet the requirement and charge accordingly.   That means, if you are giving the customer a 125 finish, they should be paying less money they would to a vendor giving them a 32 finish.   If the 32 finish is that important to the customer, they need to update their requirements.
    
  The cutting forces associated with machining can also distort parts or introduce residual stresses.  So cutting too aggressively may distort the part in such a way that it diminishes overall quality.  It may take some trial and error finding the optimum feedrate.

Whoa you say, there is a lot more to it that feedrates!

You are correct.  Feedrates are only one variable in a fairly complex process.  All of the following come into play when machining a part.

• Cutting speed
• Feedrate
• Depth of Cut
• Machinability of the material (i.e. less machinable = more difficult to cut)
• Rigidity of the set up
• Rigidity of the machine
• Horsepower of the spindle
• Geometry of the cutting tool

All of these variables affect the efficiency of the machining process and quality of the part.  But for this article the focus is limited to feedrates.  But there is a way to think about it to help keep it straight in your mind.  I promise after this section, I will show how to do the feedrate calculations but you need to have the right mindset so keep you safe and productive.

When you think of productivity, think of Cubic Inches of Material Removal Per Minute  Let’s call this the Material Removal Rate or MRR. 

• MRR is a function of Depth of Cut, Feedrate and Cutting (spindle) speed.
• The greater the MRR, the greater the cutting forces.
• The less machinable the material the greater the cutting forces
• The greater the cutting forces, the greater the requirement for horsepower and rigidity.
• Tool geometry affects cutting forces. 
• Positive cutting geometry tends to reduce cutting forces but the tool is weaker and often chip control is sacrificed. 
• Negative cutting geometry typically increases cutting forces but has the benefit of stronger tools and better chip control.
• Material properties and finish requirements often define the optimum tool geometry for the process.

How feedrates are calculated.

G95 Cutting in units per revolution

The simplest feedrate calculation is the G95 or feed per revolution (IPR) used mostly for lathe machining. 

FORMULA: Desired chip load * number of cutting edges

There really is not much calculation to do because you typically have one cutting tip cutting so if you want .030 chip load that equates to .030 feed per revolution of the spindle your program would include a G95 to set the cutting mode to IPR.  Then on the cutting line, you would have an F.03

EXAMPLE:  G00 G80 G95       . . . start-up block to set modal conditions
                         X### Z###              . . . positioning move to X, Z start of cut on a lathe
                        G01 Z-1.250 F.03   . . . cut Z-1.25 inches at .03 inches per revolution

NOTE:  if you are programming in Metric Mode, you would use mm/minute.  For example, your feedrate would be F1.5 to feed 1.5 milimeters per minute.

EXAMPLE:  G00 G80 G95     . . . start-up block to set modal conditions
                         X### Z###            . . . positioning move to X, Z start of cut on a lathe
                        G01 Z-125.0 F1.5  . . . cut Z-125.0 mm at 1.5 mm per revolution

Suppose you are drilling though.  In this case you have 2 cutting tips so to maintain a .030 chip load, you would program G95 with a feedrate of F.060

EXAMPLE:  G00 G80 G95     . . . start-up block to set modal conditions
                         X### Z###            . . . positioning move to X, Z start of cut on a lathe
                        G01 Z-1.250 F.06 . . . drill Z-1.25 inches deep at .06 IPR  (.03 per cutting edge)

G94 – Cutting using units per minute instead of units per revolution

For mills, routers, drilling machines and some older machines, the typical feed rate is expressed in units per minute.  In other words, a feedrate might be 10 inches per minute or 250 mm per minute.  This can be a little confusing because, what we are interested in is our actual chip load.

FORMULA: Desired chip load * number of cutting edges * RPM

Lathe Example:  .015 chip load * 500 RPM * 1 cutting edge = 7.5 IPM
                        G00 G80 G94         . . . start-up block to set modal conditions
                         G97 S500               . . . set spindle in direct spindle speed mode and RPM at 500
                         X### Z###            . . . positioning move to X, Z start of cut on a lathe
                        G01 Z-1.250 F7.5 . . . cut Z-1.25 inches at 7.5 IPM to achieve .015 chip load

Lathe Drilling Example:  .015 chip load * 500 RPM * 2 cutting edges = 15.0 IPM
                        G00 G80 G94            . . . start-up block to set modal conditions
                         G97 S500                  . . . Set Spindle in direct spindle speed mode and RPM at 500
                         X### Z###               . . . Positioning move to X, Z start of cut on a lathe
                        G01 Z-1.250 F15.0  . . . Cut Z-1.25 inches at 15.0 IPM to achieve .015 chip load/edge

Milling Example:  .005 chip load * 2000 RPM * 4 cutting edges = 40.0 IPM
                         G00 G80 G94            . . . start-up block to set modal conditions
                         G97 S2000                . . . Set Spindle in direct spindle speed mode and RPM at 500
                         X### Y###               . . . Positioning move to X, Y start of cut on a lathe
                         Z-###                          . . .  Positions end mill to proper depth to begin cut
                        G01 X2.5 F40.0        . . . Cut along X axis for 2.5 inches at 40 IPM to achieve .002 chip
                                                                         load per edge

Again, if programming in metric mode, units would be changed to millimeters.

G93 is the code for Inverse Time feed rates and is beyond the scope of this article but for a good discussion on the subject check out this article on Eng-Tips forum  http://www.eng-tips.com/viewthread.cfm?qid=200454&page=7

Recently a reader asked a great question about how to calculate speeds and feeds. 

Speeds and feeds are at the heart of all machining. Learning the CNC codes or using a conversational control can be achieved in a relatively short period of time. Selecting the right speeds and feeds is almost as much art as it is science.

 In this article, I will be discussing how to calculate cutting speeds, but before we get into details, here are a few things to keep in mind. (at the bottom are calculations for speeds and feeds)

1. Safety – always an important consideration – don’t jeopardize your or another operators safety for the sake of speed.
    
2. Rigidity – if your setup is not rigid, you can toss a part or tool out of the machine, experience excessive chatter, fail to achieve acceptable surface finish, fail to maintain dimensions and so on.
    
3. Machinability – all materials have unique machinability characteristics. You’ve no doubt observed aluminum machines easier than steel.
    
4. Cutting Toom Material - high speed steel, carbide, ceramic, etc.
    
5. Available Horsepower – Machinability determines the horsepower requirements to cut the material. If you don’t have the horsepower, you will have to lighten your cuts to avoid stalling the spindle.
    
6. Tool geometry- Tools that have positive cutting geometry cut more freely than do tools with negative geometry, but are limited in the amount of shock and interrupted cuts they can take. Some materials cut much better with negative geometry, others with neutral or positive geometry.
    
7. Heat – machining creates a lot of heat and it is going to go into the tool, the material, the chips that are removed and so on.  Too much heat will quickly break down your tool. Too much heat can cause the material to expand and make it difficult to control part size.
    
8. Chip control – your ability to control the chips made during the machining process is an indication of having chosen the correct speeds, feeds and tool geometry.
    
9. Surface Finish – there is a direct relationship between cutting feeds and tool radius to surface finish.

All of the above factors (and many more) affect or are directly affected by speeds and feeds.

With respect to machinability, there are numerous websites that outline the machinability of various materials. Many tool manufacturing websites like Kennametal.com have great resources for determining the optimum cutting speeds and feeds for their tools and a wide variety of materials.

Cutting speed, in the US, is generally expressed in terms of Surface Feet Per Minute often expressed as (SFM) or (SFPM). SFM is the speed at which tool tip is cutting through the material. Imagine you are dragging a stick behind a car that is traveling at 60 miles per hour. In one minute your stick has traveled 5,280 feet across the ground. That would be expressed as 5,280 SFM.

Unless you are running a shaper or other linear cutting machine, your surface feet per minute is based upon the rotational speed of either the part or the cutting tool. Obviously, on a lathe it is the chuck speed that matters. On a milling machine it is the spindle speed that matters.

The other major factor in calculating SFM is the diameter of the diameter you are cutting on a lathe or the diameter of the tool you are using on the milling machine. So here are the steps to calculating SFM.

For SFM / RPM calculations you need to know the following:

D = the diameter of the milling tool or the diameter you are cutting on a lathe
Pi / π = 3.1416 (approximately but close enough)
SFM = The surface feet per minute you want to use for a cutting speed
RPM = The RPM required to achieve the desired SFM based on the diameter of the tool/part
K = Constant use for SFM calculations (3.8197)
    = 1 / [(D*π) /12]
    = 1/( 3.1416 /12)
     = 3.8197

RPM Calculations when you know the SFM you want to achieve.

RPM = SFM * 3.8197
                            D
Example: You are cutting a 2.5 diameter on a part (or using a 2.5 dia milling cutter)

• Material is free machining steel
• Cutting tool is coated carbide
• Carbide manufacturer recommends 500 SFM

Your cutting RPM would be:
             = (500 * 3.8197) / 2.5= 1909.85 / 2.5
             = 763.94
             = 764 RPM (rounded to the nearest RPM

SFM calculations when you know the tool diameter and RPM

But what do you do if you know the diameter of the part or cutter diameter and the RPM but you need to know the SFM so you can verify if it is appropriate.

              SFM = RPM * Diameter
                                    3.8197

Example:

• You know the milling cutter is 6” in diameter
• You know the RPM is 1000
• You need to know is the SFM appropriate for cutting aluminum

          SFM= (1000 * 6) / 3.8197
                   = 6000 / 3.8197
                   = 1570.80

Since cutting speeds for aluminum using carbide can range from 800-2000 SFM  1570.8 SFM  may or may not be a good speed. It will depend on all the factors listed at the beginning.

Watch my next article that will discuss how to calculate feed rates for mills, drills and lathes.

Now how would you like to work for them.

I don’t usually do job postings, mainly because companies don’t send them to me, but this case is different.  Not only have I heard about Acero Precision, I have spoken with them and written about them.   Acero is on the leading edge of what manufacturing can and should be.

If you are into manufacturing, CNC programming, and/or Machining you might want to check out their job postings.  If you have the right attitude and skills there may be a great job opportunity for you.

http://acero.submit4jobs.com/

Tell them Dave sent you.

Opportunities and Job Satisfaction: Why a Career in Manufacturing Demands a Second Look.

A joint Study by The National Association of Manufacturers and Deloitte & Touche 1 estimated that the mass retirement of baby boom generation workers will create a need for 10 million skilled employees between 2012 and 2020. Faced with a lack of qualified job applicants, Manufacturer’s are losing their ability to maintain production levels. With the strong demand for Machinists, Engineers and Craft Workers, why is it so hard to recruit new talent?
. . . To read my entire article published in the December 2010 issue of Manufacturing Engineering Magazine . . . click link –>  Acero Work Force Article Scan

I’ve been so busy lately, but not too busy to pass along this great machining resource from Thomas NET

http://www.thomasnet.com/articles/custom-manufacturing-fabricating/machinist-machining-resources

The Problem with Counter Boring

When creating a counter bore, if the tool retracts too quickly, it may leave a step or uneven finish at the bottom of the counter bore. The CNC programming G code to address this issue is G82. This simple CNC canned cycle bores the hole to depth at the desired feedrate and allows you to specify a dwell time for the tool pause at the bottom. This insures a good clean face at the bottom.

 

CNC Code Data

Code: G82
Modal: Yes
Group: 01
Action: Boring / Counter Boring
ANSI Std: Yes
Requirements: Point to move to(X,Y), Feed Rate at which to move (F), Dwell Time (P), Final Depth (Z)
Options: R (rapid return plane, Feed rate, G98 / G99 Rapid plane selection, G17/G18/G19, P time in milliseconds to dwell
Conflicting G Codes G00, G02, G03, G04, G80 All Canned Cycles, Any other G code in Groups 00, 01 or 09 

Description and How to Use G82

The G82 is the NC command that tells the machine to: 

• Move to an X,Y location
• Rapid to a clearance Plane (R Plane)
• Feed into the bottom of a hole or counter bore at feedrate specified by the F parameter
• Dwell at the bottom of the hole for the amount of time specified by the P parameter
• After dwelling at the final depth, retract to the reference plane above the part
• Move to the next hole and start the process all over again.

Here is a side by side comparison to counter bore 2 holes 1″ deep, with a dwell at the bottom for 1 second ( hole to be drilled at X0, Y0) at 2 IPM 

With G82…………………………………………Without G82
G00 G90 X0 Y0 …………………………………………G00 G90 X0 Y0
Z.1 ………………………………………………………………….Z.1
G82 Z-1.0 P1000 F2.0……………………………G01 Z-1.0 F2.0
X1.0 Y0.0 (drill new hole)………………………..G04 X1 (or G04 P1000)
…………………………………………………………………………X1. Y0 (move to new location to start this all over again) 

Calculating Dwell Time

The P parameter in the G82 command is time in milliseconds so P1000 = 1 second, P500 = 1/2 second and so on. To calculate the correct amount of dwell time use this formula:
P = Dwell Time
DR= Desired revolutions of tool at bottom of hole
RPM = Revolutions per minute of tool 

P = DR / (RPM/60) * 1000 

For Example: You want your tool to dwell for 2 revolutions. With spindle speed is 500 RPM you would program P240 as shown below: 

P = 2 / (500 / 60) * 1000
P = 2 / (8.3333) *1000
P = .24000 * 1000
P = 240 

REMEMBER: Only dwell the tool for the minimum amount of time necessary to insure a good clean counter bore face. Dwelling too long will only dull your tool and possibly work harden the piece. Not to mention that long dwell times increase production times. 

Benefit – simplicity and time-saving
While this canned cycle doesn’t save as much programming time or NC code as other canned cycles, it is still very simple to use and edit. Like all CNC programming canned cycles any of the parameters can be changed in the middle of the cycle to adjust feedrates, depths, dwell time, clearance planes and so on. 

There are many canned drilling cycles you can use to save time. Look for future articles to learn more about these labor-saving commands. 

---

For a complete introduction to the fundamentals of CNC programming, take a look at 7 Easy Steps to CNC Programming . . . A Beginner’s Guide or 7 Easy Steps to CNC Programming . . . A Beginner’s Guide, the Ebook