Browse: Home / Shop Doc Blog

Shop Doc – Custom Macro programming

Posted on August 10, 2010

Today’s Machining World Archives August 2010 Volume 06 Issue 06

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

Posted in , , ,
Leave a response

Shop Doc – Micro Beginnings

Posted on June 25, 2010

Dear Shop Doc,

I have recently been asked if my shop does “micro” machining. I’ve done some work on small
parts recently, but I’m not exactly sure what is meant by “micro.” Any thoughts?

Small Beginnings

Dear Small Beginnings,


One of the problems with the term “micro” is that it is often used to defne a very small portion of a wide array of categories. Maybe you’ve been to a microbrewery or have a computer that uses a microprocessor. In each case, the prefx or adjective “micro” defnes a small-scale or very small feature of the original term. To date, the term is loosely used in machining to refer either to the exact measurement of the parts, such as in microns, or to a small range of work, in the neighborhood of 1 mm or less.

In May 2010, I posed a similar question to exhibitors and attendees at MM Live—the Micro and Precision Manufacturing Event for North America, in Cincinnati, Ohio. As an exhibitor myself, I thought micro meant sizes under .050”, as this was the smallest tool in our catalog and very near to the 1 mm dimension. I often referred to parts from this diameter up to .500” diameter as Swiss, so everything smaller I considered micro. A large number of attendees defned micro as being smaller than a certain dimension.

Some said micro meant parts smaller than 8 mm or .250”, or 1 mm. Kyocera’s booth advertised a .250” dimension on their sign. However, when I asked them about it, they explained that although they make a wide variety of small tools, the ones they considered to be micro sized were really those .125” or smaller.

Photo from JMMedical

A few attendees believed the term “micro” referred to parts that were smaller than the human eye can see. The MM Live show had a wide of variety of these parts on display, and it seemed that every other booth had a microscope or magnifer of some type to help you see their wares. One of the most intriguing answers to defne micro came from an exhibitor at Makuta Technics Inc. He said they use the term micro not to refer to a part’s size, but more exclusively to the feature’s size. You may have a part not considered to be a micro machined part, but if the features and tolerances are small enough, it may require what is commonly known as micro machining. This can lead to a lengthy discussion about tolerance, and if a part with +/-.001” variance can be classifed the same as a part with +/-.000010”.

I believe micro machining refers to parts with an overall size or feature in the neighborhood of 1 mm. The features are not as large as common Swiss machined parts, nor as small as a nanometer (one billionth of a meter), but you will still need some form of glasses to make out the details. My suggestion is to not split hairs, but just state the size of the features you are comfortable making. The number of people who agree on the defnition of the term “micro” is very small.

Peter Bagwell
Slater Tools Inc.

Peter Bagwell is an engineer at Slater Tools Inc. in Clinton Township, Mich., which specializes in rotary broaching tools.

Posted in , , , ,
Leave a response | Comments (1)

Shop Doc – Why are there big differences in price from one rebuilder to the next?

Posted on May 18, 2010

With Noah Graff

Today’s Machining World Archive: May 2010 Vol. 6, Issue 04

Dear Shop Doc,

I recently decided to shop around for quotes to rebuild my 1-1/4” RB8 Acme-Gridley.
I sent the RFQ out to three different rebuilders and received three very different prices.
Why is there such a big difference in price from one rebuilding company to the next?

Confused in Cleveland

Dear Confused,

This is a very common situation in our industry today, but a little knowledge can go a long way towards helping you evaluate quotes for your rebuild projects.

Many companies mistakenly assume that the term “rebuild” means the same thing to every supplier. This is not the case, and there can be a great deal of difference between machine tool rebuilders as to what constitutes a machine rebuild. These differences have a substantial impact on what it will cost a rebuilder to do the job, what will actually be done to your machine and what condition your machine will be in when you get it back. For Rebuilder A, it may be standard practice to replace every bearing in the machine, and just about every part with a new part, while Rebuilder B might have the practice of evaluating all of the current parts in the machine and then reusing the ones that pass inspection. One rebuilder may always strip the machine completely down to the castings, inspect them carefully for damage or needed repairs, then repaint the machine inside and out, while another rebuilder may consider that to be more work than necessary.

The differences in opinion about what work must be done when “rebuilding” a machine is the main cause of the wide range of price quotes. Some of the better rebuilding companies offer a written procedure detailing what they do when they rebuild a machine. Many also offer what is commonly called a machine “re-condition,” basically a mini-rebuild, which is also subject to discrepancies from company to company regarding what work is included. A written procedure for machine re-conditioning may also be available.

A great way for a customer to deal with these discrepancies is to write their own detailed outline for what work they want to be performed, and use that as the platform for every rebuilder to bid on. Be sure to include as much detail as possible and outline what is acceptable to you with regard to reusing any current parts on the machine. Also, consider if you want the electrical system to be addressed, if there are attachments that will need to be rebuilt or added, and if there are any other upgrades such as adding a PLC, that need to be outlined. The more detail you have going into the quoting process the more accurate your quotes will be, and the fewer surprises you will have down the road.

David Johnson
Champion Screw Machine Engineering, Inc.

David Johnson is the Rebuild Manager for Champion Screw Machine Engineering, Inc. in Wixom, Mich. He can be reached at djohnson@championscrew.com

Posted in ,
Leave a response

Shop Doc – Tangled Up in Tennessee

Posted on April 23, 2010

Today’s Machining World Archive: April 2010 Vol. 6, Issue 03

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

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

Posted in , , ,
Leave a response | Comments (1)

Shop Doc – Stringy Aluminum Chips

Posted on March 30, 2010

Dear Shop Doc,

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 distributor. He can be reached at dmurphy@remsales.com.

Posted in
Leave a response | Comments (1)

Shop Doc – When to go Hydromat

Posted on March 16, 2010

Dear Shop Doc,

We are a new job shop looking to add some equipment. We are wondering whether we should invest in used rotary transfer machines like a Hydromat Legacy or stick with multi-spindles. When would we want to use a rotary transfer machine versus the traditional multi-spindle?

When to go Hydromat

Dear When to go Hydromat,

Great question. While rotary transfers and multi-spindles can produce the same parts, a good used Hydromat Legacy will cost from $80,000 to $180,000, while a used multi will cost less than half of that. So it’s important to figure out which machine suits your specific job.

The following are some important factors to consider when choosing which machine is best suited to accomplish the most productive end result. This is not limited to just the Hydromat or multi-spindle. In some cases a CNC Swiss may be a viable alternative.

Quantity of parts: Hydromats are ideal for high volumes. For jobs making less than 20,000 pieces, the multi-spindle is the right choice. This is the case even for complex parts, because with a few exceptions they are easier to retool than a Hydromat Legacy. This is because there is more open space in the machine, which makes the spindles easier to access.

Complexity of parts: For machining complex parts that are hard to hold in collets or chucks yet can be run complete by holding onto the bar in a multi-spindle machine, it makes sense to use a multi-spindle, because there is more holding surface to grip.

But Hydromats are more versatile, because they can have 10, 12 or 16 tool spindles horizontally, or up to eight vertically. For example, machining off-center holes, radial or axial, on center holes, drilling four holes radially and not all the way through, or machining an eccentric dimension on both sides of a shaft, would be easy on a Hydromat. But doing those operations on a multi-spindle would likely be quite difficult and would add significant cost because of high cycle time.

Shape and type of material: The Hydromat is more versatile for machining different material shapes than the multi-spindle because the bar remains stationary rather than rotating. For example, machining hex material on a multi-spindle machine produces an extraordinary level of noise, while on the Hydromat there is very little or no increase in noise. The type of material you are machining should not make a difference when choosing between the multi-spindle and a Hydromat, as long as the material removal is within the limit of the motors on the Hydromat.

Tolerances: In most cases both multi-spindles and Hydromats hold comparably tight tolerances. One big advantage with a Hydromat is that it can turn a part around and machine the other end with a number of features as long as there are free stations. Back-finish on multi spindles with close tolerances is more difficult but usually required on one or more operations after it is partially finished.

However, multi-spindles have an advantage when you need to make a number of recesses (grooves) with a tight concentric requirement. In this case, it is more difficult to hold on the Hydromat, especially when the grooves are larger. It is hard to beat a form and shave tool, if it is in capable hands.

It’s also important to note that a lot of shops have been successful in combining both types of equipment by pre-machining or roughing parts to a semi-finished stage on a multi-spindle and then finishing them on a Hydromat.

Hydromat Rotary Transfer Machine (Photo from Griner.com)

Posted in , , ,
Leave a response

Shop Doc – 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
Leave a response | Comments (2)

Shop Doc – High Speed Hard Milling

Posted on January 27, 2010

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 , ,
Leave a response | Comments (3)

Shop Doc – 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
Leave a response | Comments (3)

Shop Doc – Vexed Hex

Posted on December 3, 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 ,
Leave a response | Comments (6)

Page 1 of 212