Category Archives: Machinist Tips and Tricks

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

Cutter Compensation – A Programmers Best Friend

In this post … we would like to touch on some of the points regarding cutter compensation … when turning angles and radii … on Fanuc based CNC controls.

Many programmers shy away from cutter compensation … primarily because they have never taken the time to fully understand both it’s power nor how to use it properly. But the reality is that cutter comp is one of a programmers best friends. The most common reason goes something like this “It’s just as easy to have the CAD/CAM system compensate for the TNR ( tool nose radius ) and out put the hard numbers.” That is true … but life on the shop floor makes this a bad practice. A couple of reasons why :

  1. The “numbers” in the G code don’t match the “numbers” on the part … because they are taking into account the TNR. If manual edits need to be made … even simple edits … this makes it much harder because the part dimensions don’t match the G code numbers.
  2. Say after cutting … the conditions warrant either a bigger or smaller TNR for better cutting conditions. If cutter comp is used … it’s a simple offset change. If not … it’s a trudge back to the CAD/CAM guy or system to re-post and make a new G code program for the revised tool and it’s TNR.
  3. In milling … let’s say I broke my last perfect .250R end mill … but I have a re-ground one that is .245R.. Again, if cutter comp is used … it’s a simple offset change. If not … it’s another trudge back to the CAD/CAM guy or system to re-post and make a new G code program for the revised tool radius.

Conversational

But here we are going to stick with turning here … and here are a couple of simple rules for when to use and when not to use cutter compensation.

  • Whenever angles or radii are involved … you must use TNR compensation or the angles and radii will be off. Because the programmed point of the cutting tool, an imaginary sharp point, does not coincide with the actual point of the cutting tool which always has some corner radius. For this reason, when machining close tolerance angle or radius cuts, inaccurate workpieces will be produced. The amount of error is proportional to the amount of the tool nose radius.
  • Only worry about using it for finishing … It’s really not worth the effort to use it roughing … the amount you leave for finish allowance will probably “hide” the mismatch due to the TNR.
  • You must start cutter comp with a “start up block”. This block is usually the move as you approach the part … the move distance must be greater than the radius in the TNR offset. So if your tool has a radius of .032 … make a move at least .035 … preferably more.
  • Make sure that your TNR is less than any radius on the part … don’t try to jam an .032 tool into a .020 radius … alarms will greet you somewhere along the way.
  • We’ll cover some additional thoughts at the end of the post.

The Details :

The CNC control has the capability to automatically compensate for the tool nose radius thru the CUTTER COMPENSATION codes of G41 and G42. G41 is called cutter compensation left. The left side is explained as the side of the workpiece the cutting tool is on when viewed in the direction of cutter movement or the cutter is moving on the left side of the programmed path. Once commanded, G41 or G42 are modal commands and remain active until the G40 or cancel condition is obtained.

In Fanuc controls, in addition to commanding G41 or G42 direction, the programmer must also tell the control two other aspects of the cutting tool which are : (a) the amount of the tool nose radius and (b) the imaginary tool tip location. Both these values are entered in the tools geometry or wear offset table. In the offset table, the R value is the amount of the tools nose radius. If the program called T0101 in the tool command, in offset table #1, under the R column, the nose radius of the tool would be entered. The T column in the offset tables holds the imaginary tool tip location.

Cutter compensation must be programmed using what is commonly referred to as a start up block. This block, which must be a G01 type block, is used to activate the cutter compensation before the cutting tool actual contacts the workpiece. The movement amount in the start up block must always be greater than the nose radius of the tool stored in the R column of the offset table. Circular commands using G02 or G03 are not allowed on start up blocks.

G40 is used to cancel the automatic compensation of the tool nose radius. G40 should always be commanded on a G00 block as the tool moves away from the workpiece with the tool in a clearance position.

More Rules and Thoughts :

Many rules apply in the use of cutter compensation as the control is always checking the tool position so it can calculate for the tool nose radius. Three rules of thumb apply and should keep you free of the controls cutter compensation alarms :

(1) Always command a start up block before contacting the workpiece and move in the G01 mode with a move greater than the nose radius of the tool.

(2) Use cutter compensation primarily in the finishing cut and try to eliminate it in the roughing passes. The more moves made with G41 or G42 modal, the more likely for a problem. To finish the part, use the start up block, finish cut the part and command G40 when done. Ifadditional cuts are required, use another start up block and cancel the cutter comp each time as soon as the profile cut is finished.

(3) Always cancel G41 or G42 using the G40 command. The best place to command G40 is on a G00 block, at a clearance point or moving to a clearance point. Because cutter compensation causes the control to perform some powerful calculations and is a complex command, you should also consult your controls instruction manual for further info on G41 or G42.

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 !!!

Canned Cycle Drilling & R Plane Tricks

Wasting time drilling air when “drilling” holes in a part with multiple levels is not uncommon for the novice programmer. In this post … we would like to discuss the always important R plane and how you can easily control it in your G code program.

First … the FACTS :

There are two planes that the programmer needs to be concerned with :

INITIAL PLANE … this is the plane used for rapiding around the workpiece. This plane should always be set high enough to avoid the workpiece as well as any clamps or other fixture related objects that can be struck by the tool as it moves around the part.

  • On  Fanuc controlled or Haas machine … the initial plane is defined as the last Z position before the canned cycle is called. So in the sample code below :

G00 G90 Z1.000
G98 G81 Z-.500 R.050 F1.0

  • Z1.00 would be considered the INITIAL PLANE … because it is the last Z position prior to the the G81 canned cycle command.
  • In an Okuma machine … the user can set the INITIAL PLANE by commanding a G71 Z— line prior to the canned cycle command line. So … imitating the above Fanuc line … we would program :

G71 Z1.000
G81 Z-.500 R.050 F1.0

R PLANE : The R plane is defined as the plane at which the drilling operation begins. So basically the tool rapids from the Initial Plane to the R plane … and then starts the drilling operation. The R plane is defined in the canned cycle command line. So in the above examples … R.050 is defined as the R plane … the point where the drilling operation would begin. In the above programs … the tool would rapid from the Z1.00 initial plane to the Z.050 R plane.

After drilling … we can tell the tool where to return by using the G98 ( initial plane return ) or G99 ( R plane return ) … for Fanuc / Haas … in the canned cycle command line. Once commanded … G98 / G99 becomes modal … which means the machine will remember where it is supposed to return … until told differently. When programming for Okuma … we can use the M53 ( like G98 ) / M54  ( like G99 ) commands.

NEXT … the TRICKS :

Did you know that you can very easily change the R plane when drilling on uneven surfaces?

Did you know that you can very easily change the return point between the INITIAL and R planes?

As mentioned above … once G98 or G99 is set … the control remembers where to go. Also … once the R plane is set in the canned cycle command … it remembers where the R plane is. But you can change either very easy … just command it !! Like this :

(1)G00 G90 Z1.000
(2)G98 G81 Z-.500 R.050 F1.0
(3)X1.00 Y1.00
(4)G99 X2.00 Y2.00
(5)X3.00 Y3.00 R-.100
(6)G98 X4.00 Y4.00 R.050
(7)G80

(1) – Sets the Initial Plane as Z1.00
(2) – Sets the R plane as Z.050 … return to the Z1.00 after drilling this hole
(3) – Drill this hole … R plane is .050 and return to Z1.00 … these were modal from (2)
(4) – After drilling this hole … return to R plane … still set to Z.050
(5) – Drill this hole but start at the new R plane of Z-.100 … return to Z-.100 after drilling … G99 is modal.
(6) – Drill this hole but start at the new R plane of Z.050 … return to Z1.00 after drilling this hole G99.
(7) – Cancel the canned cycle … all modal canned cycle information is cleared.

Conversational

On an Okuma machine … users can set and re-set the Initial Plane through the G71 command. For example, the command :
G71Z1.000
… would set the Z plane of 1.00 as the Initial Plane … and this can be changed at any time but just commanding a new G71 line.

On a Fanuc / Haas control … this is not so easy. You would have to cancel the current canned cycle with a G80 … move the Z axis to the desired Initial Plane … then re-command a new canned cycle to set a new Initial Plane.

So … as we illustrated here … it’s fairly easy to efficiently and effectively machine holes on uneven surfaces using a combination of the return plane commands G98 / G99 / M53 / M54 and R plane settings and through the Initial Plane selection.

So … STOP CUTTING AIR !!!
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 !!!

The HOW’s and WHY’s of CNC Sub Programming

If you have done any manual G code program creation, you know you are always looking for some shortcuts  that can not only help cut down the data input … but would also help eliminate errors. Whether they be typing errors or movement errors … the less chance to create one the better.

One of the more powerful tools available to a programmer is the use of SUB PROGRAMMING. In this Making Chips post … we would like to touch on some of the basic ideas, concepts and uses for sub programming. This post will illustrate the Fanuc / Haas coding format … but check out the end of the post for Okuma explanations as well.

What is a Sub Program?

Basically, a sub program is a G code program that is called from another G code program. The contents of the sub program is not limited and can contain tool calls, spindle calls … just about anything any other G code program can contain. The sub program itself resides in memory under it’s own program number … and is separate from the “main program”.

Conversational

Why Would I Use a Sub Program?

As mentioned above … the less data entry means less chance for a mistake. let’s take this example scenario where we have to let’s say spot drilling then drill then chamfer then tap a series of holes. The less times we have to re-type those hole locations, the less chance we will have a typo and / or put a hole in the wrong place. If we can store the X / Y coordinates of the hole locations in one location and call them out as needed … that saves data input and reduces our chances for errors. This is a good example of how a sub program ( in this case it would be the program that stores the hole locations ) can be a big help.

How Do I Program and Call a Sub Program?

A sub program scenario consists of a main program and the sub program. The main program consists of all the code that doesn’t repeat itself … the sub program consists of all the data that will be repeated. In our above example … the tool calls, spindle calls, drilling cycles will all be different for each hole … so we will store that in the main program … but the hole locations will be the same so we will store them in the sub program.

When you create a sub program … it is done just like you would create any other program. On Fanuc / Hass controls you start out with an O number … and type the program as normal. Let’s take our above example of hole locations … the sub program might look like this :

O1234
X1.1 Y1.1
X2.2 Y2.2
X3.3 Y3.3
X4.4 Y5.5
M99
%

Notice that we have an M99 at the end … not an M30 or M02 like a normal program. This indicates that this is a sub program … we’ll explain the M99 command a little later.

This program is entered in the control as any other program … and resides in it’s own memory space.

When a Fanuc / Haas control wants to call a sub program to run … the programmer issues an M98 command in the Main Program. The M98 command is also followed by a P address … which is the “O” number of the external program to run. Our above sample sub program would be called with the command :

M98 P1234

When the main program reads the M98 command … it jumps out of the main program and starts to execute the sub program … in this case program O1234. When it reads the M99 command at the end of the sub program … it jumps back to the main program to the line after the one through which it left. In other words, it jumps back to the line after the M98 command.

The Complete Story

Let’s take a look at the full program and the sub program calls … see if you can follow the path.

Main Program

O0001
G00G91G28Z0
G28X0Y0
M01
N0001
(SPOT DRILL)
G00G91G28Z0
T01M06
G90S3500M03
G00X1.100Y1.100
G43Z.500H01M08
G99G81Z-.130R.050F20.0L0
M98P1234
G80
G00G91G28Z0
M01
N0002
(DRILL)
G00G91G28Z0
T02M06
G90S3000M03
G00X1.100Y1.100
G43Z.500H02M08
G99G73Z-875R.050Q.125F20.0L0
M98P1234
G80
G00G91G28Z0
M01
ETC.    ETC.    ETC.
M30
%

Sub Program

O1234
X1.1 Y1.1
X2.2 Y2.2
X3.3 Y3.3
X4.4 Y5.5
M99
%

Can you follow the path as the program jumps to the sub program?
Here is an in-depth explanation.

N0001
(SPOT DRILL)
G00G91G28Z0
T01M06
G90S3500M03
G00X1.100Y1.100 ——————— Position to our first hole.
G43Z.500H01M08 ——————— Bring the Z axis to the clearance plane.
G99G81Z-.130R.050F20.0L0 ———- Call our canned cycle … but use L0 which means the control will hold the data … but will not execute the cycle.
M98P1234 —————————– Jump to our sub program O1234 which will cause a hole to be spotted at each X / Y location in the sub.
G80 ————————————- When the M99 is read … the program will jump back to here.
G00G91G28Z0
M01
N0002 ———————————- This sequence basically does the same thing …except we are establishing a different canned cycle before we jump to the sub program.
(DRILL)
G00G91G28Z0
T02M06
G90S3000M03
G00X.100Y.100
G43Z.500H02M08
G99G73Z-875R.050Q.125F20.0L0
M98P1234
G80
G00G91G28Z0
M01

Another Example …

Once you are able to follow the above … here is another scenario.

You can also call a sub program and have it executed a set number of times. Let’s take the example where we want to execute a program on our lathe to make a washer (3) times. We will enter the main program and sub program as below.

Main Program :
O0001
M98 P1234 L3
M30
%

Sub Program :
O1234
*********
between here is the complete machining program that includes
tool calls … spindle calls
the feeding of the stock
the machining of the part
the cut-off of the part
*********
M99
%

The cycle start is executed with program O0001 … which calls the sub program O1234 and executes that program (3) times … the L in the M98 line. This feature is different for the various Fanuc controls but is usually commanded either :

M98 P —- L
or
M98 P****$$$$ where **** is the program number and $$$$ is the number of times to repeat.

Differences Between Fanuc / Haas and Okuma OSP

The basic ideas of calling and executing a sub program is the same between these controls … the G code commands are a bit different. Those differences are outlined below.

Sub Program Call
Fanuc / Haas : M98
Okuma : CALL
Example : CALL O1234 will call sub program O1234

 Sub Program End

Fanuc / Haas : M99
Okuma : RTS

Sub Program Call with Repeat
Fanuc / Haas : M98 P1234 L5 or M98 P12345
Okuma : CALL O1234 Q5 with the Q value being the number of repeats.

That’s basically it … just some G code differences but the basic idea and execution is the same.

**************************************

Sub programming is a powerful tool … even if you are not trying to avoid re-typing and repeated data entry. Hopefully this Making Chips post will get you thinking and exploring all the ways sub programs can make you a better 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 !!!

Move That Vise !!

MOVE THAT VISE !!! … It could mean more years for your machine tool.

It seems the simpler, often overlooked things can be the downfall of most shop equipment. Focusing on a few simple ideas can avoid those big repair bills and keep machine tools running like new much longer.

When most setups are done on a VMC, the workholding fixture is neatly mounted right in the middle of the table. Although it looks good, this is actually one of the worst “habits” for the machine. Locating the vise or fixture in the same place has the following harmful effects on the life of the machine:

  • Table wear, resulting in dip or sag in one spot.
  • Boxway or guideway wear on or around the spot, causing loose surface and gib contact, and shuck in the ways.
  • Ball screw wear, resulting in excessive backlash in that one area of the screw, which cannot be repaired through CNC compensation.

Of course you’re going to clean the table completely before installing the vise.

Then are you going to place the vise so it looks nice and neat in the center of the table?

NO !!!

Placing the vise or fixture in or around the same area of the machine table will cause all of the above, with the most common symptom over time being backlash of the screw. When trying to compensate and set the backlash, the person making the repair will often find different backlash values when checking along the length of the axis stroke. This most often results in the need to replace the whole ball screw. Because most CNC machine controls only permit one backlash compensation value to be set in the parameters, compensating for the backlash cannot be effectively performed through the control.

Conversational

You also may find that the gibs need to be adjusted in that area of the boxway, because the axis has some side-toside movement to it when moving. Squareness in that area will disintegrate; and, in the worst case, this shucking can be heard when the axis changes direction. The most common remedy of adjusting the gib in that area causes the axis to bind when it reveals to the other areas, because the boxway wear is different along the stroke. In this repair, the machine’s boxways may need to be reground, rescraped or both. In either of these cases, the repair bill will be huge.

The remedy is to make sure to move the vise or fixture location around on the tabletop whenever possible. You will see a more consistent wear pattern for the machine, and any backlash that occurs can be taken up correctly through the control. You will not be able to stop machine wear, but you can distribute it more evenly along the machine, which provides a longer life for all the components involved.

 Happy Chip Making !!

Check out our Real World World machine shop software at www.KentechInc.com

Backlash in Your CNC – What You Need to Know

( NOTE : This article references FANUC controls but is basically applicable to all CNC controls. )

A machine is a machine is a machine. Just because the words CNC are attached to your machine tool doesn’t mean it doesn’t get old or lose it’s accuracy. And one of the main reasons your CNC machine losses it’s accuracy is due to the ever infamous backlash.

What is backlash ?

The axis motion that makes up your machine tool is done through the use of ballscrews attached to your machining center’s table and spindle housing or your lathes tool turret. The nut for the screw is usually attached to the table or turret and is connected to the ballscrew which is connected to your drive motor. As the motor turns the ballscrew, the nut moves the table or turret and your machine has motion. All ballscrew assemblies have some “slop” or backlash at assembly – the match between the screw and the nut. Basically backlash is the amount of motion the screw has to make when reversing direction before the nut and therefore the table or turret start to move.

How is backlash compensated?

Using the machine tools CNC controller, the builder can tell the controller how much motion is lost when the axis reverses direction due to the backlash. This value is stored in the machines parameters and when the particular axis goes to change direction, it looks in this parameter to know how much motion it needs to have (how many revolutions of the screw it needs to make) before the axis will physically start to move. The value of the parameter is usually in MM, although they may be in INCH settings in some instances

Why should I care ?

As the machine tool wears or as contaminants get onto the ballscrew and therefore in the nut, the original backlash settings lose their accuracy and therefore effect the accuracy of the machine tool. Positioning problems arise, straightness problems arise, as do a host of other related problems. Basically, the machine does not meet the specs like it did when it was new.

As mentioned above, sometimes contaminants can get onto the screw and then get carried into the nut. Although most nuts are protected against chips and debris, poor conditions can sometimes force the debris into the nut causing premature wearing of the screw and a pronounced backlash problem. Those contaminants can range from coolant to cutting chips. That is why it is essential to keep the machine areas clean and free from an excessive amount of chips. If chips are allowed to accumulate, they can become packed and when the machine tool moves, it forces the chips under guards and into areas where they shouldn’t be. Eventually they get forced into the screws and nut areas causing un-repairable problems. Ballscrew replacement is not a cheap repair. Keep the expression: “An ounce of prevention is worth a pound or cure” in mind when planning your maintenance efforts.

What can I do about backlash ?

The normal method for adjusting the machine’s backlash involves adjusting the backlash parameter values. This can be done by a qualified technician or you can give it a try. Outlined below is a brief but complete explanation of how to check for backlash and how to adjust it in FANUC controlled machine tools.

How often should you check it ? Recommended time frame would be about every 3-6 months. If you create the following sample programs in your memory and leave them there or upload and download them from a shop floor PC, you shouldn’t spend much more than one hour or so keeping your machine accurate and at the same time you’ll be checking for any other damaging problems. For example, if you see the backlash changing drastically, you might find a way lube problems or chip build up problem before they cause bigger problems.

How much backlash compensation is acceptable ? As mentioned above, all machines have some backlash adjustment, even when brand new and at ship time. As the machine wears, that value needs to be increased. Normal wear might have .005″ – .010″ adjustment in a ballscrew. If the value needs to be more than .010″, it might be time to take a deeper look. Also, you need to check the backlash at various areas of the screw as it might be wearing more in one area than another. One example might be on a machining center where the set-up people always mount the vise or fixture in the middle of the table. Looks good but also causes a massive amount of wear in one confined area. the best scenario is to mount the vise or fixture all over the table, changing the location for every job – spreading the wear around evenly.

The best way to check the backlash is to first clear out the current parameter value in the control. The various parameter numbers for the variety of FANUC controls are listed further down in this page. First, write down the current values, then clear them by setting them to zero. Then make the machine move through the memory mode. We have found discrepancies in the past between the machine’s handle or MPG mode and the memory mode, so we recommend you run the machine through MDI or through the machines memory mode. Below are a couple of sample programs for FANUC controls that you can use to gather your backlash data. Remember, the backlash is the amount of wasted motion when the particular axis changes direction.</p>

<p>If possible, check the backlash at different areas of the screw. On a machining center, mount the block in different areas of the table and check. On a lathe, check the backlash as various distances away from the chuck. If the values are different in the different areas, this could mean that the screw is worn in one place different than others. On a lathe, this tends to happen close to the chuck where the majority of the cutting is performed. You can’s do much about to prevent it on a lathe but on a machining center, you can help yourself by mounting the chuck or fixture in various places on the table to allow for even wear. If you find big differences in the backlash in different areas, it may be too late and you may have to replace the screw.

Conversational

Machining Center Backlash Adjusting Program.

If you have a Vertical or Horizontal machining center, the following program will give you an idea of how to create a program to test the backlash for each axis.

The following is a sample program for the X axis. Start the program with an indicator mounted to the spindle, touching a block mounted on the table, touching the right side of the block.

You can let the program run a couple of times to make certain that you get the same readings at the M00’s in the program. The difference between Reading #1 and Reading #2 is the amount of backlash in your X axis.

You can use the same style program making changes as required to perform the same function for the other axis as well. Basically, you just want the machine to move one way then back, stop so you can and collect the indicator reading, then move the other way and back and collect that reading.

CNC Lathe Backlash Adjusting Program.

If you have a CNC lathe, the following program will give you an idea of how to create a program to test the backlash for each axis.

The following is a sample program for the Z axis. Start the program with an indicator mounted to the spindle or chuck, touching a block mounted on the turret or the tool turret itself, touching the spindle side of the block or turret.

Once you collect the value and know the backlash for your machine, you’ll need to adjust the parameter values. Parameter values for FANUC controls are usually given in MM  values, without the use of decimal point. So, for example, a parameter value of 30, actually means .030 mm – the decimal point is imaginary and placed three places from the right. You can use the following conversion formula to change your backlash data to mm, then enter that value into appropriate parameter – don’t forget to drop the decimal point and add any zeros as required.

MM = inch x 25.4

For reference, 1mm = .0394 in.

On a CNC lathe, the value can either be a radius or diameter value. Since there is no easy way to tell, input a radius value then re-run the test program. Adjust as necessary and make a note so next time you will know.

When you’re done, you should re-run the particular axis program again to double check that you did the backlash adjustment correctly. When you re-run the program, you should see less than .0001″ backlash.</p>

FANUC Backlash Parameter Numbers.

Listed below are the parameter numbers for the various FANUC control models. One note, lathe controls are T models whereas machining centers are M models.

FANUC Version 6T :

X Axis = Par # 115

Z Axis = Par # 116

FANUC Version 6M :

X Axis = Par # 115

Y Axis = Par # 116

Z Axis = Par # 117

4th Axis = Par # 118

FANUC Version 10/11/12T :

Par # 1851

Seperate line for each axis.

FANUC Version 10/11/12M :

Par # 1851

Seperate line for each axis.

FANUC Version 0T :

X Axis = Par # 535

Z Axis = Par # 536

FANUC Version 0M :

X Axis = Par # 535

Y Axis = Par # 536

Z Axis = Par # 537

4th Axis = Par # 538

FANUC Version 16/18/20T :

Par # 1851

Seperate line for each axis.

FANUC Version 16/18/20M :

Par # 1851

Seperate line for each axis.

NOTE : This 16/18/20 series of control can have a seperate backlash amount when moving at a feedrate and for moving at the rapid rate. This is an option – check with your machine tool builder. If this is the case, Parameter number 1851 is for feedrate and # 1852 is for rapid. You can use the programs above, just change from G00 to G01 and add a feedrate to test for the feedrate backlash amount.

Until Next Time … Happy (and accurate) Chip Making !

 Please visit our website for the best in Real World Machine Shop Software … just CLICK the pic below !!

Chip Removal at Your CNC Machine – AIR vs. WATER

air gun for blowing chips at a cnc machineA standard component of almost every CNC machine in almost every shop is the AIR GUN. They exist in a variety of forms and power ranges … but are the tool of choice for cleaning chips off workpieces and areas of the machine itself. Fast and easy to access … easy to configure and expand.

But are there any serious drawbacks to the use of the air gun at the machine?

As a former CNC field service technician … I can emphatically state YES !! I would say that the air hose and air gun are one of the leading causes of major CNC component failures such as backlash and ball screw replacement as well as other axis positioning inaccuracies caused by machine way failures due to scoring. The innocent act of blowing off those chips can actually be one of the more destructive acts a machine operator can do to the machine. Why?? Here’s a brief run down of some of the more common problems … as experienced first hand from my experiences “in the trenches”.

Backlash and Ball Screw Replacement

Of all the damage I have witnessed due directly to air gun use … the need for the replacement of the axis ball screw assembly is by far the most common. Now for the most part I’m not talking about simply blowing off the chips at the end of the machining operation … I am primarily talking deep-cleaning the machine. Cleaning the machine and machine table table during a change over … cleaning the chuck getting ready to install the collet assembly … the “before the weekend” type cleaning of the machine where the operator may be charged with cleaning the machine from the weeks activities and is using the air gun extensively to gather the chips and “deep-clean” the machine. This type of extensive chip blowing will inevitably lead to the chips being blown into areas not designed to handle them. Perhaps the chips build up in a corner … out of sight … or under a way cover or find their way into a telescoping way cover. Looks clean … but these chips are hiding and waiting. As new machining starts … the motion of the machine forces the chips deeper and deeper into those areas until eventually they find their way onto the ballscrew where they “work their black magic”. The wiper systems for both the machine ways and the ballscrew assemblies are not designed to stop chips being forced in under pressure from the force of an air gun … but rather are designed to be effective in conjunction with the water flow of the coolant. What starts out as some axis backlash will some worsen and eventually will require the replacement of the ballscrew assembly.

Axis Way Scoring

In conjunction with the destruction mentioned above … a different scenario occurs when the chips get lodged between the way covers and the machine ways. As the axis moves … the chips dig and score the ways of the machine. What starts out as some simple score marks are soon magnified as more chips and more metal shavings lodge in those scores and they deepen and worsen and so on and so on and so on … until the damage is extensive. This type of damage is a much harder to remedy … the ways of the machine cannot simply be replaced. Now the repair consists of re-scraping or re-grinding the ways … a major machine rebuild … or replace the machine tool completely.

Other Common Component Failures

Over the years I have witnessed many other component failures that I would attribute directly to the use … or over use … of the air gun by the machine operator. These range from electrical components where chips were blown into cabinets or through seams of cabinets … CNC lathe turret issues because chips had found their way into the indexing mechanism … and ATC issues where chips were interfering with the tool change mechanisms. In short … excessive use of the air gun and blowing of the chips inside the machine enclosure is very destructive … and expensive !!

Estimating

The Better Solution – COOLANT

The fact that blowing chips is a destructive act … doesn’t help with the everyday need in the machine shop and at the machine to clear away and deal with the metal chip issue. But I can definitively state that COOLANT and WATER FLOW is a much better alternative. One easy way to eliminate the overuse of air pressure is to provide an alternative like the following.

Create a coolant hose line by installing a T-joint right after the coolant pump. Attach a standard garden hose to the T and run the hose to the front of the machine. Install a standard garden spray nozzle at the end. Now when the coolant pump is on … the operator will have pressure and in essence a garden hose with coolant flowing at his station. Instead of using the air gun in all instances … he now has the option of using the coolant as a cleaning medium. The water flow is a much better and safer alternative to the high pressure air gun. BUT NOW IT’S UP TO ALL TO INSURE THE COOLANT MIXTURE IS MAINTAINED. With a healthy coolant mixture … another benefit is the application of oil to the areas where the coolant is sprayed. Instead of leaving behind metals chips and shavings … the spray will leave behind a coating of beneficial lubricating oil.

The flow and lesser pressure of the coolant hose provide a much safer and still as efficient chip removal alternative.

Blowing chips seems like such a simple act … and one that is so common at the machine. But given a more in-depth look … one can certainly see the possible destructive side effects this simple act can have on the machine tool. If you are in a production environment … no doubt you have even experienced these destructive end results first hand.

I hope this glimpse into the “real world” can start you and your shop thinking in the direction of utilizing coolant and coolant spray as a chip cleaning alternative. Your machine tool will thank you !!

Until next time … Happy Chip Making !!

Kenney Skonieczny

Kentech Inc.

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