BACK

WIPER INSERT

What is a Wiper Insert?

The wiper insert is designed with a wiper edge that is situated where the straight edge meets the corner radius. breakers, the surface finish does not deteriorate even if the feed rate is doubled. Machining at high feed rates improves cutting efficiency.

Improving Finished Surface Roughness Under the same machining conditions against conventional breakers,but with the feed rate increased, the surface finish of the workpiece can be improved. Improving Efficiency High feed rates not only shortened machining times but also makes it possible to combine roughing and finishing operations. Increased Toollife When a change to high feed conditions is made, the time required to cut one component is decreased, thus more parts can be machined with each insert. In addition, the high feed rate prevents rubbing,therefore, delaying the progression of wear and increasing the toollife of the insert. Improving Chip Control Under high feed conditions, the chips generated became thicker and are more easily broken, thus, chip control is improved.

Wiper insert + High feed (The feed rate is doubled.) Finished surface Same surface roughness = Standard insert + The conventional feed condition *Please use wiper inserts at high feed rates. <Ex>The surface roughness does not deteriorate even when the feed rate is doubled (0.30.6)!

Wiper insert + machining at high feed rates Reduced machining time (per workpiece) Increased number of workpiece(per definitive time period) Improving chip control Wiper insert + machining at conventional feed rates Eliminating the finishing step (Separate roughing and finishing steps ? Single-step machining) Reducing cost Increased productivity Avoiding Line-Stop The realisation of downward costs!!

The Estimation of finished surface roughness in using a wiper insert

The wiper effects on external machining, boring and facing. *The surface roughness when machining at corner R or taper angle over 5°, is same quality as machining when the standard inserts.

Special attention is not necessary when using CNMG·WNMG·CCMT types

Non Restriction for Holder

Non Necessity of Adjustment of the Machining Programme

Special attention is necessary when using DNMX·TNMX types due to the special top face geometry

Restriction for Holder Use a holder with an end cutting angle of 93°to improve wiper efficiency. A holder with a cutting edge angle of 91°can marginally improve wiper efficiency (see the figure below), however, there is no wiper efficiency with other end cutting angles (60°, 90°, 107°etc.).

Necessary Adjustment of the Machining Programme When machining error occurs, please adjust the machining program. (The DNMX·TNMX types are not based on the ISO/ANSI. Please refer to the next page.)

Adjustment of machining programmes for DNMX·TNMX types

Basic Process) Adjusting Toward Z-axis and X-axis Adjusting the differential between a standard insert and Z-axis / X-axis.

A) Adjusting a Taper *It is a prerequisite condition in order to operate a correct basic process. Adjust the relief angle toward the normal line. (Note) Adjust the drive-in angle toward the normal line when the part where the adjust number in minus (=60°~70°) is not machined completely.

Classification

Nose Radius	Taper Angle °
	-25~ -15	-10	-5	0	5	10	15	20~35	40	45	50	55	60~65	70	75~85	90
1.2	0.04	0.03	0.01	0	0.02	0.03	0.04	0.05	0.04	0.04	0.02	0.01	-0.01	0	0.01	0
0.8	0.03	0.02	0.01	0	0.01	0.02	0.03	0.04	0.03	0.03	0.02	0	-0.01	0	0.01	0
0.4	0.02	0.01	0.01	0	0.01	0.01	0.2	0.02	0.02	0.01	0.01	0	-0.01	-0.01	0	0

B) Adjusting a Corner R *It is the prerequisite condition to operate the basic process. Adjust the work diameter to the same as the taper to prevent over-cut.
The value of adjusted work R = Work R + the adjusted quantity *No adjustment of the nose radius required in this case.	Ex): In the case of machining a corner with a radius R 2.0 when using an insert with a nose radius R 1.2.
The Easy-to-correct Method In correcting nose radius: It is not necessary to adjust the machining program, however, machining error can occur within max. ±0.03mm due to correcting by approximation number.

Nose Radius Correction Input the correction number of each nose radius.
The value of corrected nose radius = approximation *No adjustment of the nose radius required in this case.	Ex): In the case of machining a corner with a radius R 2.0 when using an insert with a nose radius R 1.2.
Others) The correction value is the same for both DNMX and TNMX. Descriminate between them only by the different nose radius.