Skip to content
Tutorials Center
My learning

Topics

Lesson 27 of 49 ยท Machining

Chapter review: machining

Review the machining chapter: a one-picture summary, a recap table of formulas, a speed-and-power planner you can run, and a ten-question mixed quiz.

You have now followed a cut from the first contact of the tool to the cost of a finished part. This review ties the pieces together. Read the picture, scan the table, try the planner on your own numbers, and then test yourself with the quiz at the end. If any answer surprises you, the table tells you which lesson to reread.

Five numbered blocks summarizing cutting, speeds and feeds, power, tool life and CNC, beside a lathe pass and the planning order
The chapter in one picture: choose speed from tool life, feed from finish, depth from rigidity and power, then check that the machine can deliver it.

What you will learn

  • How the five ideas of the chapter fit into one planning routine.
  • Which formula to reach for in each situation.
  • How to check a planned cut against machine power.

Key terms

Process plan: the ordered list of operations, tools, speeds and feeds for making a part.

Roughing and finishing: a fast pass with large feed and depth that removes bulk, then a light pass for size and surface.

Power limit: the cut that the spindle motor can drive without stalling; often the first limit you hit in roughing.

Recap table

Idea Key equations Rule of thumb
Chip formation r = t0/tc = sin ฯ† / cos(ฯ† โˆ’ ฮฑ), ฮณ = cot ฯ† + tan(ฯ† โˆ’ ฮฑ) Positive rake and low friction give a bigger shear angle
Forces F = Fc sin ฮฑ + Ft cos ฮฑ, N = Fc cos ฮฑ โˆ’ Ft sin ฮฑ Thrust force does no work but bends the tool
Speed V = ฯ€ D N / 1000 V comes from tool and work material, N follows
Removal rate Turning V f d ร— 1000; milling ae ap vf Depth of cut costs the least tool life
Power P = MRR ร— u Divide by drive efficiency for the motor
Finish Ra โ‰ˆ fยฒ / (32 r) Small feed and big nose radius
Tool life V Tโฟ = C A 20% speed rise can halve carbide life
Cost T_opt = (1/n โˆ’ 1)(tc + Ct/Cm) The cheapest speed is neither the fastest nor the slowest
CNC G00, G01, G02/G03, G54, G43 Offsets connect the program to reality

A planning routine

  1. Choose a tool material and grade for the work material and the cut type (smooth or interrupted).
  2. Pick V from the tool maker's range, adjusted by the tool life you want.
  3. Pick feed f from the finish required: large for roughing, small for finishing.
  4. Pick depth d from the stock allowance and the machine's rigidity.
  5. Calculate N, MRR, power and time. If the power exceeds the machine's rating, reduce depth first (it affects tool life least), then feed.
  6. Write the program, run the first part slowly, measure, and apply offsets.

Common misconceptions

"The settings in the catalog are the answer." They are a starting point. The actual best values depend on rigidity, coolant, the batch size and the tool cost.

"If the power is enough, the cut is fine." Rigidity and chatter (self-excited vibration) can limit a cut long before power does, especially with long tools and thin walls.

Try it

Here is a short planner that checks a turning cut against a machine's power. Change the inputs and watch which limit you hit.

Python Cut planner with a power check

Press Run (or Ctrl + Enter) to see the result here.

Program input ยท what you'd type while the program runs

Type the answers before you press Run, one per line. Each time the program reads a line (with input()), it gets the next line from this box.

Then a quick drill for the rpm formula. It makes up a diameter and a cutting speed; you give the spindle speed.

Spindle speed drill

Check your understanding

Quick check ยท 10 questions

of 10 answered You scored / 10 ยท perfect!

  1. 1. A chip is 0.30 mm thick from a 0.15 mm uncut layer. What is the chip thickness ratio?

    r = t0 / tc = 0.15 / 0.30 = 0.5.
  2. 2. Which force is multiplied by cutting speed to give cutting power?

    Only the cutting force acts along the direction of motion, so P = Fc ร— V.
  3. 3. What is the spindle speed for a 25 mm cutter at 100 m/min?

    N = 1000 ร— 100 / (ฯ€ ร— 25) = 1,273 rpm.
  4. 4. Removal rate in turning with V = 200 m/min, f = 0.25 mm and d = 2 mm is:

    200 ร— 0.25 ร— 2 ร— 1000 = 100,000 mmยณ/min = 100 cmยณ/min.
  5. 5. A finishing pass is changed from f = 0.2 mm to f = 0.1 mm. The ideal Ra becomes:

    Ra is proportional to f squared, so halving the feed divides it by four.
  6. 6. If the machine is power limited, which setting should you reduce first to keep tool life?

    Depth of cut raises force and power but changes tool life much less than speed does, so it is the first setting to trade.
  7. 7. Which tool material would you choose for aluminum with a long life?

    PCD resists the abrasive silicon in aluminum alloys and does not react with aluminum, so it lasts very long.
  8. 8. In Taylor's equation with n = 0.2, what happens to tool life if you cut 10 percent slower?

    T scales as V^(-1/n) = V^(-5). At 0.9 V: 0.9^(-5) = 1.69, an increase of about 69 percent. Life is very sensitive to speed.
  9. 9. Which G-code line is a straight move at feed rate?

    G01 is linear interpolation at the feed rate F. G00 is a rapid move and G02 is a clockwise arc.
  10. 10. A tool at 100 m/min lasts 60 min and at 140 m/min lasts 20 min. Roughly what is n?

    n = ln(140/100) / ln(60/20) = 0.336 / 1.099 โ‰ˆ 0.31.

Summary

  • Chip formation is shear on a plane; rake angle and friction decide the shear angle and the force.
  • Speed, feed and depth give rpm, removal rate, time, power and finish; check power and rigidity before you commit.
  • Tool life falls steeply with speed (Taylor), so the cheapest speed lies between the slowest and the fastest.
  • CNC programs move the tool; offsets connect the program to the real part.

Next: Joining and welding at a glance