Content      ..     8      9      10     

HNC8 Series CNC Controller. Programming Manual (V2.4) - page 10

%0001

（The tool position point is the ball center）

G92 X-30 Y-30 Z25

#0=5

（Fillet radius）

#1=4

（Radius of ball-end cutter）

#2=180

（The initial value of the step angle γ. Unit: Degree）

WHILE #2 GT 90

G01 Z[25+[#0+#1]*SIN[#2*PI/180]]

（Calculate Z axis height）

#3=ABS[[#0+#1]*COS[#2*PI/180]]-#0 （Calculate radius offset）

G10 L12 P3 R[#3]

G01 G41 X-20 D3

Y14

G02 X-14 Y20 R6

G01 X14

G02 X20 Y14 R6

G01 Y-14

G02 X14 Y-20 R6

G01 X-14

G02 X-20 Y-14 R6

G01Y30

G01 X-30

G40 Y-30

#2=#2-10

ENDW

M30

361

19.3

Manual Calling Subprogram

Function and Purpose



In JOG mode, user can customize the buttons on the MCP panel, set the G register to 1 by the

button, and call the related suprograms, thereby realizing some more complex functions, such as

tool change, spindle C/S switching, etc.

The correspondence of G register points to subprograms is shown in the following table

G register point

Canned cycle subprogram

G2637.1

Call canned cycle subprogram O1007

G2637.2

Call canned cycle subprogram O1008

G2637.3

Call canned cycle subprogram O1009

G2637.4

Call canned cycle subprogram O1010

G2637.5

Call canned cycle subprogram O1011

G2637.6

Call canned cycle subprogram O1012

G2637.7

Call canned cycle subprogram O1013

G2637.8

Call canned cycle subprogram O1014

G2637.9

Call canned cycle subprogram O1015

G2637.10

Call canned cycle subprogram O1016

G2637.11

Call canned cycle subprogram O1017

G2637.12

Call canned cycle subprogram O1018

G2637.13

Call canned cycle subprogram O1019

G2637.14

Call canned cycle subprogram O1020

G2637.15

Call canned cycle subprogram O1021

F2637.0

Status bit: subprogram is running in JOG mode

Description



(1) In PLC, the program can be created as shown below (user can customize the buttons based on

the actual situation), the G command signal can be output, and the corresponding subprogram can

be called.

(2) In JOG mode, call the corresponding subprogram by clicking the button. Click the F3 button

as shown in the figure above to call

O1007 subprogram.

362

Note

(1) During the execution of the program, F2637.0 is always 1, and the buttons on the panel are in

the shielding state except for the reset and emergency stop buttons, and the clicks are invalid;

when the corresponding G register signal (e.g. G2637.1) is 0, F2637.0 is 0 after the subprogram

is executed.

(2) Currently, subprograms O1007 to O1021 must be placed in the file USERDEF.CYC. The

subprogram corresponding to the O1007 program starts with %1007, and O1008 corresponds

to %1008, and so on. In the line before M99 at the end of each subprogram, G80 must be added

to clear the canned cycle mode.

(3) When the subprogram is called manually, the buttons on the MCP panel should be in the

shielding state except for emergency stop button, but for the PLC output control buttons (such as

spindle CW, spindle CCW, cooling, etc.), PLC needs to be changed to shield these buttons.

For example, shielding the function key of spindle CW:

For the M command that is only executed in the auto/single-block mode, the normally open point

of F2637.0 should be connected in parallel in the program, as shown in the figure below, to ensure

that the M command can be executed normally during calling subprogram in JOG mode.

363

20 High-speed High-Precision Function

20.1

Machining Optimization Function G125/G126

Function and Purpose



If the processing optimization function is turned on by the G command (G125) in the program,

the CNC system can optimize the speed of the related processing program (G code program) to

improve the surface quality of the part. This function is mostly used for finishing of curved or

mold parts.

Command Format

G125 ； Call machining optimization function

G126 ； Cancel machining optimization function

Example

The processing optimization function used to optimize standard curved surface parts processing

procedures

%0001

G40 G17 G49 G80 G90

G54

N0010 (ROUGH_MILL)

G0 X46.694 Y-51.205 S6000 M03

G125

； Call machining optimization function

Z5.

Z2.521

……………………………

G2 X-40.694 Y-53.651 I13.015 J58.936

G1 X-46.694 Y-51.382

G1 Z2.521

G0 Z5.

X46.694 Y-44.44

Z2.521

G1 Z-0.479

G1 X40.694 Y-47.014

G2 X16.255 Y-51.349 I-21.491 J50.099

G1 X-17.851 Y-51.371

………………………………

364

G126

； Cancel machining optimization function

M30

Description



Interface button and logo introduction

The following figure shows the program selection interface

Machining optimization

Optimize the processing program (G code) and generate the corresponding optimization file.

Operation

Select the corresponding program and click the key, then the program will be optimized. The

interface prompt bar and pop-up box display the processing optimization progress, as shown

below:

365

After the program is optimized, the optimization column will display "Yes", as shown in the figure

below.

Cancel optimization

When the program optimization process is terminated, the optimization column displays "No".

Operation

Select the corresponding program and click the button, then the program optimization will be

cancelled, and the optimization column will display "No", as shown in the figure below:

Optimization column

"Yes" means that the processing optimization operation has been completed for G code program,

"No" means that the processing optimization operation has been not completed for G code

program.

Description of processing program optimization

G code optimization operation

All G codes can be optimized through the processing optimization key. The interface operation

366

and corresponding handling are shown in the following table.

Object

Operation

Result

The G code is optimized normally. After the

Unoptimized G code

optimization is completed, the optimization column

displays "Yes".

G code optimization is canceled, and the optimization

Optimized G code

clolum displays “No”

Note

 Different programs have different processing optimization procedures. Generally, t

he larger the program, the longer the optimization time, even as long as several

minutes. The program interface will display "Processing optimization complete

d..%, please wait patiently”.

 In the process of processing optimization, the processing optimization interface is

locked and cannot be switched to other interfaces until the optimization is compl

eted, and then other operations can be performed.

 For ordinary programs (<20M), during the optimization process, the optimization

completion progress is displayed in percentage (%) on the prompt bar; for super

large programs (>20M), during the optimization process, the optimization progress

is displayed as the number of program lines that has been optimized .

 If there is an alarm in the system or an alarm occurs during the optimization, th

e optimization will fail, and user needs to perform the reset and cancel the opti

mization. The following prompt will be given: the system alarm causes the proce

ssing optimization to fail, press reset button to cancel the optimization.

Optimized G-code editing and corresponding optimization

When editing or modifying the optimized G code, the program needs to be re-optimized

automatically. The specific operation and handling are shown in the following table:

Operation

Handling

Replace the optimized program

Optimization of G code is canceled, and optimization column

with the program of the same

displays “No”

name

Optimization of G code is canceled, and optimization column

Delete optimized program

displays“No”

Save as or copy an optimized

The program is still being optimized, the optimization column

program

indicates “Yes”

367

The program saved or copied is not optimized, the optimization

column indicates "No"

The renamed program is still being optimized, the optimization

Rename the optimized program

column indicates “Yes”

Modify the optimized program,

Optimization of G code is canceled, and optimization column

and save the modification

indicates “No”

Click “cancel optimization”

Optimization of G code is canceled, and optimization column

button for the optimized program

indicates “No”

Optimization of called subprograms in the main program

In the main program/subprogram calling mode, the optimization processing mode can be called

by adding G125 to the main program, so that all subprograms adopt the optimization processing

mode. It is also possible to optimize a subprogram separately to realize the optimization

processing of the subprogram.

Operation

Handling

All subprograms called by the main program can be optimized

Optimize main program

synchronously, and the optimization attribute of each program is

displayed as "Yes".

Optimize subprogram

The optimization attribute of the corresponding subprogram is

seperately

displayed as "Yes".

Modify the optimized

Optimization of main program is canceled, and optimization

main program

column indicates “No”

Modify the optimized

Optimization of G code is canceled, and optimization column

subprogram

indicates “No”

Note

 When the main program is used in combination with an external subprogram, if a

certain subprogram needs to use the optimization processing mode, add the G125

command at the head of the subprogram, add the G126 command before M99 at the

end of the program, and optimize the corresponding subprogram.

 Currently calling processing optimization function of internal subprogram is not

supported.

 The processing optimization function of M98P_L_ mode is not supported.

Activation of machining optimization mode

The optimized program can call the mold optimization processing mode only through the G

command calling. Generally, the G125 command is added to the program header.

368

1.5

0

0.015

800

20

Acceleration time

Acceleration

Centripetal

Smooth closing

Collinear

proportional factor

jerk time

acceleration

of preprocessing

angle

proportional

(mm/s2)

threshold

factor

(radians)

1

1

200~2000

1

0.017

G05.1Q1, G05.1Q2, and G05.1Q3 can be set.

(2) Axis parameter

Acceleration deceleration time constant (ms)

Acceleration deceleration jerk time constant (ms)

16

8

Example

Using of mold optimization processing mode

The mold optimization processing mode improves the processing speed planning, reduces the

frequency of the speed fluctuations during the processing, improves the smoothness of the

processing speed, and at the same time ensures the consistency of the speed of the adjacent tool

path in the three-dimensional surface processing, improves the processed surface quality, and

effectively solves the obvious cut marks in surface processing. In the case of the same processing

effect, the processing efficiency can be improved.

High-speed machining

Without machining

optimization

After machining

optimization

371

Without machining

optimization

Resultant speed curve

High-speed machining

After machining

optimization

Resultant speed curve

Improvement of machining

efficiency and quality

High

Comparing with ordinary

machining, the optimization

machining control can increase

the surface quality when the

machining efficiency is

constant.

7min33s

Optimization

machining

control

9min6s

Ordinary

machining control

Low

7min16s

Short

Machining time

Long

Note

(1) Use G125 in the program to turn on the optimization processing mode. If G125 is not used to

turn on the optimization processing mode, the processing is the same as the normal version.

(2) The optimization processing mode is generally used for three-dimensional surface finishing,

mainly to solve the obvious over-cutting in the processing of complex parts, and at the same time,

it can improve the processing efficiency while ensuring the processing quality.

(3) The G125 command must be placed before the traverse command of the program head.

(4) When the main program is used in combination with an external subprogram, if a certain

subprogram needs to use the optimization processing mode, then add G125 command at the head

of the subprogram, add G126 command before M99 at the end of the program, and optimize the

corresponding subprogram.

(5) The internal subprogram processing optimization function is not supported.

(6) The processing optimization function in M98P_L_ mode is not supported.

372

20.2

High Speed High Precision Mode Selection（M）（G05.1）

Function and Purpose



In modern CNC systems in order to ensure the quality of the contour processing, in addition to

the good mechanical accuracy of the CNC equipment, a CNC system with high-speed processing

capabilities and high-speed and high-precision functions is also required.

For the actual contour processing, it can generally be divided into roughing, semi-finishing and

finishing according to the parts processing procedure. Regardless of the processing mode, the

actual processing and finished product quality requirements can be decomposed as follows:

Machining

Feature

requirement

Focus on the processing time and increase the processing speed of the free

High efficiency

curve. There is no high requirement on dimensional precision of workpiece.

It is generally required for roughing or intermediate processing.

Balance of efficiency

There is no high requirement for processing time and accuracy, but both

and precision

need to be controlled within a certain range.

Focus on the dimensional accuracy of the workpiece. The surface quality

High precision

is high, and the processing efficiency is not considered. It is generally

finishing.

As shown in the above table, in the actual machining process, both efficiency and accuracy cannot

reach the optimal level, and only one of them can be emphasized or a balance between them is

maintained based on different process characteristics and requirements. There are a series of

control parameters that play a major role in processing efficiency and processing accuracy in the

system. The combined application of these control parameters can meet different processing

requirements.

Through this command, different processing modes can be switched to meet the processing

requirements of different technological characteristics.

Command Format

G05.1 Q_； Specifying processing mode

G05.1 Q0； Default mode

Parameter

Meaning

Q_

Select the processing mode, the value can be 0, 1, 2, 3. The four groups of

processing modes can be switched mutually by G05.1Q_.

373

Command

Description

G05.1Q0

Default mode: focus on a balance of efficiency and precision

G05.1Q1

High precision mode: focus on the machining surface and

dimensional precision

G05.1Q2

High-speed high-precision mode: focus on smoothness of processing

and a balance of efficiency and precision

G05.1Q3

High speed mode: focus on efficiency, improve processing speed of

free curve

With G05.1Q1, G05.1Q2, and G05.1Q3, user selects different high-speed and high-precision

machining modes and configures different parameters (speed smoothing, spline smoothing, etc.)

to achieve high efficiency, high precision, or balance of efficiency and precision.

Example

High-speed high-precision mode is used to edit small line segment program

1） G05.1Q0

； Default mode; balance of efficiency and

precision is focused

example

G54

G0 X48.689 Y-51.225 S6000 M03

G05.1Q0

； Default mode; balance of efficiency and

precision is focused

X46.694 Y-37.445

………………

Z2.521

M30

2） G05.1Q1

； High-precision mode; machining surface and

dimensional precision is focused

Example

G54

G0 X48.689 Y-51.225 S6000 M03

G05.1Q1

； Default mode; balance of efficiency and

precision is focused

X46.694 Y-37.445

………………

Z2.521

M30

3） G05.1Q2

；High-speed high-precision mode; machining smoothness and balance

of efficiency and precision is focused

Example

G54

G0 X48.689 Y-51.225 S6000 M03

374

20.3

High Speed High Precision Parameter Setting

Function and Purpose



In the actual CNC machining process, different workpieces processed by the same machine tool

or different parts and procedures of the same workpiece have their own technological

characteristics and processing requirements. The use of a set of control parameters obviously

cannot achieve good processing results. It is necessary to adopt a combination of different control

parameters for different parts and processes for overall coordinated control, so as to achieve the

best processing effect.

Description



Control parameters

Command speed smoothing periods

Parameter type

Parameter

Unit

Value range

Default value

Channel

040082

ms

0 to 50

0

parameter

Through the command speed smoothing window, the smooth transition of the command speed is

realized, the speed fluctuation is reduced, the speed stability in the high-speed control is ensured,

the vibration of the machine tool is reduced, and the processing efficiency is improved. The

working principle is shown in the figure below. For a small square (side length <0.5mm), as the

smoothing period increases, the 90° corners of the square will gradually become a circular

transition until it becomes a full circle; The amount of change in the composite speed gradually

decreases until it becomes a constant speed section, and the uniaxial speed gradually becomes a

smooth transition.

376

Command speed smoothing periods

Resultant speed

Resultant speed

Resultant speed

X axis speed

X axis speed

X axis speed

Y axis speed

Y axis speed

Y axis speed

It can be seen from the above principle that the command speed smoothing periods help to

improve the smoothness of processing speed, reduce machine tool vibration and improve

efficiency, and at the same time it will affect machining accuracy. The larger the command

smoothing periods, the lower the accuracy. That is, when the accuracy is the priority, the lower

value the better; when the efficiency is the priority, the larger value the better; when considering

the smoothness (efficiency and accuracy are both balanced), the value is between 10 and 30.

Centripetal acceleration

Parameter type

Parameter

Unit

Value range

Default value

Channel

040084

mm/s2

1.0 to 100000.0

1000.0

parameter

According to Newton's second law, the force will cause the object to produce an acceleration. The

acceleration produced by the centripetal force is the centripetal acceleration. Centripetal

acceleration is a physical quantity that reflects the speed and the direction of circular motion.

Centripetal acceleration only changes the direction of the velocity. The maximum centripetal

acceleration is used to set the limit of the maximum centripetal acceleration.

As shown in the figure below, the centripetal acceleration (ⁿa ), linear speed (^v ) and radius R

satisfy the following relationship:

2

a



v

R

n

377

Command path

When R is constant,

V (feedrate F)



Actual path

The feed cutting speed of the circular arc can be limited by the centripetal acceleration. The table

of comparison between the maximum feed speed of a circle with a certain radius (R) and the

centripetal acceleration is as follows:

Centripetal acceleration

500

1000

2000

3000

5000

6000

(mm/s2)

R5mm circular

deceleration speed

3000

4242.64

6000

7348.47

9486.83

10392.3

（mm/min）

R1mm circular

deceleration speed

1341.64

1897.36

2683.28

3286.33

4242.64

4647.58

（mm/min）

When the given feedrate F is larger than the circular deceleration speed of the current radius, the

speed will reduce to the circular deceleration speed of the current radius; when the given feedrate

F is lower than the circular deceleration speed of the current radius, the circular feed cutting is

executed at the given speed F.

According to the acceleration principle diagram, for a circular arc with a certain radius (R), the

radius error (△R) is proportional to the centripetal acceleration. Therefore, in the case of accuracy

priority, the feedrate on arc can be limited by reducing the acceleration; in the case of efficiency

priority, the feedrate on arc can be increased by increasing the acceleration, but the centripetal

acceleration needs to be adjusted based on the actual situation to meet the efficiency and precision

requirements.

Example: When the centripetal acceleration is set to 1000 mm/s2 and the given feedrate is

3000mm/min, for an arc with a radius of 5mm, the feed cutting is performed at 3000mm/min; for

an arc with a radius of 1mm, the feed cutting is performed at 1897.36mm/min.

Minimum internal angle of corner smoothing

Parameter type

Parameter

Unit

Value range

Default

Channel

040071

Degree

0 to 180

100

378

parameter

During continuous small line segment interpolation, local speed reduction can be performed based

on the actual programmed path. For situations where the sharpness of contour corner needs to be

highlighted, the speed will be reduced to 0 at the top of the sharp corner. This parameter is used

to set the value of the angle. If the processing angle is smaller than this angle, the exact stop will

be performed. If it is greater than this value, other determinations will be used to plan the speed

reduction at this angle, as shown in the figure below;

If θ is larger than the set value, the

speed will be reduced to 0 at the top of

the sharp corner.

Example: When the minimum interior angle of corner smoothing is set to 90°, the 45° (<90°) and

135° (>90°) corner paths and speed curves are shown in the following figure:

Resultant speed

Resultant speed

Corner deceleration proportional factor

Parameter

Parameter

Unit

Value range

Default value

type

Channel

040074

%

0 to 150

100

parameter

For the polyline of which corner angle is greater than the minimum inner angle of corner

smoothing, that is, it adopts arc transition mode to execute the feed at the corner. The corner

deceleration speed can be controlled by the corner deceleration proportional factor. The smaller

the setting value, the smaller the corner deceleration speed, the smaller the corner roundness, and

the smaller the accuracy error in theory, but the milling time at the corner will be longer and the

efficiency will be reduced.

379

Resultant speed

Resultant speed

The corner deceleration proportional factor can be adjusted based on the specific processing

requirements. In the case of accuracy priority, the value is set as small as possible; in the case of

efficiency priority, the value is set as large as possible; for the case of both efficiency and accuracy

being balanced, the value is between 90 and 99.

Whether the arc is discrete into straight lines

Parameter

Parameter

Unit

Value range

Default value

type

Channel

040079

-

0~1

0

parameter

If this function is turned on, the arc can be discretized into the connection of tiny line segments,

then the situation where a straight line meets an arc or an arc meets an arc can be equivalent to

the connection of a straight line to a straight line, as shown in below figure. The speed at the

junction of the two can be processed by the corner deceleration.

Connection between straight

line and arc

Connection between arc

and arc

Spline smoothing function

Parameter type

Parameter

Unit

Value range

Default

value

Axis parameter (servo

100209

-

-32767 to 32767

0

parameter)

380

Spline curve refers to a curve obtained by a given set of control points, which can be used to

describe free curves and curved surfaces. It is specified as a CAD/CAM data exchange standard

by the International Organization for Standardization. The chord line is usually used for

approximating the arc at the time of spline curve interpolation, and the accuracy depends on the

number of the approximating chord. As shown in the figure below; the system interpolation period

is 1ms, and the system is specified to run a full circle in 8ms, then it will approximate the circle

to a regular octagon, and the servo position control period is 0.2ms. After the spline smoothing

function is turned on (100 is set), the full circle spline can be approximated to a regular 40-sided

polygon.

a-a

1=135°

△d2

△d1

158°

2=

2> 1 △d2 >△d1

图（a）

图（a-a）

After the spline is smoothed, the included angle of the spline segment becomes larger, which is

beneficial to reduce the speed fluctuation and improve the surface finish; the contour error is

greatly reduced compared with the previous one, which reduces the loss of precision and improves

the processing accuracy.

Machining acceleration/deceleration time constant

Parameter type

Parameter

Unit

Value range

Default value

Axis parameter

100038

ms

0~2000.0

32

"Machining acceleration/deceleration time constant" refers to the time for linear axis (G01, G02,

etc.) to accelerate from 0 to 1000mm/min or decelerate from 1000mm/min to 0, as shown in the

figure below (T represents the machining acceleration deceleration time constant). This parameter

determines the axis's processing acceleration. The larger the processing acceleration/ deceleration

time constant, the slower the acceleration/deceleration. This parameter is set based on the motor

inertia moment, the load inertia, and the acceleration capability of the drive.

381

The comparison table of common machining acceleration/deceleration time constant and

acceleration is as follows:

Machining

acceleration/dec

2ms

8 ms

16 ms

32 ms

64 ms

eleration time

constant

Acceleration

1g

0.2g

0.1g

0.05g

0.02g

Example: The machining acceleration/deceleration time constant is set to 6ms, then the processing

acceleration is calculated as follows:

1000mm/60s≈16.667mm/s

16.667/0.006≈2778mm/s2≈0.283g

(1g=9.8m/s2 )

Machining acceleration/deceleration jerk time constant

Parameter type

Parameter

Unit

Value range

Default value

Axis parameter

100039

ms

0~2000.0

128

"Machining acceleration/deceleration jerk time constant" refers to the time when the acceleration

increases from 0 to 1m/s2 or decreases from 1m/s2 to 0 during axis machining movement (G01,

G02, etc.), as shown in the figure below (T represents the machining acceleration deceleration

jerk time constant). This parameter determines the machining jerk of the axis. The larger the time

constant, the smoother the acceleration changes. This parameter is set based on the motor, the

performance of the drive and the load, and is generally set between 8 and 150.

Example: Assuming that the processing acceleration is 0.05g (0.49m/s2) and the processing

acceleration/deceleration jerk time constant is set to 128ms, the jerk is 0.49/0.128≈3.8m/s3.

Machining acceleration time coefficient

Parameter type

Parameter

Unit

Value range

Default

value

Axis parameter

040156/040176/040196

-

0.01 to 100.0

1

Take the axis parameter "machining acceleration/deceleration time constant" as the reference

382

value, and use the "machining acceleration time coefficient" to convert the machining acceleration

/deceleration time to change the acceleration. The formula is as follows:

Converted value of machining acceleration/deceleration

time

= machining

acceleration/deceleration time constant * machining acceleration time coefficient

According to the characteristics of the processing program and the actual processing conditions,

this parameter can realize the flexible switching of the acceleration, and optimize the processing

efficiency or processing accuracy. When efficiency is the priority, this parameter can be

appropriately reduced; when accuracy is the priority, this parameter can be appropriately

increased.

Example: The machining acceleration/deceleration time constant is set to 8ms in the axis

parameters, and the corresponding acceleration is 0.2g. When the machining acceleration time

coefficient is 0.25, the machining acceleration/deceleration time is converted to 2ms, and the

corresponding acceleration becomes 1g.

Machining jerk time coefficient

Parameter type

Parameter

Unit

Value range

Default

value

Axis parameter

040157/040177/040197

-

0.01 to 100.0

1

Taking the axis parameter "machining acceleration/deceleration jerk time constant" as the

reference value, the machining acceleration/deceleration jerk time is converted through the

"machining jerk time coefficient" to change the time that the acceleration increases. The

conversion formula is as follows:

Converted value of machining jerk time = machining acceleration/deceleration jerk time constant

* machining acceleration time coefficient

Through this parameter, the acceleration speed can be flexibly switched, and the acceleration

change can be reasonably controlled to ensure the stability of the machining.

Example: Assuming that the current processing acceleration is 0.05g (0.49m/s2) and the axis

parameter "machining acceleration/deceleration jerk time constant" is set to 64ms, the jerk is

0.49/0.64≈7.6m/s3. When the machining acceleration time coefficient is 2, the converted value of

the machining acceleration/deceleration time is 128ms, and the corresponding jerk becomes 3.8

m/s3.

Example

In the actual CNC machining process, different machining processes and part contours will

produce parts processing procedures with their own characteristics, and different machining

requirements will also bring different control modes. Efficiency and precision are the two ends of

the balance of CNC machining. Therefore, only the combination of the above parameters can be

adjusted according to the specific processing object and customer needs, so that the efficiency

383

and accuracy can be biased or reach a suitable balance point, so that the overall processing effect

can be optimized. The following explains the combination adjustment of parameters through

practical application examples.

Cleanup machining parameter application

The cleanup machining is popular in 3C industries including mobile phone casings and circuit

board fixtures.

The contour path is shown as below

① In the actual processing process, the requirements for the cleanup machining efficiency is high,

that is, the processing time is as short as possible.

② It can be seen from the machining process and machining contour that the machining requires

high precision at 90-degree corners, and there is no actual effective cutting on the arc segment, so

there is no need to consider the contour accuracy.

③ The overall machining contour is small, there are connections between straight lines and arcs,

as well as G00 and G01, the speed changes quickly, and the speed fluctuates greatly. As shown in

the figure below, the single-axis speed curve has a sudden change in speed. During the actual

processing, this sudden change in speed is the main cause of severe vibration of the machine tool.

384

Parameter combination application

① To meet the high-efficiency requirements of machining, improve the system's acceleration

capability, that is, reduce the machining acceleration/deceleration time constant and the

machining acceleration/deceleration jerk time constant to the suitable values, but the values

should not be too small to cause excessive acceleration and increase the vibration of the machine

tool. For example, when the acceleration time constant and the jerk time constant are 4 and 1, 2

and 2 respectively in the actual debugging, and the machining time is the same. However, when

the acceleration time constant is 2, the acceleration is too large and the machine vibration is severe,

so choose the appropriate acceleration time constant as 4.

② For the sudden change of single-axis, increase the command speed smoothing coefficient to

make the speed transition smoothly. As shown in the figure below, in the actual machining process,

when the command speed smoothing coefficient is 40, the machine vibration almost disappears.

Without command speed smoothing

Command speed smoothing periods： 40 (ms)

Time (s)

Time (s)

③ Since the accuracy of this machining arc is not high, the centripetal acceleration can be

increased, and the circular cutting feedrate can be increased; at the same time, in order to improve

the processing efficiency, reduce the minimum internal angle value of corner smoothing and

increase the corner deceleration factor to increase the feedrate at the corner.

385

Parameter setting

Parameter

Set value

Machining acceleration time

4

constant (ms)

Machining acceleration jerk time

1

constant (ms)

Command speed smoothing periods

40

(ms)

Min. interior angle of corner

80

smoothing（°）

Corner deceleration factor (%)

90

Centripetal acceleration (mm/s2)

6000

Combination application of laser processing parameters

Laser cutting is widely used in contour processing. Take the "horse" contour as an example here;

The contour path is shown in the figure below:

Analysis of processing requirements and characteristics:

① It can be seen from the outline of the horse that it has hair shape processing on the horse head

and tail which need a large number of sharp corner processing, and the speed fluctuates greatly.

② According to the laser cutting processing requirements of the horse shape, when a certain

processing time is ensured, the sharp corners of the processing contour must be sharp, and there

is no rounded corners.

③ The processing speed is high and above F10000, and its acceleration is required to be close to

1g, but at the same time it is necessary to ensure that the machine vibration is small.

386

Parameter combination application

① For problems such as large speed fluctuations and strong machine tool vibration, and its sharp

corners are processed into a large number of small line segments, the spline smoothing function

is turned on to smooth the speed step changes in the high-speed section.

② Although the command speed smoothing function can effectively reduce speed fluctuations,

but the excessive large value will change the sharp corners to rounded corners, so the command

smoothing speed here should not be too high. In the actual debugging the value of 5 can reduce

machine vibration , improve efficiency without affecting the shape of horse's hair.

③ For the acceleration requirement of 1g, the machining acceleration time constant must be

reduced. The appropriate value is 2. However, the vibration of the machine tool increases due to

excessive acceleration changes. Therefore, the acceleration jerk time constant is reduced to lower

the acceleration change and increase the smoothness of the axis in the acceleration and

deceleration stages, reducting machine vibration.

④ The processed parts require high precision and processing time. Appropriately reduce the

centripetal acceleration so that the deceleration is performed at the small arc; increase the

minimum interior angle of corner smoothing to improve the corner contour accuracy; adjust the

appropriate corner deceleration factor to keep its value about 70, then the balance of accuracy and

efficiency is ensured.

Parameter setting reference value

Parameter

Set value

Machining acceleration time constant (ms)

2

Machining acceleration jerk time constant

10

(ms)

Command speed smoothing periods (ms)

5

Min. interior angle of corner smoothing

130

（°）

Corner deceleration factor (%)

70

Centripetal acceleration (mm/s2)

2500

Spline smoothing coefficient

100

Note

1) In HNC8 CNC system, multiple sets of small line segment control parameters are used to

achieve different parameter combination control, which includes the various control parameters

described above that play a major role in processing accuracy and efficiency.

2) As shown in the above example, according to the specific processing technology and processing

requirements, different parameter combinations are summarized to set the small line segment

387

Content      ..     8      9      10