External grooving

For grooving, high productivity is the goal. External grooving is generally less demanding than parting-off, and because of this, process security is easier to achieve. This allows the focus to be moved to improving productivity, especially for wide grooves since they take more time and make a bigger impact on the component’s total machining time than small grooves.

External grooving methods

For deep grooves, process security can be a challenge due to the long overhangs required, difficulties with chip evacuation, and difficulties ensuring coolant access to the cutting edge. Single cut grooving is the most economical and productive method of producing grooves. However, if the width of the groove is larger than the width of the insert, multiple grooving plunge turning, ramping, or profiling can be used to make the groove. For external grooving, a tool with high-precision coolant is First Choice.

Application Tips: How to Apply External Grooving

Single cut grooving

Single cut grooving is an economical and productive method of producing grooves. When applying a single cut, these are the aspects to consider:

• If surface finish is of high importance, use insert geometry with Wiper technology
• Make sure you use an insert with tight tolerances and the correct corner radii and width, ground inserts are recommended (e.g., -GF)
• If you work with mass production, use an insert with the correct profile and chamfer. If not found in standard assortment, it is worth investing in Tailor Made inserts

Roughing wide grooves

The most common methods for producing wide grooves or for turning between shoulders are:

• Multiple grooving
• Plunge turning
• Ramping

All three methods are roughing operations and must be followed by a separate finishing operation.

The rule of thumb is: if the width of the groove is smaller than the depth, then use the multiple grooving method; if the reverse is true, then use plunge turning. For slender components, the ramping method may be used.

Multiple grooving

• For deep wide grooves (depth greater than width)
• Flanges left for final cuts (4 and 5) should be thinner than insert width (CW -2 × corner radii)
• Increase feed 30–50% when machining flanges
• First Choice geometry is -GM

Plunge turning

• For wider and more shallow grooves (width greater than depth)
• Do not feed against shoulder
• First Choice geometries are -TF and -TM

Ramping (turning/profiling)

• Best chip control
• Minimize radial cutting forces and notch wear
• First Choice geometries are -RO and -RM

Turning and External Grooving

Turning with a parting and grooving insert

• When side turning, use a depth of cut (ap) larger than the insert corner radii
• Wiper effect − feed rate per depth of cut (fn/ap) must be relatively high to ensure a slight deflection of tool and insert. This provides a clearance between the cutting edge and machined surface
• Too low fn/ap causes tool rubbing, vibration, and poor surface finish
• Max. ap = 75% of insert width

The diagram shows surface finish for parting and grooving inserts in comparison to a TNMG insert with a 04 or 08 corner radius.

Turning a groove

When side turning, tool and insert must bend. However, too much bending can cause vibration and breakages:

• Thicker blade decreases bending
• Shorter overhang (OH) decreases bending (δ)
• Avoid turning operations with long and/or thin tools

Shorter overhang decreases bending sideways

Undercutting and external grooving

A grinding or threading operation is required on many components. Clearance is needed to grind or thread into a shoulder; therefore, we recommend the use of inserts dedicated to undercutting operations. For example: T-Max® Q-Cut and CoroCut® 1-2