The Method and Technique of Machining Variable-pitch Thread with Macro Program on CNC Lathe

The Method and Technique of Machining Variable-pitch Thread with Macro Program on CNC Lathe

This article explains four contents:

1. What is a variable pitch thread.

2. G code for variable pitch thread

3. Macro program of variable pitch thread

1. What is a variable pitch thread

The so-called variable pitch thread, that is, the pitch value is not fixed, but gradually changes along the axis direction.

2. G code for machining variable pitch thread

G34 X__ Z__ F__K__

1, F is the initial pitch of the processed variable pitch thread.

2. K value is the increment or decrement of the pitch when the main shaft rotates one revolution. If K is a positive value, then the pitch is increasing, and K is negative, that is, decreasing.

Of course, you can also use the commonly used G92, G32 or even G01 commands. How to use it, follow Zou Jun to learn "CNC Macro Program" version 3.0, start from scratch, step by step, let you play macro programming thoroughly.

Well, look at the following diagram, which is a variable pitch thread.

picture

The pitch gradually decreases from the initial 20 to 19, 18, 17..., then the K value in the G34 command is -1.

3. How to write the program of variable pitch thread

You can use the method of calculating point coordinates shared by Jun to turn along the contour line sequentially. It is also possible to use a commonly used layered car, which is turned layer by layer.

However, in layered cutting, due to the increasing depth of cut, the contact surface between the tool and the tooth flank is getting larger and larger, and the cutting force is also increasing, which can easily cause damage to the tool or workpiece. Then I can use the depth of each layer to decrease continuously, thereby reducing the cutting force and completing the thread processing.

The procedure is as follows:

O 1111

G21G40 G97 G99 T0100

T0101 thread cutter

S300 M03

G00 X38. Z21 Thread cycle starting point

#1= 0.5 first cut depth

#2= 3.0 profile height (radius value)

N1 #2=#2-#1 The remaining tooth height after each depth of cut

IF [#2 LE 0.05 ] GOTO2 If the remaining tooth height≦0.05, transfer to N2 block

G00 X[30+2*#2] 30 is the outer diameter of the thread

G34 Z-100. F20 K-1

G00 X38.

Z21.

#1=0.8*#1 Each cutting depth is 0.8 times of last time

IF [#1 GE 0.05 ] GOTO1 If the depth of cut≧0.05, transfer to N1 block.

#1=0.05 Otherwise, the depth of cut is fixed at 0.05

GOTO1 transfer to N1 block

N2 G00 X30 Z21

G34 Z-100 F20 K-1

G00 X38

Z200

M30