DTB Roughing Series Reference Information


Technical Considerations


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 products after purchase.

Grinding produces hazardous dust. To avoid adverse health effects, use adequate ventilation and read material safety data sheet first.


Your double-sided DTB series inserts are very thick, providing outstanding strength and superior tool life in operation. With this increased thickness comes the requirement that the feed per tooth (FPT) not exceed the clearance the insert allows. In general, it is recommended to initially not exceed an FPT of .025". Under certain circumstances (lighter DOC and/or WOC) the feed can be higher, but the potential for rubbing (or heeling) of the back-side cutting edge exists. When trying heavier feeds, evaluate the back-side cutting edge after running the tool for only a few minutes, looking for evidence of rubbing or damage.

Your DTB series inserts utilize chip-thinning for optimum performance. Chip-thinning is the process in which the actual chip thickness created by a cut is less than the FPT at which the tool is programmed. See the chart below to see the chip-thinning factor for various depths of cut. For a correct chip thickness, multiply the FPT (from page 10) by the chip thinning factor below. This will give you an accurate feed and optimize your performance.

Diagram (left) shows the varying chip thickness when feeding .010" feed per tooth (FPT) at different depths of cut (DOC) with a 12mm diameter insert: At .250" DOC, the chip thickness is a true .010" At .100" DOC, the chip thickness is .008" At .060" DOC, the chip thickness is .006" At .020" DOC, the chip thickness is only .004"

Feed Rate Compensation

After determining the desired chip thickness (FPT – see chart on page 10), find the Depth of Cut intersection in the chart at right. Multiply the desired chip thickness by the factor shown in the chart. This will be the Adjusted Feed per Tooth (AFPT), resulting in a true chip thickness of the desired amount. Example: @ .03" Depth of Cut (DOC), the factor for the chip thickness = 2.1. So, if a chip thickness of .005" is desired, a feed rate of .0105" (.005 x 2.1) needs to be programmed into the machine tool. or Adjusted Feed per Tooth (AFPT) = chip thickness x chip thinning factor (from chart)


Concern Possible Cause Solutions
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
  • Increase DOC
  • Use harder grade
Insert Chipping
  • Surface footage is low
  • Incorrect grade or coating
  • Using Dished insert incorrectly
  • Feed too high
  • Verify correct speed and feed
  • Increase spindle speed
  • Decrease feed rate
  • Decrease DOC 
  • Use T-Land Insert 
  • Use tougher grade
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
  • Use coolant
Poor finish/chatter
  • Cutter hung out too far
  • Excessive runout
  • Inadequate tool holding
  • Reduce tool gage length
  • Check tool holder wear
  • Use high-rigidity tool holder
Tool shank breaks
  • Tool pressure too great
  • Fatigued cutter body
  • Decrease DOC
  • Reduce tool gage length
  • Decrease feed rate


Hole Diameter Calculation

(R2 – 8mm IC)
Shell Mill Part Number Minimum Hole Dia. Maximum Hole Dia.*
DTEM125-300-R4-3 2.00" 2.50"
DTEM150-350-R4-3 2.50" 3.00"
DTSM200-075-R4-5 3.50" 4.00"
DTSM250-100-R4-6 4.50" 5.00"
DTSM300-100-R4-7 5.50" 6.00"
DTSM400-150-R4-8 7.50" 8.00"

Formulas: Minimum Hole Dia.: (Tool Dia. x 2) - (1.5 x Insert Dia.)
Maximum Hole Dia.*: Tool Dia. x 2

* Not generally recommended. At this diameter, the center tip is at its maximum. It is suggested that you stay slightly under this number.

Larger diameter hole making can be quick and easy when a DTB Series Cutter is used in combination with helical interpolation. This technique resembles thread milling in that all three axes (X, Y and Z) are in motion simultaneously. It differs from thread milling in that the tool is introduced into the material without a start hole of any kind. The tool simply is positioned at the inside diameter of the hole to begin its helix from there, achieving complete material removal from the hole by ramping down to the final depth. This smooth operation tends to avoid the high horsepower consumption characteristic of large diameter hole making. This quick and easy process offers the added advantage of allowing many different hole sizes to be generated with the same diameter tool. Hole size variation is all in the programming.

For more information on how helical interpolation can improve your manufacturing efficiency, contact your Dapra Applications Specialist.

Recommended Cutting Speeds & Feeds

Click chart image to enlarge

Insert Grade Selection

DTB Insert Grade Selection
Shock & Wear Resistance Uncoated (Base Grade) with Coating Description Specifications
Shock Resistance
DMK30 Moderate wear resistance/high shock resistance. Recommended for interrupted or unstable steel, most stainless steel, high-temperature alloys and cast iron applications. ANSI C1-C2 ISO K25-K40, M25-M35
  DMK30-TCI High-performance medium- to high-temperature grade. Outstanding shock and wear resistance in steels, irons and stainless steels. Best suited for materials < 44 Rc.
DMK30-GLH Premium high-temperature coating. Best resistance to heat for high-shock applications. Excellent for tough stainless steels, high-temperature alloys and many tool steels.
Shock and Wear
DMP25 High wear resistance/moderate shock resistance. Recommended for most steel and ductile iron applications. ANSI C5-C6 ISO P25-P40
  DMP25-TCI High-performance medium- to high-temperature grade. Outstanding wear resistance in steels and ductile. Best suited for materials < 44 Rc.
DMP25-GLH Premium high-temperature grade. Unbeatable performance and wear resistance in high-heat applications such as higher-speed machining in steels (< 44 Rc) and ductile irons.
Wear Resistance
DMK15 Highest wear resistance with reduced shock absorption capabilities. Micro-grain carbide provides excellent edge strength. Suitable for all materials under stable conditions. ANSI C2-C3 ISO K15-K25, M15-M25
  DMK15-TCI High-performance medium- to high-temperature grade. Great for higher-speed gray iron applications and lighter cuts in steels <52 Rc or ductile iron.
DMK15-GLH Premium high-temperature grade for optimum wear resistance in cast irons and steel hard milling > 44 Rc.
Other coatings available upon request