SBN Finishing Series Reference Information

Usage Information

ONLY with Dapra's New SBN tool system can you achieve high-quality finishes AND use a Ball Nose insert twice! Achieving this cost savings requires adhering to a few simple application guidelines (see Diagram D1 below for examples):

MOST IMPORTANT! – Your SBN insert has a full 360 degrees of metal-cutting surface, but it must be used only 180 degrees at a time. All cutting must be kept at or below the insert center line to allow the cutting edges to perform correctly. Any attempts at cutting above the insert center line may result in failure, including insert and/or cutter damage.

Finishing – Use your SBN insert for finishing, preferably with a top-down program. In other words, start your cutting at the top of a part and profile around, slowly working your way down to the bottom (water-line programming/Z-level finishing). A raster-pass (lacing) cut may be used, but take care to leave less than .010" finish stock to avoid cutting above the insert center line. Best performance is achieved in tapered-wall work, but straight-wall finishing can be accomplished by using ONLY the "top-down" approach detailed below (see Diagram D1).

Semi-Finishing (Light Roughing) – Use your SBN insert ONLY with a top-down approach when semi-finishing or light roughing. Start your cutting at the top of a part and profile around, working your way down. Do NOT attempt to lace cut or raster, as rubbing on the back side of your SBN insert may occur (cutting above insert centerline), ruining the surface finish and potentially damaging your SBN insert.

Roughing – Your SBN insert is NOT suitable for roughing.


SBN Usage Information

Technical Considerations


CAUTION: Modern metal cutting techniques involve the potential use of very high operating parameters (speeds, feeds, depths of cut, etc.). This creates the potential for flying chips and debris, and can also create tool breakage due to a variety of causes. As such, any metal cutting operation should be executed in a completely enclosed (shielded) environment to protect against injury from flying objects. Dapra does not assume responsibility for any loss, damage or expense incurred in any use or handling of our product after purchase. Grinding produces hazardous dust. To avoid adverse health effects, use adequate ventilation and read material safety data sheet first. This product contains a chemical known to the state of California to cause cancer.

Feed, Speed and Diameter Compensation

Table 1: Effective Cutting Diameter (ECD)

Depth of Cut
Insert Diameter   .005 .010 .015 .025 .035 .050 .100 .125 .150 .200 .250
.500 .099 .140 .171 .218 .255 .300 .400 .433 .458 .490 .500
.750 .122 .172 .210 .269 .316 .374 .510 .559 .600 .663 .707
1.000 .141 .199 .243 .312 .368 .436 .600 .661 .714 .800 .866

Figure 1

  1. Select diameter of tool to be used.
  2. Determine Depth of Cut (DOC) to be used.
  3. Refer to Figure 1 and Table 1 to find the Effective Cutting Diameter (ECD).
  4. Refer to Feed and Speed chart on back cover to select the surface footage to be used (SFM).
  5. Calculate RPM using the ECD and SFM. (SFM x 3.82 / ECD = RPM)
  6. Refer to Table 2 to determine Feed Rate Adjustment (FRA).
  7. Refer to chart on back cover to select Feed per Tooth (FPT). Calculate Inches per Minute (IPM). (RPM x FPT x 2 x FRA = IPM)

* For the cuts that are not strictly tip-cutting, but will use both the tips and sides of the SBN insert, pick an effective cutting diameter in between the ECD in the chart and the actual diameter of the insert. For example: If the ECD comes out to .210" with a .750" diameter insert, use .480" as your ECD when calculating RPM.

Table 2: Feed Rate Adjustment (FRA)

These feed rate multipliers are for applications involving tip-cutting only.
For applications including side-cutting or slight/draft angles, lower the multiplier by 20-50%.


Insert Diameter
Depth of Cut   1/2" 3/4" 1"
.005 5.0 6.1 7.1
.010 3.6 4.4 5.0
.015 2.9 3.6 4.1
.020 2.6 3.1 3.6
.025 2.3 2.8 3.2
.050 1.7 2.0 2.3
.075 N/R 1.7 1.9
.100 N/R N/R 1.7

Use multiple above to calculate adjusted feed rate.


Concern Possible Cause Solutions
Insert wear at tip
  • Not enough chip load
  • Verify correct speed and feed
  • Increase feed rate
  • Decrease RPM
  • Increase DOC
Insert wear appears high (flank wear)
  • Not enough chip load
  • Surface footage is high
  • Incorrect grade or coating
  • Verify correct speed and feed
  • Increase feed rate
  • Decrease RPM 
  • Consider different insert
Insert chipping
  • Surface footage is low
  • Incorrect grade or coating
  • Using CB style insert incorrectly
  • Feed too high
  • Verify correct speed and feed 
  • Increase spindle speed
  • Decrease feed rate 
  • Change insert selection
  • Decrease DOC
  • Use N style insert
Built-up edge on insert
  • Low surface footage
  • Light chip load (feed per tooth)
  • Incorrect coating
  • Verify correct speed and feed
  • Increase cutting speed
  • Increase feed rate
  • Select different coating
Poor finish/chatter
  • Cutter hung out too far
  • Excessive runout
  • Use Carbide Core cutter body
  • Reduce tool gage length
  • Check tool holder wear
Tool shank breaks
  • Tool pressure too great
  • Fatigued cutter body
  • Decrease DOC
  • Reduce tool gage length
  • Decrease feed rate

Recommended Cutting Speeds & Feeds

Recommended Cutting Speeds & Feeds
Click chart image to enlarge

Insert Grade Selection

Spherical Ball Nose Finishing Insert Grade Descriptions
(Base Grade)
with Coating Description Specifications
UC   Micro-grain tungsten carbide with high edge strength and good toughness. Good for machining steels, stainless steels, high-temperature alloys, cast iron and nonferrous materials. (C-2), (K10)
  GLH Premium high-temperature and high-hardness coating. Optimum performance and wear resistance in virtually all materials makes this an extremely versatile and simple grade choice. 3600 HV, 2000˚ F, .2 Co