Cutting Tool Engineering
August 2012 / Volume 64 / Issue 8

Groove milling

By Susan Woods, Contributing Editor

While it may have different names, groove milling can be an effective way to perform slotting and slitting.

As we all know, industry terms mean different things to different people. This is the case with “groove milling.”

“Words and terms are intermixed and overplayed no matter how you look at it,” said Duane Drape, national sales manager for HORN USA Inc., Franklin, Tenn. “The difference between groove milling and slot milling or slitting or anything along that line is hard to define.”

Courtesy of HORN USA

A HORN groove milling tool creates square, linear grooves. The same tool was used to bore mill the largest bore (including the face), groove mill the two grooves on that diameter and bore mill a smaller diameter from the bottom up.

William Durow, applications and development project coordinator for Sandvik Coromant Co., Fair Lawn, N.J., agreed that groove milling is basically slotting and slitting. “It depends on who you talk to, what industry they are in and, frankly, who they were taught by. But groove milling and slotting are fundamentally the same thing,” he said. Sandvik Coromant offers a full line of CoroMill indexable-insert groove mills.

Michael Trimble, product manager for Vargus USA, Janesville, Wis., said “groove milling tools to us are slotting tools that can run at higher speeds and feed rates than traditional slotting tools, such as Woodruff cutters.”

Turn Instead

A groove can be created via turning on a lathe or groove milling. “If you can produce the groove on a lathe, you do it,” said Matthew Schmitz, national product manager—GRIP products for Iscar Metals Inc., Arlington, Texas, which offers groove mills as part of its TANG, GRIP, CHAMSLIT and MULTI-MASTER products. “In nearly every case, it will take more time to generate that same groove on a mill than a lathe.”

Schmitz also noted that if the groove has a shape other than parallel sidewalls, the task becomes difficult on a mill and will likely require a special tool, which adds cost.

Courtesy of Sandvik Coromant

Sandvik Coromant’s CoroMill 329, typically used for deeper, narrower grooves, offers a DOC from 100mm to 160mm (4 " to 5 ") and has a width from 2.5mm to 4mm (0.098 " to 0.157 ").

“There are only a handful of reasons to use a mill for a groove rather than a lathe,” he said. “These include the shape or size of a workpiece, machine capability or capacity in a given shop, to gain chip control, to eliminate an additional setup and to control workpiece feature tolerances without the concern of an additional setup.”

Also, because groove turning uses a single-point tool, Schmitz feels it is more accurate.

Drape doesn’t necessarily agree that groove turning is more accurate—it is definitely application specific—but said with “groove milling you have a rotating tool so you will get more of a scalloped-type finish.”

Notable Inserts

Groove milling tools are available as solid carbide, with a replaceable head (or insert) that screws on the end of the shank or with indexable inserts that fit into pockets on the tool body.

“We offer solid and insertable based on a diametric requirement,” Drape said. When groove milling a small ID, an insertable tool might not fit. “We typically switch to insertable at 10mm in diameter and up,” he said.

As the diameter increases, the cost of solid-carbide tools gets progressively larger, which is where inserts come in. “The problem you can potentially run into with an insertable tool is there is a fine line where the accuracy of an insertable cannot be as good as a solid,” Draped added. “Because you have replaceable components, you can’t maintain the same accuracy.”

When the diameter is large enough, Vargus’ Trimble indicated that indexable-insert groove mills are more economical. Say a solid-carbide tool costs $150 vs. $150 for a tool body and $25 for a replaceable head (insert) with three or six teeth. If the solid-carbide tool produces 1,000 grooves and the insertable tool produces 1,000 grooves, the solid-carbide tool will cost more over the long run because the user has to pay for a completely new tool once it’s worn. (Vargus doesn’t recommend resharpening.) For the insertable tool, he only has to pay $25 for each replacement head. Vargus offers Groovex solid-carbide and indexable-insert groove milling tools.

Whether solid or insertable, groove mills create simple linear and circumferential grooves—a square bottom or half-round groove such as for internal circlip or O-ring grooves.

Insertable tools are more flexible in terms of grades and geometries because the head or inserts can be changed. These tools are used for angled grooving, chamfering, parting off and generating gear teeth profiles, Woodruff keyways and T-slots, just to name a few applications.

Add threading to the list. “Thread milling is nothing more than helical grooving,” Drape said. “A thread is a groove that commonly has 60°, 55° or 30° included sidewalls. It is a constant groove that is moving up a component. You have to use different-shaped tools but the process is the same.”

Making a Slit

Slitting cutters are applied to create narrow, square grooves up to a couple inches deep. “It is all relevant to the size of the groove, but it is usually deeper than the width of what you are grooving,” Drape said.

Iscar differentiates slitting and slotting cutters by noting slitting cutters are blade-type cutters that accept inserts that resemble parting or grooving inserts most commonly applied when turning. Slotting cutters are also blade-type cutters, but they hold inserts that resemble those typically found in milling cutters.

According to Iscar, slitting cutters are generally used when the width of the groove is less than ¼ ", while slotting cutters are for making wider grooves. However, there can be some overlap.

Courtesy of Vargus USA

Vargus USA’s Groovex GM Slot groove milling tools are available for creating groove widths from 1.2mm to 4mm and up to 3.25mm deep.

“Because the slitting cutter is such as expensive tool—you have to mount many expensive inserts—you use it only when you absolutely need to,” Schmitz said. “But for a long, deep groove that runs the length of a shaft, it might be more economical to use a slitting cutter [rather than a slotting cutter].”

For example, a 6 "-dia. slitting cutter that accepts 12 single-edge inserts requires $168 worth of inserts at $14 each. If the cutter body is $800, it would cost almost $1,000 just to set up the tool. Using a cost per edge to keep the comparison relative, a slotting insert with four cutting edges for a 6 "-dia. slotting cutter costs about $4.30 per edge × 16 inserts, or $68.80. The cutter body costs about $1,500. While the initial cost is greater, each insert index for the slotting cutter is $100 less compared to the slitting cutter, according to Schmitz.

But, in this example, the slotting cutter has half-effective teeth. In other words, there are only eight effective cutting edges (opposed inserts), which is 20 percent less effective than the comparable slitting cutter. And the slotting cutter generally requires a reduced chip load compared to a relative slitting cutter.

“So you always have to weigh the advantages and disadvantages of slitting and slotting to see which cutter will fit your environment best,” Schmitz said. “The tooling cost of the slitting cutter may be more in the long run, but some will easily justify the cost with its performance. Others will slow down the machine performance and keep the economics in the overall tooling cost.”

Get out the Chips

Chip evacuation is a concern in any metalcutting operation, but it is critical when grooving because chips are more prone to being trapped inside a groove and being recut. However, several tool design factors can aid chip evacuation when grooving.

Groove milling is an interrupted cutting operation, so the chips typically break into manageable sizes. Groove turning can produce long, stringy chips.

Courtesy of Iscar

Iscar’s CHAMSLIT groove milling tool is an economical slitting tool but is used only for making shallow grooves, according to Iscar. It can produce a groove up to about 1/8 " deep and from 0.047 " to 0.158 " wide. It can produce internal and external grooves.

A staggered-tooth, or half-effective, cutter design helps break chips. “In the case of our slotting cutters, we have opposing, or half-effective, cutters,” Schmitz said. “So if you have 10 inserts in the cutter, only five are effective. One insert cuts the top side of the groove while the insert behind it cuts the bottom (or opposing) wall, which helps with chipbreaking. It also produces a narrower chip than what would be produced with a single wide insert, enhancing chip evacuation.”

Generally, a cutting edge on a slotting cutter is oriented at 90° to the slot wall. The angle of the cut sends the chip into the sidewall.

Iscar’s tools feature the cutting edge orientated at a different angle. “It is not 90° to the slot,” said Hassan Naraimhan, national product manager for indexable milling cutters at Iscar. “It could be 70° or 60°, so that deflects the chip from the slot surface so it doesn’t damage it. The angle actually draws the chip away from the slot wall.”

Also, most groove mills have through-coolant capability for chip flushing.

Milling deep grooves can also be challenging. “As the depth of the groove increases, your cutter diameter needs to grow exponentially,” Schmitz said. “So if the groove depth is increased by 1 ", the diameter of your cutter will increase at least another 2 " in diameter or more.”

Sandvik Coromant’s Durow noted that heat-resistant superalloys, such as Inconel, create a lot of heat during machining. “When you cut a deep, narrow groove, there is no place for the heat to go so it goes back into the cutter, which will inevitably give you poor and unpredictable tool life,” he said. “You will need to take multiple shallow cuts—at least 15 to 25 percent the diameter of the cutter for each pass—until you reach the desired depth. This will help prevent some of the heat going into the tool.”

Tricks of the Trade

Feed rate control plays an important role in grooving. “Feed rates are largely dependent on the width of the slot and tool,” Schmitz said. “If you have a very narrow slot, you need to consider the strength and rigidity of the tool required for the groove.”

Courtesy of Sandvik Coromant

Sandvik Coromant’s CoroMill 327 is for grooving small holes or creating circlips or O-ring grooves. Geometries are also available for thread milling. The 327 goes down to 9.7mm (0.382 ") in diameter and provides a limited DOC.

When using circular interpolation to perform groove milling, feed rates are decreased when cutting IDs and increased when cutting ODs, according to Durow.

“Your programming has to be a bit different when grooving internally vs. externally,” he said. “People need to remember to program on the centerline of the tool. They must understand the danger of chip thinning and program accordingly so they do not underfeed or overfeed their tools.”

For an internal groove in a hole, the programmed feed rate is often that of the feed rate at the center of the hole. The feed rate calculated at the periphery is different and the result is often an excessive feed rate for the cutter. The feed rate, then, should be decreased to allow for the difference.

As for external grooves, it is just the opposite. Again, the feed rate calculated at the periphery is different but the result is often too low of a feed rate for the cutter. The feed rate should be increased to allow for the difference.

Iscar’s Schmitz noted one tooth should be engaged at all times when groove milling. “You always want the spindle under load, and that applies to any milling operation,” he said. “If you have a period where the spindle is not under load, you could experience spindle whip (typically accompanied with a hammering sound during the cut), damage the spindle and cause tool failure. Therefore, if you have a shallow groove, it would be in your best interest to have a fine-pitch cutter so you always have the cutter under load.”

One final recommendation from HORN is to enter the groove with a ramp angle of 45° to 180° to achieve the maximum DOC. A radial entry of the milling cutter creates a long contact angle, which leads to vibration.

“The fastest method to get to the groove depth is to take the tool directly to the groove depth.” Drape said. “But you inherently put chatter into the workpiece if you do that. So we recommend that from the time you make your first contact with the workpiece to the point where you get to full depth, you should have traveled a minimum of 90° of the workpiece diameter. If you are still getting chatter because of other factors, such as weak fixturing or long tool projection, take 180° or even 360° to reach full depth. You actually reduce the workpiece pressure and that can help eliminate chatter.” CTE

About the Author: Susan Woods is a contributing editor for CTE. Contact her at (224) 225-6120 or


(888) 818-HORN

Iscar Metals Inc.
(877) BY-ISCAR

Sandvik Coromant Co.

Vargus USA
(800) 828-8765

CUTTING TOOL ENGINEERING Magazine is protected under U.S. and international copyright laws. Before reproducing anything from this Web site, call the Copyright Clearance Center Inc.
at (978) 750-8400.