Shop Doc Blog | Todays Machining World

Justifying Use of a High-Speed-Spindle

Posted on February 22, 2010

Dear Shop Doc,

We have often heard the high speed machine spindle is expensive and has to be replaced at some point. Can you shed some light on the high speed spindle construction and service?

Speedster

Dear Speedster,

To understand the cost and justification of a High-Speed-Spindle, let’s look at the more common belt-driven spindle first. A belt-driven spindle has the motor and spindle mounted separately, linked with a belt-pulley mechanism. With this simple and cost effective system, builders can also install pulley combinations that change ratios on the fly to boost both low end torque and high end rpm. However this time honored design runs into difficulties when rpm continues to push higher. Slipping, vibration, and noise from belt-pulley mechanism eventually become hard to control, so most builders cap belt-driven spindles around 12,000 to15,000 rpm. To answer the market’s demand for higher rpm, the industry’s solution is the Integral-Motor-Spindle (also known as a motorized spindle or built-in spindle).

Integral-Motor-Spindle has all three elements – motor, spindle and tooling – built into one single unit. Its motor winding surrounds the rotary shaft, completely eliminating the mechanical linkage, like belts, pulleys or gears. It can deliver low vibration speed all the way to 100,000 rpm and beyond. But cramming all these elements into one tight unit makes an Integral-Motor-Spindle a more complex device that carries a higher price tag than that of a belt-driven spindle. Over the years, the Integral-Motor-Spindle has proven itself, becoming the spindle of choice for speed over 12,000 rpm. Practically all main-stream high-speed-spindles are Integral-Motor-Spindles. Due to its clean self-contained modular design, we have seen Integral-Motor-Spindles constantly extending their uses. They show up in some not so high-speed, heavy-duty 50-Taper CNC mills and high-end lathes and offer comparable, if not better, spindle life to that of a belt-driven spindle.

However, when it comes to High-Speed-Spindle life with speed over 20,000 rpm, there are some justified concerns. Our experience shows the spindle life is much more sensitive to how it is used, and the biggest culprit for premature failure is cutting heavier than the High-Speed-Spindle designed for.

High-Speed-Spindle advocates smaller tools with faster and lighter cuts (High-Speed-Machining method) not only because it works for many applications – like surfacing and hard milling – but also because of the spindle limitation. First of all, once spindle bearing DN factor (speed times bore) reaches a limit, increasing max speed (N) requires decreasing bearing ID (D), which in turn constraints the tool holder size. Typically you will find HSK63 for 24,000 rpm, HSK50 for 36,000 rpm, HSK40 for 42,000 rpm and HSK32 for 60,000 rpm. When tool holder size is reduced, so is overall tooling rigidity. Secondly, motor size is often limited by the housing available for the spindle, and with no belt/gear ratio to amplify the torque, a High-Speed-Spindle can lack low end torque for heavy cutting. When a programmer enjoys the high speed but is inconsiderate of the rigidity and torque the High-Speed-Spindle has sacrificed, and cuts too heavy from time to time, that would cause a shortened spindle life. That’s why proper programming training with the machine delivery is critical.

Regarding the pricy image of the High-Speed-Spindle, one observation we have is that it has less to do with spindle life and more to do with its crash-resistant ability. The High-Speed-Spindle is compact and complex, and like any device of this nature, it tends to be less forgiving of mistakes. A survivable or low-cost crash for a simple belt-driven spindle might not be the case for a High-Speed-Spindle.

From service point of view, one should not try to fix a High-Speed-Spindle on the field. It’s typically a cartridge design, so switch out entirely and ship to the factory for repair. For an end user, it is important to ask the machine sales person about the spindle service program in advance, and make sure the high- speed machine or spindle OEM has a repair program in the States instead of overseas.

Jesse Xi Chen
Compumachine Inc.

Posted in Shop Doc Blog
Leave a response | Comments (1)

Should I rebuild my Acme?

Posted on January 5, 2010

Dear Shop Doc,

My Acme-Gridley screw machines have been real money makers over the years, but all that production takes its toll in wear and tear on the machines. Will I be better off doing major repairs to my current Acmes, looking for deals on good used Acmes, or investing in some type of new machinery?

Which Way Should I Go

Dear Which Way,

Acme-Gridley multi-spindle automatics are well designed to be rebuilt or reconditioned, and worn machines can be returned to good running or like new condition by those qualified to perform that type of work. There are different levels of repair to choose from.

For example, you have a 1-1/4” RA6 Acme machine that needs some work. The heart of an Acme is the spindle carrier, which you might start looking at having rebuilt for around $10,000. This includes rebuilt work spindles, new precision spindle bearings, new front and rear retainers and flingers, and new spindle gears, adjusting nuts and keys. The carrier stem is also ground, and fitted to your re-bushed and bored main tool slide. At the high end of your list of options you have a complete machine rebuild, which for all practical purposes is like a new machine. That will cost in the neighborhood of $100,000 to $150,000, depending on your machine and requirements. Compare that to a price tag of $500,000 or more for a comparable new multi-spindle cam machine.

Another factor to consider is that a rebuilt Acme, when properly maintained, can be run hard for 10 years or more before it will require another rebuild. Most single-spindle CNC machines never get that old before they are obsolete or worn out. Acme-Gridley machines come in a wide variety of models, capacities, and vintages. Some machines in service today predate 1950. With sound castings most of these machines are still great candidates for rebuild or recondition, with just a few old models that are obsolete.

A concern for some shop owners today is a lack of experienced machine repair personnel to remove or re-install a spindle carrier, but most qualified rebuilders can offer contracted field service work to do this for you.

Another option popular with some shop owners is look for an inexpensive, worn, late model machine and have it rebuilt. This could be a good option because its mechanical condition is not a concern as long as the castings are in good shape. But even if a machine is examined by experienced personnel when purchasing, the condition of the spindle bearings will largely be an unknown. So it may be a better option to invest money in a machine that you already have and know.

Acmes are well suited for high production part runs, or running a family of similar parts at moderate volumes, but may not be the best choice for small lot runs unless efforts are made to reduce setup times. Attachments are available for Acmes that allow even complex parts to come off the machine complete. In some cases shops are using Acmes in tandem with single-spindle CNC machines, with the Acme blanking the part and then a robot transferring the part to one or several inexpensive CNCs to finish it off. Your production time may be longer, but in the right type of job the dramatic savings on equipment could very well make up for the additional second or two.

Bottom line, your Acmes still have a lot of life left in them, so if you have the right work for them, rebuilding and refurbishing can definitely pay off.

Posted in Shop Doc Blog
Leave a response | Comments (3)

Shop Doc – High Speed Hard Milling

Posted on December 2, 2009

Dear Shop Doc,

We are a mold shop specializing in cutlery molds with large cavities and tiny details, usually from 420 stainless steel hardened to 48 to 50HRC. Some corner radii are as small as 0.008”. For years, we have been using EDM machines to burn our hardened cavities and cores—a very time consuming process. I’ve heard that high-speed hard milling is the new process for mold-making. Can it really replace our EDM?

-Make Us Faster

Dear Make Us Faster,

You are right. High Speed Machining (HSM) has made a huge impact on the mold-making process in recent years. HSM is a machining process using smaller tools with high rpm and feed-rate to perform faster, lighter cuts. Surprisingly, tackling hard milling is simplified using this high-speed technique. Conventionally, cutting hardened tool steel with large tools generates a lot of heat that breaks down the end mill rapidly, making milling an impractical option. Hence the EDM (Electrical Discharge Machining) became the standard process to machine hardened steel. With HSM however, every cut is small, light and fast, minimizing thermal effects and lowering heat transfer to the end mill, so the tool will last to finish the cavity. Together with the advances in cutting tool technology, HSM Hard Milling has become a very practical alternative with major savings in time and cost.

To determine whether HSM can replace your EDM process, you must study the characteristics of your mold cavities. Obviously a 90 degree sharp internal corner can only be accomplished with EDM. For big cavities, milling is always faster than EDM. As for small features, the recommended rpm goes up proportionally as the end mill radius goes down. Small radius alone is not the issue. What makes hard milling difficult is when the end mill becomes too slim and therefore lacks strength to support its cutting. It is the ratio of the end mill diameter to neck length that is important. When hard milling with end mills under 1/4”, the rules of thumb are: a 1:3 ratio is considered stubby, 1:5 is practical, 1:8 is difficult and requires a lot of careful programming, and 1:10 probably is the limit.

Having said that, please bear in mind that HSM also compliments the EDM process. Mold cavities typically consist of free-form surfaces that are machined with ball end-mills, and the “cusp” between paths decides the final surface finish. For example, a 1/8” ball end mill with 0.003” step-over will produce a “cusp” height of 18 micro-inches. A silky smooth surface finish requires densely packed tool paths that make machining at a high rpm and feed-rate essential for cycle time reduction. This is true for both hard milling and electrode machining.

When you are considering HSM for your shop, please be aware of the upfront costs associated. A true high speed machine costs more than a conventional CNC machining center. They typically have bridge construction and are equipped with high-speed motor spindles with anywhere from 20,000 rpm to 50,000 rpm. Other critical features to look into include advanced CNC with look-forward capabilities, large storage, Ethernet connection and thermal control. Last but not least, it is the human factor, from process planning and tooling selection, to programming and setup that separates the men from the boys in HSM implementation.

-Jesse Xi Chen
Jesse Xi Chen Compumachine Inc.

Posted in Columns, Shop Doc, Shop Doc Blog
Leave a response | Comments (2)

Shop Doc – Vexed Hex

Posted on December 2, 2009

Dear Shop Doc,

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 programa 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

Posted in Shop Doc, Shop Doc Blog
Leave a response | Comments (6)

“Twisted” while Broaching 400 Series Stainless

Posted on November 22, 2009

I’m using a quarter inch hexagon broach to create a quarter inch deep form in 400 series stainless steel. However, the form is twisted, somehow spiraling from one end to the other. I don’t see any type of adjustment available on the broach holder. How can I get rid of the twist?

Spinning out of Control

Dear Spin Doctor,

The solution to removing the twist from your form is easier to find when you understand the nature of the problem. The sides of the broach include a relief angle greater than the angle of the rotary broach holder so it will not interfere with the part. The broach is held in the holder at a one degree angle. The rotary broach is designed to cut a form into the part using a cutting edge with contact points that are constantly changing. The center of the cutting edge is always kept in line with the axis of the part. As the contact point continually changes, separate chips develop in each corner of the form. As these chips increase in size, pressure is absorbed by the broach tool and tool holder. This resistance against the broach holder spindle and bearings may cause the broach to drag slightly against the material being broached. The sides of the broach cannot hold it straight because they have a greater relief angle for clearance and sometimes a spiral will develop along the length (depth) of the form.

At first you may have noticed that the form appeared smaller at the bottom. What you are really seeing is the sides of the form following this spiral path. Although there may be a slight twist, the part may still be within specification. Technicians will often recommend that you broach to the high side of your tolerance for this reason.

Work piece material can also affect this condition. Some materials could be too tough or too hard for the capabilities of the tool holder. Your material (400 series stainless) is difficult to broach, and may result in poor tool life. The combination of a dulling tool and hard material increases the thrust required to broach which increases drag thus increasing the spiraling of the form. However, at this small size and form, I’m hopeful that there are a few things you can do to try to reduce or eliminate the spiral.

First of all, good broaching practice is to check your tool holder and broach to make sure they are on center. If not, re-center the tool holder. If you are using an adjustment free model, make adjustments on the machine to assure that the broach is on center with the part. It is also good to check and make sure the pre-drilled hole is on center. Next, anything you can do to reduce the pressure caused by chip accumulation will help. Check your pre-drill diameter. Can you make it larger? The recommended pre-drill for a hexagon is 1.035 times the across-the-flat dimension. The standard quarter inch broach is likely .253 inches, and the pre-drill should therefore be .261 inches. If your customer will allow it, make the pre-drilled hole larger. This will reduce the required thrust. Have you checked your speed and feed to compare them to the recommended settings? If your tool is moving too slow, the chip may not curl over as readily as is necessary and this could result in added pressure. Increase the feed rate to improve the chip flow.

Finally, if the above recommendations do not help or are not practical, reverse the direction of the spindle at half of the depth. This will drag the spiral in the opposite direction and can reduce the overall deviation by half. Hopefully, these suggestions will help you make a turn in the right direction.

Peter Bagwell
Slater Tools Inc.

Peter Bagwell is an engineer at Slater Tools Inc., which specializes in rotary broaching tools. For more information go to www.slatertools.com

Posted in Shop Doc Blog
Leave a response | Comments (5)