Plain Turning Using G71 Canned Cycle – My Practical Experience (Complete Guide)

 Introduction 

When I first started working with CNC lathes, I used to write manual turning programs for every step. If I had to reduce the diameter from 20 mm to 15 mm, I would write multiple G01 lines — pass by pass. It worked, but it was slow, confusing, and sometimes risky.

Later, I learned the G71 canned cycle, and honestly, it completely changed the way I program CNC machines. It saves time, reduces errors, and is perfect for real production work.

In this guide, I’ll explain the G71 canned cycle from real shop-floor experience, how it’s actually used in industry, along with common mistakes and practical solutions.

What is G71? (Simple Understanding) 

G71 is a rough turning cycle.

In simple words:

Instead of telling the machine “cut again and again,”
 You define the shape once, and G71 will automatically remove material in multiple passes.

This is very useful when:

• Material removal is high
• Diameter reduction is large
• Production is continuous

Why I Prefer G71 in Real Work

From my experience:

• Writing 10–15 lines manually is tiring
• One mistake = scrap part
• Time wasted during programming

With G71:

• Programming becomes simple
• The machine does roughing automatically
• Consistent cutting every time

G71 Syntax (What I Actually Remember)

I don’t try to memorise everything like a formula. I remember it like this:

G71 U(depth) R(retract)
G71 P(start) Q(end) U(finish X) W(finish Z) F(feed)

That’s enough to work confidently.

How I Understand Each Value (Practical Way)

• ·      U (depth of cut)

a.       How much material to remove per pass?

b.        I usually give 0.5 to 1 mm, depending on the material

• ·      R (retraction)

a.       Small movement back after each cut

b.       Prevents tool rubbing

•      P & Q

a.       These are block numbers where the profile starts and ends

b.       Many beginners make mistakes here

•      U & W (finishing allowance)

a.       Always leave small material (like 0.2 mm)

b.       Final finishing will be clean

Practical Example (Real Shop Situation)

Problem I Worked On:

• Raw diameter =  12 mm
• Final diameter = 10 mm
• Length = 90 mm

Program I Use

O1020;

G28 U0.0 W0.0;

T0101;

G97 M03 S1200;

M08;

G00 X14.0 Z2.0;

(--- Facing ---)

G01 Z0.0 F0.2;

G01 X-1.0;

G00 X14.0 Z2.0;

(--- Turning ---)

G71 U0.5 R0.5;

G71 P10 Q30 U0.05 W0.05 F0.15;

N10 G01 Z0.0;

N20 G01 X10.0;

N30 G01 Z-85.0; 

(--- Finishing ---)

G70 P10 Q30 F0.1;

G00 X100 Z100;

M09;

M05;

G28 U0.0 W0.0;

M30;

What Actually Happens in a Machine

From my observation:

• Tool starts from a safe position
• Cuts layer by layer (automatic passes)
• After each pass, it slightly retracts
• Leaves small material for finishing
• Finally, G70 gives smooth finish

This is exactly what we want in production.

Mistakes I Personally Faced (Very Important)

1. Tool Not Cutting

Once I gave the wrong X value (like X20 instead of X16 in diameter mode)

The machine moved but didn’t cut

Lesson:
Always check:

• Diameter mode
• Offset value

2. Wrong P and Q Blocks

I gave the wrong block numbers.

The machine didn’t follow the correct profile

Lesson:
Always double-check sequence numbers.

3. Too High Depth of Cut

I gave U = 2 mm in steel

Tool vibration + poor finish

a.       Lesson:

• Mild steel → 0.5 to 1 mm
• Hard material → even less

4. No Finishing Allowance

I forgot U and W in the second line

The final size was wrong

Lesson:
Always leave a small finishing stock.

My Practical Tips (From Real Work)

a.        Always start from a safe position (X > raw dia)

b.        Do a dry run first (very important)

c.        Use coolant properly

d.        Check the insert condition before running

e.        Don’t hurry — most errors happen due to tension

When I Use G71 (Real Decision)

I use G71 when:

• Diameter reduction is more
• Batch production is there
• Simple profile turning

I don’t use G71 when:

• Only a small finishing cut is needed
• Very complex contour

Why G70 is Important After G71

G71 only does rough cutting.

If you stop there:

• Surface will be rough
• Dimension may not be accurate

So I always use:

G70 P10 Q30

This gives the final finish and exact size

Real Advantage I Felt

After using G71 regularly:

• Programming time reduced
• Confidence increased
• Mistakes reduced
• Production became faster

This is why industries prefer canned cycles

FAQs (Based on Real Doubts)

1. Why is my tool not cutting in the G71 cycle?

Most common reasons:

• Wrong offset
• Wrong X value
• Tool above diameter

2. What is the correct depth of cut in G71?

It depends on the material:

• Aluminum → 1 to 2 mm
• Mild steel → 0.5 to 1 mm
• Hard material → 0.2 to 0.5 mm

Choosing the right depth improves tool life and surface finish.

3. Why is my G71 cycle taking too many passes?

If your U value (depth of cut) is too small, the machine will take more passes. Increase it slightly for faster machining, but stay within safe limits.

4. What happens if I don’t use G70 after G71?

G71 performs only roughing. Without G70:

• Surface finish will be poor
• Final dimensions may not be accurate

Always use G70 for finishing.

5. Can I use G71 for small diameter changes?

Yes, but it’s not efficient. For small cuts, manual G01 programming is faster and more suitable.

6. Why is my final dimension oversized after G71?

This happens when the finishing allowance (U and W) is not properly set. Always leave a small allowance (like 0.05 mm) and use G70 to achieve the final size.

7. What is the role of P and Q in G71?

P and Q define the start and end of the profile. If these block numbers are wrong, the machine will not follow the correct path.

8. Why does the tool retract after every pass in G71?

The R value controls retraction. This helps:

• Avoid tool rubbing
• Improve cutting efficiency
• Increase tool life

9. Can I use G00 inside G71 profile blocks?

No, it is not recommended. Always use G01 (cutting movement) inside profile blocks to ensure proper machining.

10. Why is my tool vibrating during G71 operation?

Common reasons:

• Too high depth of cut
• Worn-out tool insert
• Improper clamping
• Low spindle speed

Adjust cutting parameters and check tool condition.

Conclusion

If you are serious about CNC programming, G71 is a must-learn cycle. In real industry work, no one writes long manual programs for rough turning.

Once you understand G71 properly and practice it on different jobs, your programming speed and confidence will improve a lot.

 Final Advice

Don’t just read this.

·        Try this program on the machine

·        Change values

·        Observe tool movement

That’s how real learning happens.