Milling & Drilling Information

Basic Milling Operations

ContourMilling.jpg

Contour Milling

Contour milling is for remove material from the outer surface of a part. This operation is for machining parts with flat faces. Keep in mind that you can create convex right angles, but cannot create concave right angles without a radius between segments.

  • Normally preformed with a flat bottom End Mill.
  • Always use a collet.
  • Never use a drill chuck!
Slotting.jpg

Slotting

Slotting is the removal of material were the slot width is the same size of the cutter.

  • A flat bottom or Ball End Mill is normally used for this operation.
  • Always use a COLLET to secure the End Mill!
  • Never use a drill chuck to hold an End Mill!
PlungeMilling.jpg

Plunge Milling

Plunge milling is a process of feeding an end mill into the workpiece to create a vertical hole. Use plunge milling for overlapping holes, or when entering a part to start a pocket/slot.

  • A flat bottom CENTER-CUTTING End Mill is normally used for this operation.
  • Always use a COLLET to secure the End Mill!
  • Never use a drill chuck to hold an End Mill!
  • Never use a non-center cutting end mill!
PocketMilling.jpg

Pocketing

Pocketing is to remove material from the inside of a workpiece to create a cavity, or "pocket". You start by plunging into the part in the Z-axis. Then, cut in the X- and Y-axes to remove material.

  • A flat bottom or bullnose End Mill is normally used for this operation.
  • Always use a COLLET to secure the End Mill!
  • Never use a drill chuck to hold an End Mill!
Chamfering.jpg

Chamfering

Chamfering is the removal of material from the edge of a workpiece, resulting in a slanted surface where two faces intersect.

  • Use a Chamfer End Mill
  • Always use a COLLET to secure the End Mill!
  • Never use a drill chuck to hold an End Mill!
Facing.jpg

Face Milling

Facing is for achieving a flat surface on the a workpiece. This can be done either by using a regular Flat Bottom End Mill or a Face Mill.

  • Use a Face Mill or Flat Bottom End Mill in the appropriate tool holder.
Facing%20%28Fly%20Cutter%29.jpg

Fly-Cutting

Facing is for achieving a flat surface on the a workpiece.

  • Always use a COLLET to secure the Fly-Cutter!
  • Never use a drill chuck to hold a Fly-Cutter!
Drilling.jpg

Drilling

Drilling is for the creating a hole in the workpiece by feeding the drill bit in the Z-axis (vertically).

  • A drill chuck is normally used for securing the drill bit.
  • See the Drill Basics section of this Wiki for more details.
Reaming.jpg

Reaming
Reaming is for finishing a hole. This creates better surface finish and a more precise hole.

  • A drill chuck is normally used for securing the reamer.
  • ONLY feed the reamer in the direction of the hole.
  • NEVER bottom out a reamer in the hole!
Counterboring.jpg

Counterboring

Counterboring is for making larger size diameter hole near the top of the part for the head of a screw to be recessed below the top surface.

  • A Counterbore or Flat Bottom End Mill can be used for this process.
  • If an End Mill is being used, put it in a Collet!
Countersinking.jpg

Countersinking

Countersinking is for creating a chamfer on the edge of a hole or slot.

  • This is used for sinking a flat head cap screw flush with the surface of a part
  • A great way to break an edge of a hole or slot so that hand deburring can be avoided.
  • A taped hole should be countersunk before tapping it.
Boring.jpg

Boring

Boring involves the use of a boring head and boring bar to create an inside diameter in a workpiece.

  • This process allows for a precision hole to be created at any desired size.
  • An Automatic Boring Head can be used to machine internal and external grooves, and face the workpiece.
Tapping.jpg

Tapping

Tapping is a process of create threads on the inside of a hole using a cutting tool called a tap.

  • Use a spring-loaded tap guide mounted in the drill chuck or collet and a tap mounted in a tap holder.
  • The tap is then turned by hand to create the threads.
  • Never Turn on the mill for this operation!
Dovetailing.jpg

Dovetailing

Dovetailing is normally used for two parts to slip fit together and allowing leaner movements between the parts.

  • A Dovetail cutter is used to create this feature.
Broaching.jpg

Broaching

Broaching is for removing material in linear strokes by using a broaching tool. This is done by mounting the broach in the spindle and using it to remove material vertically.

  • Useful for creating shaft keyways and right-angled channels.
  • Use the correct Broaching tool for this operation.

Drilling Basics

When Must I Use a Spot Drill?

Is a spot drill necessary every time an accurate hole is to be drilled? After all, its purpose is to ensure the hole is accurately located. The short spot drill is very rigid, and the spotting motion is unlikely to deflect, correct? Well it depends, if you use a carbide drill, or a screw machine length drill, spotting is typically not required. The carbide itself is so rigid compared to HSS that the drill will produce a hole where it is located. As a matter of fact, most manufacturers recommend against spotting either a carbide twist drill or an insertable drill because its easy to chip the carbide in the dimple.

Screw machine-length twist drills are shorter and more rigid than jobber length, they normally do not need to be spot drilled first unless you are drilling into a curved surface.
StubDrill.jpg

There are times when you won’t be able to avoid a jobber length drill because the hole is too deep for a screw machine drill. In that case, you could spot drill to start the twist drill, or you could drill the shallow part of the hole with a screw machine length and then switch to the longer drill bit. Either way you’re facing a tool change, so it’s six of one and half a dozen of the other.

NC spot drills due not have body clearance and are not designed to drill greater than the depth of the point angle. The 90º and 120º spot drills are primarily used to create an initial spot for 118º and 135º secondary drills respectively. The 142º point NC Spot drill, is designed to help center carbide drills with an angle of 140º.

Note for Carbide Drills: The center of the carbide drill bit must make contact with the center of the spot drilled hole, if the outer edges make contact first, it will chip the drill bit!

Can I Use a Center Drill Instead of a Spot Drill?

A lot of machinists use center drills for spotting instead of true spotting drills. Center drills are intended to be used to create a hole suitable for a lathe center. They have a two part tip that has a small pilot as well as the larger countersinking area of the bit. While center drills are available more cheaply than spot drills, they have some disadvantages. The small pilot tip is very delicate for example, and if it breaks, the drill will quit cutting. Not a happy thing if you’re running a job that involves spotting a lot of holes. Another problem is the hole angle of a center drill is typically 60°. When spotting, you want an angle that is larger than the HSS twist drill’s angle when possible. The narrower the spot angle, the more near the outside diameter of the twist drill comes in contact first. If the twist drill’s flutes aren’t perfectly sharpened, one will contact the spot hole before the other and the drill will try to deflect. This defeats the purpose of spot drilling and can result in a less accurate hole. The broader angle of a true spot drill means the tip of the twist drill cuts first, which makes for a more accurate hole. Lastly, the web of a spot drill is typically thinner than a center drill, so it cuts more easily and with less heat.

Drills for Sheet Metal:

Spade Drills:
SpadeDrill.png

These drill bits require rigid tool-holding to prevent breakage and should not be used in hand-held drilling applications. These bits have short flutes and a sturdy construction which prevent snagging that deforms sheet metal and thin-wall tubing. A Straight-Flute Drill Bit may also be used, see image in the "Drills for Copper and Brass" section below.

Step Drills:
StepDrill.png

These drill bits can be use with hand powered drills, they have steps with progressively larger diameters that allows you to drill a wide range of sizes with one bit. A Straight-Flute Drill Bit may also be used, see image in the "Drills for Copper and Brass" section below.

Drills for Copper and Brass:

Straight-Flute Drills:
Straight-FluteDrillBit.png

These drill bits are used when drilling copper or brass because they have less of a tendency to "dig in" or grab the material, they may also be used for drilling sheet metal.

Should One Use a Drill Chuck or Collet Chuck?

ColletVsChuck.jpg

The choice of whether to use a Drill Chuck or Collet Chuck for a Spot Drill or any other Twist Drill is a divided one, because we’re optimizing two parameters and there is a different choice for each.

For best accuracy, use a collet chuck for your spot drill and twist drills. Traditional drill chucks are less accurate and setscrew endmill holders are even worse.

However, for holding power, the drill chuck is the winner.
Here’s why: The Drill chuck concentrates its grip in three narrow places which has a high localized bearing stress causing mynute surface deformations that resists slipping.

If you need more rigidity than torque holding power, use a collet. One sign of needing more rigidity is a drill creating a trilobal shaped hole, in this case use a collet to hold the drill bit.
There are time were a flat bottomed drill bit might be used to make a counterbore. It is preferred that an end mill be used for this application but if a flat bottom drill bit is used, use a collet instead of a drill chuck, the drill chuck will let the drill bit wonder all over the place…

When drilling through material that is prone to work hardening, reduce the feed rate just before the drill exists the material by 50% to prolong the tool life.


Select the Correct Drill Length

DrillDepth.png

Select the Correct Helix Angle

HelexAngles.png

Drill Bit Selection

Reamer Basics

Whenever a hole needs to have a tolerance greater than approximately ±1% of its diameter, the hole should be reamed or bored to size.

  • Reamers should be run at half the spindle speed and twice the federate of the comparable sized drill bit. Use a G86, the reamer should be retracted with the spindle off to preserve the surface finish of the hole and to mitigate bell-mouthing the holes entrance area.
  • The Pre-Ream hole size should be left UNDERSIZE by the amount listed below:
    • Reamer Sizes: <0.06 = 0.005"
    • Reamer Sizes: 0.06≤D<0.25 = 0.010"
    • Reamer Sizes: 0.25≤D<0.50 = 0.015"
    • Reamer Sizes: 0.50≤D<1.50 = 0.025"
  • FLUTE STYLES
    • Straight Flutes - Good in a wide variety of applications.
    • Right Spiral Flutes - Tend to bridge interruptions such as keyways, slots or intersecting holes; Good chip clearing ability for ductile materials and blind holes.
    • Left Spiral Flutes - Also tend to bridge interruptions; Good for cast irons, heat treated steels and other hard materials; Do not use in blind holes.
    • Expansion Reamers - Economical for abrasive materials.
  • See this Reamer Guide for more details.

Chatter Issues


Please click here to find out possible causes of End Mill chatter.


Climb Milling vs Conventional Milling

Conventional_vs_Climb_Milling.jpg


End Mill Shapes

Flat Bottom
BottomEM.jpg
Bull-Nose
BullNoseEM.jpg
Ball
BallEM.jpg
Chamfer
ChamferEM.jpg

End Mill Troubleshooting Guide


Fixture Components


Machine Vise Options and Accessories


Tool changing Procedure


Squaring Up a Block

Squaring%20up%20a%20part.jpg

Tool Run-out vs Tool Life


How bad is tool run out?


Big Kaiser ran tests with drills and reducing runout on carbide drills from 0.0006″ to 0.00008″ (tiny!) resulted in a 3x tool life improvement. Wow!

There are a lot of rule of thumb and anecdotal answers floating around the web, but here’s a quick and easy to understand chart that explains how runout affects your tool life:

RunoutVsToolLife.jpg


Runout (TIR) as a percentage of chip load versus Tool Life…


In this chart, runout is given as a percentage of chip load, which is the thickness of a single chip being sliced off by your cutter. This is how I like to think of runout–it increases chip load beyond what you intended. As you can see, tool life goes down dramatically when we get to TIR’s (Total Indicated Runout) beyond about 20% of your cutter’s targeted chip load. This also explains why runout is so hard on tiny cutters–they have small chip loads and can tolerate very little runout as a result.


Please click here to find out more about tool run-out.



Unless otherwise stated, the content of this page is licensed under Creative Commons Attribution-ShareAlike 3.0 License