Content      ..     2      3      4      5     ..

SINUMERIK 840D sl. Training. Operate - Turning (2016-2020) - page 4

Advantages of ShopMill

2.1 You will save time for training

2.1

You will save time for training

• ShopMill does not use any foreign-language terms you would otherwise have to learn. All

required inputs are requested in plain text.

• When working with ShopMill, you are assisted optimally by colored help displays.

Easy milling with ShopMill

10

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Advantages of ShopMill

2.1 You will save time for training

• You can also integrate DIN/ISO commands into the Process Plan of ShopMill. You may also

program in DIN/ISO 66025 and use DIN cycles.

• You may switch between the individual work step and the workpiece graphic at any time

when creating a process plan.

Figure 2-1

Work step in a process plan

Figure 2-2

Graphic view

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

11

Advantages of ShopMill

2.2 You will save time for programming...

2.2

You will save time for programming...

• ShopMill already assists you in entering the technological values: You will only have to enter

the handbook values feed/tooth and cutting rate - speed and feedrate are calculated by

ShopMill automatically.

• ShopMill enables you to describe a complete machining sequence using only one work step,

and the required positioning motions (in this case, from the tool change point to the

workpiece and reverse) are created automatically.

• All work steps are represented by ShopMill in a compact and clear fashion in the Graphical

Process Plan. This provides you a complete overview and thus better editing possibilities

even if comprehensive manufacturing sequences are to be performed.

• In drilling, for example, several machining operations can be connected together so that they

need not be called repeatedly.

Easy milling with ShopMill

12

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Advantages of ShopMill

2.2 You will save time for programming...

• The integrated contour calculator can process all standard dimensions (Cartesian, polar); it

is nevertheless very easy to handle and understand - thanks to colloquial input and graphic

support.

Figure 2-3

Technical drawing

Figure 2-4

Screenform

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

13

Advantages of ShopMill

2.2 You will save time for programming...

• You may switch between the graphic view and parameter screenform with help display at any

time.

Figure 2-5

Parameter screen with help display

• Process plan and manufacturing do not exclude each other. With ShopMill, you can create a

new process plan parallel to manufacturing.

Easy milling with ShopMill

14

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Advantages of ShopMill

2.3 You will save time for manufacturing...

2.3

You will save time for manufacturing...

• You need not take into account the pocket radii when selecting the milling cutter for

removing the contour pockets from the solid: Any residual material ① is detected and

removed automatically using a smaller milling cutter.

1

• There are no unnecessary infeed motions between retraction and machining planes when

positioning the tool. This is made possible by the settings Retract to retraction plane (RP)

and Optimized retraction.

The Optimized retraction setting is to be made by a skilled worker in the program header.

He must take into account obstacles, such as clamping elements.

Retraction to retraction plane (RP)

Retraction to retraction planes = time saved in

manufacturing

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

15

Advantages of ShopMill

2.3 You will save time for manufacturing...

• You can optimize your machining sequence with a minimum of work - thanks to the compact

structure of the process plan (in this case, by saving of a tool change, for example).

Figure 2-6

Original machining sequence

Figure 2-7

Optimized machining sequence with cutting and pasting a work step

• With ShopMill, you can achieve extremely high feedrates with optimum repeat accuracy

based on consistent digital technology (SINAMICS drives,

, SINUMERIK control systems).

Easy milling with ShopMill

16

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

To make everything function smoothly...

3.1 Multitouch operation of SINUMERIK Operate

3.1

Multitouch operation of SINUMERIK Operate

3.1.1

Screen layout

Touch and gesture operator controls for SINUMERIK Operate with the "SINUMERIK Operate

Generation 2" user interface.

① Cancel alarms

② Function key block

③ Virtual keyboard

3.1.2

Function key block

Operator control

Function

Switch operating area

Tap the current operating area, and select the desired operating area from the

operating area bar.

Switch operating mode

The operating mode is only displayed.

To switch the operating mode, tap the operating area and select the operating

area from the vertical softkey bar.

The selection for the functions available for the operating mode is opened.

Easy milling with ShopMill

18

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

To make everything function smoothly...

3.1 Multitouch operation of SINUMERIK Operate

Operator control

Function

Close the selection

The selection for the functions available for the operating mode is closed.

Undo

Multiple changes are undone one by one.

As soon as a change has been completed in an input field, this function is no

longer available.

Restoring

Multiple changes are restored one by one.

As soon as a change has been completed in an input field, this function is no

longer available.

Virtual keyboard

Activates the virtual keyboard.

Calculator

Displays a calculator.

Online help

Opens the online help.

Camera

Generates a screenshot.

3.1.3

Further operator touch controls

Operator control

Function

Advances to the next horizontal softkey bar.

When page 2 of the menu is called, the arrow appears

on the right.

Advances to the higher-level menu.

Advances to the next vertical softkey bar.

Tapping the Cancel alarm symbol clears all queued can-

cel alarms.

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

19

To make everything function smoothly...

3.1 Multitouch operation of SINUMERIK Operate

3.1.4

Virtual keyboard

If you called the virtual keyboard using the function key block, then you have the option of

adapting the key assignment using the shift keys.

① Shift key for uppercase and lowercase letters

② Shift key for letters and special characters

③ Shift key for country-specific keyboard assignment

④ Shift key for full keyboard and numerical key block

Hardware keyboard

If a real keyboard is connected, the icon of a minimized keyboard appears in place of the virtual

keyboard.

Use the icon to open the virtual keyboard again.

3.1.5

Finger gestures

Finger gestures

Tap

• Select window

• Select object (e.g. NC set)

• Activate entry field

- Enter or overwrite value

- Tap again to change the value

Tap with 2 fingers

• Call the shortcut menu (e.g. copy, paste)

Easy milling with ShopMill

20

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

To make everything function smoothly...

3.1 Multitouch operation of SINUMERIK Operate

Flick vertically with one finger

• Scroll in lists (e.g. programs, tools, zero points)

• Scroll in files (e.g. NC program)

Flick vertically with two fingers

• Page-scroll in lists (e.g. ZO)

• Page-scroll in files (e.g. NC programs)

Flick vertically with three fingers

• Scroll to the start or end of lists

• Scroll to the start or end of files

Flick horizontally with one finger

• Scroll in lists with many columns

Spread

• Zoom in on graphic contents (e.g. simulation, mold mak-

ing view)

Pinch

• Zoom out from graphic contents (e.g. simulation, mold

making view)

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

21

To make everything function smoothly...

3.1 Multitouch operation of SINUMERIK Operate

Pan with one finger

• Move graphic contents (e.g. simulation, mold making

view)

• Move list contents

Pan with two fingers

• Rotate graphic contents (e.g. simulation, mold making

view)

Tap and hold

• Open input fields to change

• Activate or deactivate edit mode (e.g. current block dis-

play)

Tap and hold using 2 fingers

• Open cycles line by line to change (without input screen

form)

Tap with two index fingers

• Tap with two fingers simultaneously in the lower right- and

left-hand corners to open the TCU menu.

The menu has to be opened for service purposes.

Note

Flicking gestures with several fingers

The gestures only function reliably if you hold your fingers sufficiently far apart. The fingers

should be at least 1 cm apart.

Easy milling with ShopMill

22

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

To make everything function smoothly...

3.2 The operating areas

3.2

The operating areas

3.2.1

Machine

Machine - Manual

Select the "Machine" softkey.

Switch to "JOG" mode.

In this mode, the machine is set up; the tool is traversed in the MANUAL mode. It is also possible

to gauge tools and to set workpiece zeros.

Figure 3-1

Call of a tool and input of technological values

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

23

To make everything function smoothly...

3.2 The operating areas

Figure 3-2

Input of a target position

Machine - AUTO

Select the "Machine" softkey.

Switch to "AUTO" mode.

During manufacturing, the current work step is displayed. It is possible to switch to a running

simulation using the relevant key ("Simultaneous recording"). When executing a process plan,

you may insert work steps and/or create a new process plan.

Easy milling with ShopMill

24

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

To make everything function smoothly...

3.2 The operating areas

3.2.2

Parameters

Parameter lists

This key can be used to edit data for the tool management and for programs.

Tool lists

No cutting without tools.

The tools can be managed in a tool list.

Figure 3-3

Tool list

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

25

To make everything function smoothly...

3.2 The operating areas

Magazine

Tools can be organized into a magazine.

Figure 3-4

Magazine

Work offsets

Zero points are saved in a clearly laid-out zero-point table.

Figure 3-5

Work offsets

Easy milling with ShopMill

26

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

To make everything function smoothly...

3.2 The operating areas

3.2.3

Program

Editing programs

This key can be used to edit programs.

If you have created a ShopMill program in the Program Manager, you can now create the

process plan with the complete machining sequence for the appropriate workpiece.

Prerequisites for the optimum order of sequence are the experience and knowledge of the

skilled worker.

The contour to be machined is entered graphically as a machining step.

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

27

To make everything function smoothly...

3.2 The operating areas

Geometry and technology constitute a unit in programming. The subsequent technological

machining operations are applied to the contour.

Example for the dovetailing of geometry and technology:

&RQWRXU

3DWK PLOOLQJ LQFO DSSURDFK DQG UHWUDFW VWUDWHJLHV

&LUFXODU SRFNHW LQFO WHFKQRORJ\ DQG SRVLWLRQ

%RULQJ WHFKQRORJ\

3RVLWLRQ IRU ERULQJ

&HQWHULQJ WHFKQRORJ\

'ULOOLQJ WHFKQRORJ\

3RVLWLRQV IRU FHQWHULQJ DQG GULOOLQJ

This geometrical-technological interrelation is represented very clearly in the graphical display

of the work steps by putting the appropriate symbols in brackets. The brackets mean linking of

geometry and technology to one work step.

Simulating programs

Before machining a workpiece on the machine, it is possible to display the program execution

graphically on the screen.

• To this end, select the "Simulation" and "Start" softkeys.

• To stop simulation, select the "Stop" softkey.

• To cancel simulation, use the "Reset" softkey.

The following views are available for simulation:

Figure 3-6

Top view

Easy milling with ShopMill

28

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

To make everything function smoothly...

3.2 The operating areas

Figure 3-7

3D view

Figure 3-8

Side view

3.2.4

Program Manager

Managing programs

With the Program Manager, you can create new programs at any time. You can similarly open

existing programs to execute, modify, copy or rename them. Programs no longer required can

be deleted.

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

29

To make everything function smoothly...

3.2 The operating areas

Active programs are marked with a green symbol.

USB flash drives can be used for data exchange. For example, programs which were created on

an external device can be copied and executed on the NC.

Creating a new workpiece

You can manage your programs and other files, such as tool data, zero points, magazine

mapping, in a workpiece.

Creating a new program

If you create a new program, you can specify the type of programming using the following

softkeys:

ShopMill program

G code program

3.2.5

Diagnosis

Alarms and messages

Here you can see alarm lists, messages and alarm logs.

Easy milling with ShopMill

30

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

To make everything function smoothly...

3.2 The operating areas

Figure 3-9

Alarm log

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

31

Geometrical basics

4.1 Tool axes and work planes

4.1

Tool axes and work planes

On universal milling machines, the tool can be mounted parallel to any of the three main axes.

These perpendicular axes are aligned to the main guideway of the machine according to DIN

66217 or ISO 841.

The appropriate working plane results from the mounting position of the tool. Z is the tool axis

in most cases.

Figure 4-1

Vertical spindle

On modern machines, the tool mounting position is changed without any modification and in

a few seconds by way of a universal swivel head.

Figure 4-2

Horizontal spindle

If the coordinate system shown on the previous page is rotated accordingly, the axes and their

directions in the appropriate working plane (DIN 66217) will change.

With the "Various" and "Settings" softkeys, you can call a parameter screenform in which you can

specify the working planes in the program header.

Select the "Various" softkey.

Select the "Settings" softkey.

Easy milling with ShopMill

34

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Geometrical basics

4.1 Tool axes and work planes

Figure 4-3

The "Working planes" parameter screenform

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

35

Geometrical basics

4.2 Points in the work space

4.2

Points in the work space

Various important reference points are provided for a CNC - such as the SINUMERIK 828D with

ShopMill - for orientation in the working space by way of the measuring system.

Machine zero (M)

The machine zero (M) is specified by the manufacturer and cannot be changed. It lies in the

origin of the machine coordinate system.

Workpiece zero (W)

The workpiece zero (W) - also called program zero - is the origin of the workpiece coordinate

system. It can be selected freely and should be located at a point from which the most

dimensions start in the drawing.

Reference point (R)

The reference point (R) is approached to set the measuring system to zero, as the machine zero

cannot be approached in most cases. Thus, the control system finds the start of counting in the

position measuring system.

Easy milling with ShopMill

36

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Geometrical basics

4.3 Absolute and incremental dimensioning

4.3

Absolute and incremental dimensioning

Absolute input

The entered values refer to the workpiece zero.

With absolute inputs, the absolute coordinate values of the end point must always be entered

(the starting point is not taken into account).

Incremental input

The entered values refer to the starting point.

With incremental inputs, the difference values between starting point and end point must

always be entered, observing the direction.

Click on the toggle field to switch between the absolute and incremental input.

A few examples for the absolute/incremental combination can be found below:

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

37

Geometrical basics

4.3 Absolute and incremental dimensioning

$EVROXWH

$EVROXWH

$EVROXWH

;

<

;

<

;

<

,QFUHPHQWDO

,QFUHPHQWDO

,QFUHPHQWDO

;

<

;

<

;

<

Easy milling with ShopMill

38

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Geometrical basics

4.4 Linear motions

4.4

Linear motions

Two specifications are required to define an end point unambiguously. These specifications

could be:

Cartesian

Input of the X and Y coordinates.

Polar

Input of the length and an angle.

Angle 38.13° = angle with reference to the previous element

or

angle 53.13° = starting angle with reference to the positive X axis

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

39

Geometrical basics

4.4 Linear motions

Cartesian and polar

It is possible to combine Cartesian and polar inputs, e.g.:

• Input of the end point in Y and the length.

• Input of the end point in X and of an angle (either 38.13° or 53.13°)

Easy milling with ShopMill

40

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Geometrical basics

4.5 Circular motions

4.5

Circular motions

In the case of arcs, X and Y specify the end point; the circle center is specified with I and J. In

ShopMill, these four values can be entered separately - either as absolute or incremental

dimensions.

While X and Y are entered as absolute dimensions, the center point is specified with I and J as an

incremental dimension in the most control systems. Not only the difference from the starting

point A to the center M must be determined (often even in combination with mathematic

calculations), but also the direction and thus the sign.

When working with ShopMill, however, you need not perform any calculations thanks to the

possibility of entering the center point as an absolute dimension - even the most complicated

contour can be determined easily using the graphical contour calculator.

Input of the center point (absolute)

Values (here: radii) which result from data already entered are calculated by ShopMill

automatically.

<

$

0

(

(

$

0

;

After the input:

After the input:

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

41

Geometrical basics

4.5 Circular motions

Display of all parameters

ShopMill also allows to display all possible geometry values:

<

$

-

0

(

(

,

$

0

-

,

;

A further advantage of absolute center-point dimensioning: You need not recalculate the values

for I and J when reversing the milling direction.

Easy milling with ShopMill

42

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Well equipped

5.1 Tool management

5.1

Tool management

ShopMill offers three lists for tool management:

• Tool list (Page 44)

• Tool wear list (Page 45)

• Magazine list (Page 46)

5.1.1

Tool list

The tool list displays all parameters and functions required to create and set up the tools.

Figure 5-1

Example for tool lists

Meaning of the most important parameters in the tool list:

Location

Location number

Type

Tool type

Tool name

The tool is identified by the name and the replacement tool number. You

may enter the names as text or numbers.

ST

Replacement tool number (for replacement tool strategy)

D

Cutting edge number

Length

Tool length

Diameter

Tool diameter

Point angle or lead

Point angle or lead

N

Number of teeth

Direction of spindle rotation

Coolants 1 and 2 (e.g. internal and external cooling)

Easy milling with ShopMill

44

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Well equipped

5.1 Tool management

ShopMill provides various tool types (favorites, milling cutters, drills, and special tools). Tools

can be created in the tool list by means of a predefined tool catalog. The geometrical parameters

(e.g. angle specifications for drills) are different for each tool type.

Figure 5-2

Example of Favorites list

5.1.2

Tool wear list

The wearing data for the appropriate tools are defined here.

Figure 5-3

Tool wear list

The most important tool wearing parameters are:

Δ Length

Length wear

Δ Radius

Radius wear

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

45

Well equipped

5.1 Tool management

TC

Selection of tool monitoring

• by tool life (T)

• by count (C)

• by wear (W)

Tool life or

Tool life

workpiece count or

Number of workpieces

wear *

Tool wear

*Parameter depends on selec-

tion in TC

Setpoint

Setpoint for tool life, workpiece count, or wear

Prewarning limit

Specification of the tool life, workpiece count or wear at which a

warning is displayed.

G

The tool is disabled when the checkbox is selected.

5.1.3

Magazine list

All tools that are assigned to one or several tool magazines are contained in the magazine list.

This list displays the condition of each tool. Individual magazine locations can be reserved or

disabled for existing tools.

Figure 5-4

Magazine list

Meanings of the most important parameters:

G

Disabling of the magazine location

Ü

Marking of a tool as oversized. The tool occupies two half locations left, two half locations right, one

half location top and one half location bottom in a magazine.

P

Fixed location coding

The tool is permanently assigned to this magazine location.

Easy milling with ShopMill

46

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Well equipped

5.2 Tools used

5.2

Tools used

In this section you will learn how to enter tools required for the later machining in the tool list.

Select the "Parameters" area in the main menu.

Select the "Tool list” softkey.

To create a new tool, call the tool list and search for a free location.

Select the "New tool" softkey.

Select the desired tool type from the tool catalog displayed. This tool type is inserted in the tool

list and you can enter the data of the tool.

Note

The milling cutters with the diameters 6, 10, 20 and 32 (Cutter6, 10, 20 and 32) must immerse,

as they will also be used for the milling of pockets in the following examples.

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

47

Well equipped

5.3 Tools in the magazine

5.3

Tools in the magazine

In the following you will learn how to insert the tools into the magazine.

Select a tool without location number from the tool list and select the "Load" softkey.

The following dialog offers the first free magazine location for you to change or accept directly.

The magazine for the following exercises could look like the one in the screen below:

Easy milling with ShopMill

48

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Well equipped

5.4 Gauging tools

5.4

Gauging tools

In the following you will learn how to calculate tools.

Insert a tool from the tool list into the spindle using the "T,S,M" softkey.

Then switch to the "Gauge tool" menu.

The tool is measured in the Z direction using the Length, manual function.

The diameter of the tool is measured using the Diameter, manual function.

The Length, autom. function can be used to measure the tool in the Z direction using a tool

probe.

The Diameter, autom. function is used to measure the diameter of the tool using a tool probe.

The Calibrate probe function is used to determine the position of the sensing probe on the

machine table with reference to the machine zero.

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

49

Well equipped

5.4 Gauging tools

The Fixed-point calibration function is used to determine the fixed point used as the reference

point for measuring the tool length manually.

Easy milling with ShopMill

50

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Well equipped

5.5 Setting the workpiece zero

5.5

Setting the workpiece zero

To set the workpiece zero, switch to the Machine - Manual mode in the main menu.

The submenu of the Workp. zero option offers various possibilities to set the workpiece zero.

The zero point of a workpiece edge will be set in the following example using a 3D probe.

Step 1: Selecting the edge

Define the sampling direction for the probe: LH (+) or (-). The X0 parameter can be used to

specify an offset for the workpiece zero if the zero is not to lie on the edge of the workpiece.

Step 2: Sampling the workpiece edge

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

51

Well equipped

5.5 Setting the workpiece zero

Step 3: Set the workpiece zero taking into account the edge probe diameter (5 mm). Now this

process of calculation must be repeated for Y using the edge probe and for Z (in most cases, with

the milling cutter).

Since the workpieces to be machined are not always present in the form of a cuboid or can be

clamped at right angles, further calculation possibilities are provided:

Example 1: Any corner

If the workpiece is positioned as shown here, the position/corner of the workpiece can be

determined by approaching four points.

Easy milling with ShopMill

52

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Well equipped

5.5 Setting the workpiece zero

3D probes are offered in both the electronic and mechanical variants. The signals issued by

electronic probes can be processed by the control system directly.

3D probe, electronic

3D probe, mechanical

Example 2: Calculating a drill hole

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

53

Well equipped

5.5 Setting the workpiece zero

Example 3: Calculating a circular spigot

If an electronic 3D probe from the tool magazine is inserted into the spindle, clamping tolerances

will occur. This would lead to incorrect results in further measurements. This can be avoided by

calibration of the 3D probe at any reference surface or in any reference drill hole using the

Calibrate probe cycle.

Figure 5-5

Calibrating the probe for the length

Easy milling with ShopMill

54

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Well equipped

5.5 Setting the workpiece zero

Figure 5-6

Calibrating the probe for the radius

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

55

Example 1: Longitudinal guide

6

6.1

Overview

Learning objectives

This section will explain the first steps to create a workpiece in detail. You will learn how to...

• create and manage programs;

• call tools and perform a cutter radius compensation;

• enter traversing paths;

• create drill holes and handle position repetitions.

Task

Figure 6-1

Workshop drawing - Example 1:

Figure 6-2

Workpiece - Example 1:

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

57

Example 1: Longitudinal guide

6.1 Overview

Note

ShopMill always saves the last setting selected with the toggle field. Therefore, make sure that

all units, texts and symbols are specified as in the dialog boxes shown here in all toggle fields.

Whenever it is possible to switch, this is indicated in the help text by the

icon (see screenshot

below).

Figure 6-3

Toggle field with help text

Easy milling with ShopMill

58

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Example 1: Longitudinal guide

6.2 Program management / creating programs

6.2

Program management / creating programs

Operating sequences

After power-up of the control system, you are in the main menu.

Figure 6-4

Main screen

Open the basic menu. In the main menu, you may call various areas of ShopMill.

Figure 6-5

Main menu

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

59

Example 1: Longitudinal guide

6.2 Program management / creating programs

Select the Program Manager softkey. The Program Manager is opened.

In the Program Manager, you can manage process plans and contours (e.g. "New", "Open",

"Copy", ...).

Use the cursor key or right-click to select the 'Workpieces' directory.

Figure 6-6

Program Manager

Open the "Workpieces" directory.

Enter the name 'EXAMPLE1' for the workpiece.

Figure 6-7

Creating a workpiece

Confirm your input. The following dialog box is opened:

Figure 6-8

Creating a step sequence program

Select the input format using the ShopMill and ProgramGUIDE G code softkeys.

Via the ShopMill softkey, you specify the program type.

Specify the name of the process plan, in this case 'Longitudinal_guide'.

Easy milling with ShopMill

60

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Example 1: Longitudinal guide

6.2 Program management / creating programs

Press "Accept" to apply your input.

After confirming, the following interactive screenform is displayed to enter the workpiece data.

Figure 6-9

Program header - Help display

Enter the workpiece data and general program specifications in the program header.

Enter the following values:

Field

Value

Toggle field

Notes

Unit of measurement

mm

X

Work offset

G54

X

Blank

Cuboid

X

X0

-75

Since the workpiece zero

lies centrally on the work-

Y0

-50

piece surface, the coordi-

nates of the left workpiece

corner have negative val-

ues.

X1

150 inc

X (for selection of inc/abs)

Y1

100 inc

X (for selection of inc/abs)

ZA

0

ZI

-20 abs

X (for selection of inc/abs)

PL

G17 (XY)

X

Retraction plane

100

Safety clearance

1

Machining direction

Synchronous

X

Retraction position pattern

Optimized

X

See below Retraction posi-

tion pattern

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

61

Example 1: Longitudinal guide

6.2 Program management / creating programs

Press "Accept" to apply the values entered. After confirming, the program header is displayed.

Figure 6-10

Program header, example 1 - Work step editor

Now the program has been created as the basis for further machining steps. It has a name, a

program header (pictogram "P") and a program end (pictogram "END"). The individual

machining steps and contours are stored in the program one beneath the other. The later

machining is performed from top to bottom.

You may call the program header again at any time to make changes or check the values.

Retraction position pattern

The position pattern can be set to "Optimized" (= time-optimized traversing distances) or

"Retraction plane".

Optimized retraction

To retraction plane (standard)

The tool traverses over the workpiece at the

The tool traverses back to the retraction plane

safety clearance in accordance with the speci-

and performs infeed to the new position.

fied contour.

Softkeys

Use this softkey to switch to the online graphic of the workpiece (see screenform below).

Easy milling with ShopMill

62

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Example 1: Longitudinal guide

6.2 Program management / creating programs

Figure 6-11

Program header - graphical view

Use this softkey to switch back to the help display.

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

63

Example 1: Longitudinal guide

6.3 Calling a tool and specifying cutter radius compensation

6.3

Calling a tool and specifying cutter radius compensation

Operating sequences

To call the required tool, proceed as follows:

Use this key to extend the horizontal softkey menu.

Select the Straight line Circle softkey.

Select the Tool softkey.

Open the tool list. Select the CUTTER 60 tool.

Figure 6-12

Tool list

Accept the tool into your program. After accepting the tool, specify the cutting rate 80 m/min (if

necessary, change the unit using the toggle field).

Figure 6-13

Tool cutting rate

Easy milling with ShopMill

64

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Example 1: Longitudinal guide

6.4 Specifying the distance to be traversed

6.4

Specifying the distance to be traversed

Operating sequences

Now enter the distances to be traversed:

Select the "Straight line" softkey.

Select the "Rapid traverse" softkey.

Enter the following values in the interactive screenform:

Field

Value

Toggle field

Notes

X

110 abs

X

Y

0 abs

X

Radius compensation

off

X

See below Radius compen-

sation

Figure 6-14

Specifying the distance to be traversed - Radius compensation

Press "Accept" to apply the values entered.

Select the "Straight line" softkey.

Select the "Rapid traverse" softkey.

Easy milling with ShopMill

66

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Example 1: Longitudinal guide

6.4 Specifying the distance to be traversed

Enter the following values in the interactive screenform:

Field

Value

Toggle field

Notes

Z

-10 abs

X

Radius compensation

Empty field

X

See below Radius compen-

sation

Figure 6-15

Specifying the distance to be traversed - Tool positioned in Z

Press "Accept" to apply the values entered.

Select the "Straight line" softkey.

Enter the following values in the interactive screenform:

Field

Value

Toggle field

Notes

X

- 110 abs

X

F

400 mm/min

X

Radius compensation

Empty field

X

See below Radius compen-

sation

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

67

Example 1: Longitudinal guide

6.4 Specifying the distance to be traversed

Figure 6-16

Specifying the distance to be traversed - First machining path

Press "Accept" to apply the values entered. After acceptance, the list of work steps looks like this:

Figure 6-17

Specifying the distance to be traversed - List of work steps

Select the "Tools" softkey and perform the following work steps without help.

Load the next tool CUTTER 16. After accepting the tool, specify the cutting rate 100 m/min.

Create the distance to be traversed according to the following list of work steps.

Figure 6-18

Specifying the distance to be traversed - Work step list

Easy milling with ShopMill

68

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Example 1: Longitudinal guide

6.4 Specifying the distance to be traversed

Figure 6-19

Specifying the distance to be traversed - Complete

Start simulation.

Figure 6-20

Simulation of the distance to be traversed

You may end simulation by selecting either the Simulation softkey again or any other softkey.

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

69

Example 1: Longitudinal guide

6.4 Specifying the distance to be traversed

Radius compensation

Selection

Result

Radius compensation is disabled. The milling cutter traverses with its center point along the

created contour.

The existing settings for the radius compensation is maintained.

The compensation is performed to the left of the contour in the milling direction.

The compensation is performed to the right of the contour in the milling direction.

Easy milling with ShopMill

70

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Example 1: Longitudinal guide

6.5 Creating drill holes and position repetitions

6.5

Creating drill holes and position repetitions

Operating sequences

Now enter the values for the drill holes and position repetitions. You will have to center, through-

drill and make threads for 12 drill holes.

Figure 6-21

Drilling positions

Select the Drilling softkey.

Select the Center softkey.

Open the tool list. Use the cursor key to select the CENTERDRILL 12 tool.

Accept the tool into your program. After accepting the tool, enter the following values:

Field

Value

Toggle field

Notes

F

150 mm/min

X

S

500 rpm

X

Diameter/tip

Diameter

X

Centering can be entered

with reference either to

the diameter or to the

depth (tip).

Since the drill holes pos-

sess a 0.5 mm chamfer,

you may specify a diame-

ter of 11 mm.

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

71

Example 1: Longitudinal guide

6.5 Creating drill holes and position repetitions

Figure 6-22

Centering

Press "Accept" to apply the values entered.

Proceed as follows to specify and link the drilling positions with the cutting data:

Select the Positions softkey.

Select the Positions softkey for the position pattern.

Figure 6-23

Positions - Individual drill holes

Easy milling with ShopMill

72

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Example 1: Longitudinal guide

6.5 Creating drill holes and position repetitions

Enter the following values for the two individual drill holes:

Field

Value

Toggle field

Notes

Coordinate system

Rectangular

X

Z0

-10

The starting depth is

-10mm.

X0

-50

Y0

0

X1

50 abs

X

Y1

0 abs

X

Note

If you deselect the Graphic view softkey, detailed help displays are displayed (see table below).

Positions

Position grid

Position circle

Help displays - Positions

Press "Accept" to apply the values entered.

Select the Positions softkey.

Select the Position circle softkey.

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

73

Example 1: Longitudinal guide

6.5 Creating drill holes and position repetitions

Figure 6-24

Position circle

Enter the following values:

Field

Value

Toggle field

Notes

Z0

-10

X0

0

Y0

0

α1

0

R

20

N

6

Positioning

Straight line

X

Use the "Positioning" field

to define how to approach

the drill holes within the

drill pattern. If the drill

holes lie in a circumferen-

tial groove, for example,

do not use "Positioning -

Straight line"; otherwise, a

contour violation would

result.

Along a straight line,

along a circle

Easy milling with ShopMill

74

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Example 1: Longitudinal guide

6.5 Creating drill holes and position repetitions

Press "Accept" to apply the values entered.

Select the Positions softkey.

Select the position grid softkey.

Figure 6-25

Position grid

Enter the following values:

Field

Value

Toggle field

Notes

Z0

0

X0

-65

Y0

-40

α0

0

L1

130

L2

80

N1

2

N2

2

Press "Accept" to apply the values entered.

Select the Drilling Reaming softkey.

Open the tool list. Use the cursor key to select the DRILL 8.5 tool.

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

75

Example 1: Longitudinal guide

6.5 Creating drill holes and position repetitions

Accept the tool into your program. After accepting the tool, enter the following values:

Field

Value

Toggle field

Notes

F

150 mm/min

X

V

35 m/min

X

Shank/tip

Shank

X

Specify the depth with ref-

erence to the shank incre-

mentally. In other words:

The 1/3 D drill tip is taken

into account automatical-

ly.

Z1

20 inc

X

DT

0 s

X

Drilling is performed with-

out a dwell time.

Note

The work steps 'Centering', 'Drilling' and 'Tapping' are linked with each other automatically.

Figure 6-26

Drilling

Press "Accept" to apply the values entered.

Select the Thread softkey.

Select the Tapping softkey.

Easy milling with ShopMill

76

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

Example 1: Longitudinal guide

6.5 Creating drill holes and position repetitions

Open the tool list. Use the cursor key to select the THREADCUTTER M10 tool.

Accept the tool into your program. After accepting the tool, enter the following values:

Field

Value

Toggle field

Notes

P

1.5 mm/rev

X

S

60 rpm

X

SR

60 rpm

X

Z1

22 inc

X

The cutting depth must be

entered incrementally.

Figure 6-27

Thread

Press "Accept" to apply the values entered.

Select the Repeat position softkey.

The drilling positions are numbered consecutively during creation. The appropriate number is to

be found directly after the block number of the corresponding position pattern. Specify "Hole

matrix" for position 3.

Figure 6-28

Repeating a position

Easy milling with ShopMill

Training Documents, 05/2020, 6FC5095-0AB50-1BP2

77

Content      ..     2      3      4      5     ..