We have a CNC Swiss that we use to turn very small precise parts. When a part has several different diameters I notice that when one diameter is on the nominal dimension, often the others are off nominal by several tenths. Is this due to different tool pressure at the different depth of cuts? Is there a solution?

Tiny Turner

Dear Tiny,

I doubt the issue is from tool pressure. It is more likely that your turning tool center height is off. Old timers will tell you that tool center height is very important in very small turning. I’ll attempt to explain why that is so.

In the following example take a look at how being off center can affect the diameter being turned. First let’s assume that if your tool was brought to X0, the tip would be dead on the centerline of the bar.

Line “a” is how far your tool is off center. Line “b” is your programmed X-axis dimension.  Line “c” is the actual distance to the cutting edge of the tool or ½ the actual turned diameter dimension on your work.

Imagine making Line “b” longer and longer (turning progressively larger diameters) and you’ll see that Angle “A” flattens out, which in turn will make Line “c” shorter relative to Line “b.” In other words the error becomes less the larger the diameter you turn is. So when turning very small diameters it is critical to be on center.

The Pythagorean Theorem tells us that a ²+b ²=c ².  Using that information, let’s assume that your tool is 0.003” off center, and you are turning a 0.030” diameter (side a=0.003”, side “b”=0.015”). Side c therefore is equal to 0.0153” because c=√ (.003 ²+.015 ²), so your turned diameter will be 0.0306” or will be 0.0006” off of nominal size.

Now assume you are using the same tool to turn a 0.125” diameter. Running the same math we find that the turned diameter (rounded) will be 0.1251” or will be 0.0001” off of nominal size.

Since the 0.030” diameter was 0.0006” off of nominal we have a differential of 0.0005” between the two dimensions. It follows that when you offset one dimension to nominal size, the other dimension will be 0.0005” off of nominal. All of which makes it difficult to dial in the workpiece without editing the program (bad), or using two separate offsets (nearly as bad).

You can also add a macro variable to the programmed dimension. But when you think about it, all that does is provide a convenient way for the operator to edit the programmed dimension. It’s better to fix the root cause of the problem by getting the tool on center.

You can use this information to calculate how far your tool is off center and correct it with an offset assuming you have Y-axis capability. Small capacity Tsugami Swiss lathes have a feature built into the control to calculate tool height using this principle. But you can see it works best at very small diameters where Angle A and the resulting error is greater.

There can also be mechanical reasons for disparity between turned diameters. If your tool is on center check for backlash, flex in the machine/tool holder, and of course the fit of the material to the guide bushing.

Question: When you watch the Super Bowl, are you more interested in the game or the commercials?

We are having trouble with chatter while turning on our 20mm Swiss CNC lathe. We recently replaced the guide bushing bearings and we have the bushing adjusted so tight that the bar is a press fit inside the bushing, but it still chatters. We have also tried different tool geometries and slowing the rpm down. Nothing works. Can you help?

Squealing in Wheeling

Dear Squeal,
I’m pretty sure I see the problem. These are some of the possible causes of chatter while turning on a Swiss:

1) Incorrect Tool Geometry: Positive rake tools cut more freely and can reduce the cutting pressure, which in turn can help eliminate chatter. Smaller nose radii also generate less pressure. However, this effect is minimal compared to reducing the feed rate or the depth of cut.

2) Guide bushing is too loose: Obviously not the problem here, but when the bushing is too loose the bar can move about during turning causing chatter.

3) Guide bushing is too tight: While this seems counterintuitive, over-tightening the guide bushing can cause chatter. A typical driven bushing has two angular contact bearings in the front and one or two bearings at the rear. When the bushing is run too tight, the back bearings will compress under the load caused by the bar moving forward, and the front bearings will unload. With the preload on the front bearings being pressed out by the bar being forced through the bushing, the bearing set is unable to support the cutting forces created by turning. This is probably your problem. This situation will lead to the back bearing failing, followed soon after by the front bearings. There is no need to run the bushing as tight as you describe. If you are after better roundness use ground bar stock. The bushing should be adjusted snug to the bar but still be loose enough that you can rotate it by hand with the bushing locked. You should feel some drag on the bar when you rotate it.

Read full article here

Dear Shop Doc,

We are turning a part made from PEEK (polyetheretherketone plastic) and need an 8 Ra surface finish on the part. We have tried carbide and a PCD insert. We can achieve around a 10 Ra finish but that is about the best we can do. Since it is a medical implant we can’t use coolant or abrasives. What process will enable the required surface finish?

Too rough

Dear Too rough,

You are on the right track using a PCD (polycrystalline diamond) for machining PEEK. The high hardness, abrasion resistance, and heat tolerance of diamond makes it an ideal tool material for machining medical grade PEEK.

However, in order to achieve very low surface finishes in soft materials like PEEK, or even metals like aluminum, you need a tool with a nearly flawless edge. Polycrystalline literally means “many crystals.” A PCD insert has a tip composed of small diamond crystals held together with a metallic binder. The random orientation of the crystals along with the metallic binder (usually containing cobalt) helps give the very hard diamond some toughness to resist fracture.

If you were to look at a micrograph of the cutting edge, you would see the diamond crystals do not provide a continuous, smooth cutting edge. In turning, each little crystal in the matrix will leave its “mark” on the turned surface. The solution is to use a monocrystalline diamond tool, which is a single piece of diamond crystal with a lapped cutting edge.

In addition to the better tool, you will need to address as many of the other variables that affect surface roughness as possible. Ideally your lathe would have a dynamically balanced integral motor spindle with ultra high precision ceramic bearings. The closer the lathe you run it on is to the ideal, the better off you’ll be. Choose the proper feed rate for the nose radius (see sidebar). Keep tool and work overhang to a minimum. Make sure your finish pass depth of cut is at least 60 percent or more of the nose radius.

Formula for Estimating Surface Roughness:
Ra= f²1,000,000/(24 r)
Ra= Surface Roughness in micro-inches
f = Feed rate in inches per revolution
r = Tool nose radius

If you are turning from bar, consider running short lengths of material and be sure to use a spindle liner that closely matches the bar diameter in order to minimize bar whip. Installing a close fitting bushing into the back of the collet can also help damp bar vibration.

Cool the work with a cold gun (vortex tube). Make sure you prevent chips from wrapping around the work. You can rig up a Shop Vac or use a compressed air gun mounted below the cutting area to draw the stringy chips away from the work.

Dan Murphy
REM Sales LLC

Dan Murphy is a regional sales manager for REM Sales LLC., a U.S. Tsugami importer. He can be reached at dmurphy@remsales.com

We are turning a part made from PEEK (polyetheretherketone plastic) and need an 8 Ra surface finish on the part. We have tried carbide and a PCD insert. We can achieve around a 10 Ra finish but that is about the best we can do. Since it is a medical implant we can’t use coolant or abrasives. What process will enable the required surface finish?

Too rough

Dear Too rough,

You are on the right track using a PCD (polycrystalline diamond) for machining PEEK. The high hardness, abrasion resistance, and heat tolerance of diamond makes it an ideal tool material for machining medical grade PEEK.

However, in order to achieve very low surface finishes in soft materials like PEEK, or even metals like aluminum, you need a tool with a nearly flawless edge. Polycrystalline literally means “many crystals.” A PCD insert has a tip composed of small diamond crystals held together with a metallic binder. The random orientation of the crystals along with the metallic binder (usually containing cobalt) helps give the very hard diamond some toughness to resist fracture.

If you were to look at a micrograph of the cutting edge, you would see the diamond crystals do not provide a continuous, smooth cutting edge. In turning, each little crystal in the matrix will leave its “mark” on the turned surface. The solution is to use a monocrystalline diamond tool, which is a single piece of diamond crystal with a lapped cutting edge.

Read full article here

Dear Shop Doc,

We are trying to run a variety of very small parts on a 20 mm gang tool CNC Swiss and are having trouble with deflection when cross drilling and milling. Is there a way to get the live tools closer to the guide bushing?

 Bent in Benton Harbor

Dear Bent,

There is no way to bring the tool closer to the guide bushing face. You can bring the guide bushing face closer to the bar by ordering an extended nose guide bushing.

An ER16 live tool spindle is usually between 14-16 mm away from the face of the guide bushing. You can decrease that distance by using an extended nose guide bushing to take up most of that space. However there are several issues to consider.

The fixed position of the live spindle is set so that the spindle has adequate clearance for the collet nut on the live tool attachment. Simply extending the nose of the bushing out means that the nut will now interfere with the face of the guide bushing, so you must do one of two things:

1)      Extend the spindle by chucking on a smaller capacity ER8 or ER11 collet chuck. You can buy an ER8 or ER11 with a 10 mm shank and a mini nut. Mount the drill chuck in the live spindle and chuck the tool in the smaller capacity drill chuck. Stick the small drill chuck out far enough so that the ER16 chuck nut doesn’t hit the bushing face.

2)      Order the extended nose to be turned to a smaller diameter. You could for example have the extension made to a 3/8” diameter by 0.300” long. Then keep the ER16 chuck nut above that diameter while cross drilling.

You will also need to shim out all of your turning tools by the same amount of the extension, as well as set your drills back by the same amount. Your machine tool builder might offer blocks that will shim the whole gang slide out by a set distance.

One final solution that might work depending on your situation is to use larger diameter bar stock. A larger bar can provide extra rigidity if you turn up to the live tool feature, machine it, then turn. In order to work, the bar diameter must be at least 1/3 of the distance from the face of the bushing to the center of your live spindle or larger.

Dan Murphy is a regional sales manager for REM Sales LLC., a U.S. Tsugami importer. He can be reached at dmurphy@remsales.com.

Have a technical question of your own? Email us and we’ll find a Shop Doc to answer it. Or, if you know a Shop Doc or are a Shop Doc contact us to contribute. emily@todaysmachiningworld.com, 708-535-2237

Extended nose guide bushings, courtesy of REM Sales, LLC.

Dear Shop Doc,

On our CNC lathes we occasionally have trouble with push back when using collets on bar jobs. Our collets have smooth bores and I am wondering if a serrated collet would help or if it will just create more problems.

Chuck Force

Dear Chuck Force,

Serrated collets will probably help, but first let’s consider all of the variables.

1. Bar whip—Bar whip can cause the bar to act as a lever against the collet, prying it open. You should always use a spindle liner and/or a properly sized liner set in your bar feeder to minimize bar whip.
2. Collet bore—Most collet systems have some gripping range, but the bore of the collet can only be machined to one given nominal diameter, and that diameter fits the bar the best. Avoid using a collet that’s “close enough.”
3. Chucking pressure—The hydraulic pressure to the rotary actuator can be adjusted. Follow the manufacturer’s recommendation for the operating range and adjust accordingly. In general, you need higher pressure for larger diameter bar and less pressure for small diameters.
4. Maintenance—Make sure that the sliding components of your collet chuck are clean, lubricated and slide easily. Make sure your hydraulic oil is in good condition, the level is adequate, and the system is operating in the proper temperature range.

Serrated collets work by reducing the surface area of the collet bore, thereby increasing the pressure that the contact area of the collet exerts against the work. You can calculate the surface area of the collet bore using the formula: 2 π r2 + 2 π r h. Ignoring the area removed by the slots in the collet, a 1.0” diameter collet with a 1-1/4” land has 5.5 in² of gripping surface.

If the collet closes with 1,000 pounds of force, that force is distributed over the 5.5 in² surface area of the bore, resulting in a contact pressure of 181.8 psi. If you decrease the surface area of the collet bore by machining in serrations, you increase the contact pressure by a corresponding amount. This doesn’t multiply the holding force in any way; you are still applying the same 1,000 pounds of force to the task of holding the work. By applying the force to a smaller area with greater pressure, the collet can dig into (deform) the work. Whether or not the collet permanently marks the work (plastic deformation), or the work bounces back (elastic deformation) depends on the force applied.

Another option is to have the collet coated with a textured carbide alloy coating like Carbinite (go to www.carbinite.com for more info). The principle is the same as serrations, but instead of grooves cut into the collet bore, the bore is coated with a crystalline like carbide alloy. The coating has a texture similar to sandpaper, which provides tremendous grip.

Dan Murphy
REM Sales LLC

Dan Murphy is a regional sales manager for REM Sales LLC., a U.S. Tsugami importer. He can be reached at dmurphy@remsales.com.

Dear Shop Doc,

We are running a long aluminum part on our CNC Swiss and have problems with the long stringy chips building up in the machine and getting wrapped around the part. We’ve tried every “aluminum” insert under the sun and have 2,000 psi coolant, but nothing works. Please help!

Tangled Up in Tennessee

Dear Tangled,

There is a new chip control technology for aluminum that I’ve found to be very effective. It’s a PCD (polycrystalline diamond) insert that has a 3D chipbreaker. Up until now, manufacturers have been unable to produce 3D chipbreakers in the ultra-hard polycrystalline diamond material. A new process has been developed that uses a laser to etch a variety of 3D chipbreaker shapes into the PCD. The inserts are made by Becker Diamont.

They have a video on YouTube that can be found at: www.youtube.com/watch?v=gLRJdMDvbpY. A brochure can be downloaded at: www.ranitool.com/ChipBreaker-ranilowres.pdf.

On a Swiss I’ve found that it’s the feed rate that is critical to getting the chip to break. In general, a larger depth of cut requires a slightly higher feed rate. On a fixed headstock lathe, you can also vary the depth of cut and the feed rate for optimum results.

Other possible solutions include milling a flat or narrow slot along the length of the cut before turning. I prefer to use a narrow slotting saw to cut an off-center slot along the turn length. A narrow slot has less chance of generating an out-of-round condition on the turned diameters. Milling the slot off of the centerline of the work prevents the slot from hitting the turning insert squarely. The slot being off center along with the rotation of the work causes the slot to hit the insert and travel by it on an angle. This eliminates any pounding caused by the interruption while providing enough interruption to break the chip.

Problems with grooving and cutoff tools can often be solved by using a peck cycle like G75, which is like a peck drilling cycle, but from the cross axis rather than along the Z-axis.

Ultimately these other options add cycle time while the PCD insert will likely reduce cycle time and improve uptime.

You will pay more for PCD, but it almost always costs less than a polished carbide insert due to the vastly improved tool life.

Another added benefit is that once you start breaking the chips up, you won’t have to empty out the chip bin nearly as often. Those long wiry chips create big air pockets that take up a lot of space.

Dan Murphy
Tsugami REM Sales

We are running a long aluminum part on our CNC Swiss and are having problems with long stringy chips building up in the machine that are getting wrapped around the part. We’ve tried every “aluminum” insert under the sun and have 2,000 psi coolant, but nothing works. Please help!

Tangled Up in Tennessee

Dear Tangled,

There is a new chip control technology for aluminum that I’ve found to be very effective. It’s a PCD (polycrystalline diamond) insert that has a 3D chipbreaker. Up until now, manufacturers have been unable to produce 3D chipbreakers in the ultra-hard polycrystalline diamond material.  A new process has been developed that uses a laser to etch a variety of 3D chipbreaker shapes into the PCD. The inserts are made by Becker Diamont. They have a video on YouTube that can be found at: http://www.youtube.com/watch?v=gLRJdMDvbpY.

A brochure can be downloaded at: http://www.ranitool.com/ChipBreaker-rani-lowres.pdf.

On a Swiss I’ve found that the feed rate is critical to getting the chip to break. In general a heavier depth of cut requires a slightly higher feed rate. On a fixed headstock lathe, you can also vary the depth of cut as well as the feed rate to obtain optimum results.

Other possible solutions include milling a flat or a narrow slot along the length of the cut before turning. I prefer to use a narrow slotting saw to cut a slot off center along the turn length. The narrow slot leaves less chance of generating an out of round condition on the turned diameters. Milling the slot off of the centerline of the work prevents the slot from hitting the turning insert squarely. The slot being off center along with the rotation of the work causes the slot to hit the insert and travel by it on an angle. This eliminates any pounding caused by the interruption while providing enough interruption to break the chip.

Problems with grooving and cutoff tools can often be solved by using a peck cycle like G75, which is like a peck drilling cycle, but from the cross axis rather than along the Z-axis.

Ultimately these other options add cycle time while the PCD insert will likely reduce cycle time while improving uptime. You will pay more for PCD, but it almost always costs less than a polished carbide insert due to the vastly improved tool life.

Another added benefit is that once you start breaking the chips up, you won’t have to empty out the chip bin nearly as often. Those long wiry chips create big air pockets that take up a lot of space.

-Dan Murphy
Tsugami REM Sales

Dan Murphy is a regional sales manager for Rem Sales LLC., a U.S. Tsugami importer. He can be reached at dmurphy@remsales.com.

Dear Shop Doc,

One of our operators came from another shop and told us that we can use Custom Macro for tool life management, but he doesn’t know how. I checked the manuals but don’t see anything obvious. Can you help?

Through the Grapevine

Dear Grapevine,
Custom Macro programming, also known as parametric programming, is capable of performing many different tasks, even ones not specifically outlined in the programming manual.

Macro programming allows the use of variables, logic, arithmetic, conditional branches, and custom alarms. For tool life management, we’ll need to use most of those functions. Ideally you should make a flow chart to outline the sequence of events that need to take place. In this case, you want to check the life remaining on all tools and either run a part or have the machine generate an alarm to notify the operator that a tool needs to be changed. Since all this needs to take place before machining, you can put that part of the Macro at the beginning of the program.

You should use variables to hold the life count and the life number for each tool. I like to relate the variable register number to the tool number. Let’s assume there are four tools and they are T0100, T0300, T1100 and T1400. We will use variable numbers 501, 503, 511 and 514 to hold the life count and variables 101, 103, 111 and 114 to hold the tool life value. Values stored in variables 100-149 are lost when the power is switched off. Variables 500-531 retain the value at power down.

O1234; (Machining program number)
#101=1000; (Tool life value for T0100)
#103=500; (Tool life value for T0300)
#111=775; (Tool life for T1100)
#114=2300; (Tool life value for T1400)

Setting the tool life from the program ensures that the proper values are used and saved. Next, you need to check the life of each tool. For this you can use a conditional BRANCH statement.

IF[#501 GT #101] GOTO 1000; (If the count in #501 is greater than the life set in #101 skip to line N1000)
IF[#503 GT #103] GOTO 3000;
IF[#511 GT #111] GOTO 11000;
IF[#514 GT #114] GOTO 14000;
(Normal machining program goes here)

At the end of the program you need to add to the tool life count and list the alarms. With the alarms you will also reset the tool life count so that you don’t have to rely on the operator to remember.

(End of normal machining program is here)
#501=#501+1; (Add one to the tool life count of tool T0100)
#503=#503+1;
#511=#511+1;
#514=#514+1;
GOTO 9999; (Skips over alarms and goes to M30 code)

N1000 #501=0; (Reset life count for T0100)
#3000=1 (TOOL LIFE OVER CHANGE TOOL T0100) (Alarm to stop machine with message)
N3000 #503=0;
#3000=1 (TOOL LIFE OVER CHANGE TOOL T0300)
(Repeat for #511 and #514);
N9999 M30; (End of program)

The GOTO statement will cause the program to skip over the alarms while the previous IF GOTO statements will cause them to be read. There are lots of different ways to program this. Submit your program in the comments on the Shop Doc Blog at www.todaysmachiningworld.com.

Dan Murphy
REM Sales LLC

I have a part that has an internal hexagon that needs to be put into the part in relation to milled features. Is there some way that a wobble broach can be oriented to the C-axis on my CNC Swiss?

-Vexed Hex

Dear Vexed,

On a full featured CNC Swiss there is a unique solution to this issue. As you know, rotary broaching holders offer no way of orienting the polygon shaped broaches to the work. The method that follows will also allow you to broach faster and will never “spiral” on a deep broached feature.

If your CNC Swiss has a Fanuc control equipped with the polygon cutting option, you should be able to use an adjustable angle live drill unit to wobble broach the hexagon shape while holding angular relationship to other live tool features on the work. Here’s how; mount an off-the-shelf rotary broaching bit into the angular drill unit and set the angle to 1 degree. This puts the broach in the same attitude as it would be if it were sitting in an ordinary rotary broach holder. If you have a CNC lathe or Swiss with a programmable B-axis, simply command the live tool B-axis to a 1 degree angle.

Use the G51.2 polygon cutting command to orient and synchronize the live tool spindle to the work spindle. Ordinarily this command is used for cutting external polygons on the work using a polygon attachment and cutter, but it works just fine for wobble broaching.

Example of the command when used for broaching: G51.2 P1 Q-1 R45.0;

The P value equals the ratio of the work spindle to the tool spindle. Q equals the ratio of the live tool spindle to the work spindle. The sign of the value determines the spindle rotation direction of the live tool. A negative value is usually the Vexed Hex counter-clockwise direction, which would match a clockwise direction on the opposing work spindle.

If the live angle tool attachment has a gear ratio to the commanded speed then you would use P and Q to compensate for that ratio. For example, if the live tool spins at 4,000 rpm when you program 2,000 then you would program values of P1 Q-2.

The R value sets the angular relationship of the live spindle to the work spindle. This allows you to adjust the orientation of the broach in relation to the C-axis of the main spindle. The value range is from 0 degrees to 359.999 degrees. I prefer to program a macro variable instead of a numeric value so that the orientation can be adjusted without editing the program. For example—G51.2 P1 Q-1 R#510: Variable 510 can now be used as an offset to adjust the orientation of the broach to the work.

Once you have commanded the polygon turning function G51.2, program the broaching operation the same exact way you would if you were using a conventional rotary broaching tool. In most cases you can broach at a much higher rpm using this method than you can with a rotary broach holder. You are only limited by the maximum speed of the main or tool spindle. Cancel polygon mode by commanding G50.2.

-Dan Murphy
Tsugami REM Sales