3.4.12.

3 Invert

It inverts the initial point with the final one of any geometric entity.

In order to invert the direction of one or more geometries:

- Select one or more geometric entities
-
The inversion is evident when the symbol linked with the geometric initial point has changed.

3.4.12.4 Initial point

It changes the initial point of a closed geometry (circle or polyline).

In order to modify the initial point of a closed geometry:

-
- move the mouse
- click with the left button of the mouse (for a new initial point )

The representation of the initial point is performed with an arrow that detects the position and
the direction.

3.4.12.5 Join

It creates a polyline by combining geometric entity with coinciding vertex.

In order to combine one or more geometries with coinciding vertex:

- Select one or more geometric entities
- click on the command "Join"

One or more polylines can be combined only with the entities that have coinciding vertex.
In case of more entities with coinciding vertex, the entities inserted in the polyline will follow the
selection order.

The direction of the new polylines is casual

100
3.4.12.6 Explode

This command explodes a polyline in all basic geometric elements in its structure.

In order to explode one or more polylines:

- select one or more polylines
-

The direction of the single entities will be the one inside the polyline.

3.4.12.7 Split geometry

By selecting a 2D geometry of the arc,

segment or polyline type, it is possible to break
it at a point, creating two parts via the Split
geometry command in the Draw Edit menu.

The first part of the geometry will go from the

start point of the geometry (geometries always
have a start point and an end point, coincident
for closed geometries) to the point selected
with the mouse; the second part of the
geometry will go from the selected point to the
end point. If machining is associated with the
geometry to be split, splitting is not permitted and a message notifies the user of this if splitting
is attempted.

3.4.12.8 Editing geometries with the mouse

You can modify any geometry by using the mouse directly rather than through tables (recalling
properties and changing values of coordinates, radii, etc.).
The command is activated by the

CAD tool button for geometry modification.

If no geometry is selected at the start, the desired geometry selection is requested. Once the selection
has been made, grip points appear on the specified geometry that can be used for manual modification
of the geometry itself:

101
More precisely, grips are associated with the segments (visible as a thickened segment in a different
colour) and at the vertices or significant points of the curves:
for linear segments, the ends of the curve are shown for repositioning;
for the segments of the arc of a circle, in addition to the ends, the centre of the arc can be
modified (by moving the original circle) or the quadrant point to 0° to modify its radius, keeping
the centre and the ends stationary;
similarly, for the segments of an ellipse, the major and minor semi-axes of the ellipse and its
inclination can be modified;
for circles (and ellipses), it is possible to move their centre (and therefore the entire curve) and
modify their radius (or semi-axes and inclination);
for polylines, it is possible to move the vertices in common to two adjacent segments (by
stretching them both) or the centre of an arc (by changing its radius of curvature).
Osnaps can also be used to carry out controlled movements.

3.4.12.9 Simplifying a polyline (smoothing)

A very common occurrence when importing geometries from DXF files is to end up with
polylines made up of hundreds or thousands of very small segments. Machining of these curves
creates a variety of problems for the machines and the result is almost never satisfactory.
Furthermore, the presence of so many segments can lead to slowdowns in the calculations
required for their management.

The Simplify polyline command allows you to eliminate a considerable number of segments,
reducing the discrepancy between the original curve and the simplified curve.

The command is found in the Draw Edit menu or

in the context menu of the drawing area, (after
selecting the curve to simplify)

The parameters governing simplification are those relating to

the geometries in the appropriate section of the Maestro CNC
102
options (maximum chord error and discontinuity of the maximum tangent, in degrees).
You can also simplify all the polylines imported from DXF using a special check box on the
relevant import page:

By activating this check box, all the imported polylines will be simplified, reducing the complexity
of the curves and avoiding having to do this manually at a later time for each curve.

103
3.4.12.10 Change surfaces

There are two commands to change the surfaces:

- Extend surface;
- Intersection between surfaces.
- Cut surface
- Fillet between surfaces
- Chamfer between surfaces.

3.4.12.10.1 Extend surfaces

To extend the surface proceed as follows:

- select the surface to extend;

- enter the extension length values.

The surface extension occurs in tangency and it generates a new surface that replaces the
original one.

3.4.12.10.2 Intersection between surfaces

The surfaces intersection procedure is performed as follows:

- select the first surface;

- select the second surface.

104
3.4.12.10.3 Cut surface

The surface cutting procedure requires:

- selecting the surface to be cut;

- selecting one or more curves.

The permitted curves must be:

- Closed (if inside the surface)
- Open but with the initial and final points on the edge of the surface

The result will be to divide the original surface into two or more surfaces.

3.4.12.11 Fillet between surfaces

You can modify two or more contiguous surfaces (i.e. with one shared side) using the fitting
between surfaces command contained in the set of tools for modifying surfaces:

This command provides for the selection of two or more contiguous surfaces (if this is not the
case, an error message is displayed) and the radius of curvature to be given to the fitting
between them: if the radius is compatible with the selected surfaces, they will be modified
accordingly and a rounded surface will be inserted between them to fit them to each other:

105
3.4.12.12 Adapt piece to surfaces

3.4.12.12.1 Automatic counterprofile creation

To create a counterprofile of a solid model, use the

Create counterprofile from surfaces command in the
Draw Edit Fit workpiece to surfaces menu

As a first step, you are requested to select the surfaces of the solid model to make the
counterprofile. Once the surfaces have been selected, the Z value required to sink the 3D model
into the counterprofile is requested. Note that while the Z value is specified, the preview of the
counterprofile shape is shown in real time above the 3D model. Once the Z dimension is
confirmed, a new workpiece is created within the same project with the surfaces and
dimensions required to build the counterprofile (this typically requires one flush milling and one
or more finishing), plus some geometries that identify the contour of the cavity in which the 3D
model will be housed once it is turned and inserted in the counterprofile: these geometries can
be used for milling needed to insert a gasket to seal the workpiece. A third workpiece is
generated with the initial 3D model, upside down, at the Z dimension it will assume once
inserted in the counterprofile: the machining of this workpiece will complete the underlying part
of the initial workpiece.

3.4.12.12.2 3D model sectioning

This command allows you to create portions of a 3D model (consisting of surfaces), sectioning it
along a predetermined direction.
To launch the command, press the appropriate button in the group relating to management of a
workpiece associated with a 3D model:
Draw Edit Fit workpiece to surfaces 3D model sectioning

106
After selecting the surfaces of the model, the command requests the maximum size of the
section along the preselected axis.
The options allow for selection of the axis to cut (X, Y or Z): in this way, based on the maximum
acceptable size, theoretical section planes will be created and displayed showing the points
where the 3D model will be cut.

Each portion of the divided model will be inserted into a new workpiece: each workpiece created
will be added to the current project and its dimensions will be automatically adapted to the
surfaces.
Two other options are also available: the first allows you to create closing surfaces in
correspondence with the section points of the model, as long as this is made up of contiguous
surfaces so that the section curves are closed (some may be internal to the others). For user
convenience, the edge of this closing surface is added to the face where it is located.
A final option allows the sectioning command to add reference points on the faces originating
from the sectioning cuts as a suggestion for pin hole positioning: this guarantees absolute
correspondence in the drilling of two counterpoints on two opposite faces, even if the
workpieces to which they belong are of different sizes.

107
3.4.13 Move and/or copy the existing geometries

The icons on the commands to move, rotate, mirror or copy the existing geometries are to be

All commands of geometry modification are interrupted by selecting a new command or

pressing the button "Esc".

Further recurring commands are to be found in the menu "Home" "Clipboard".

108
3.4.13.1 Move

Move one or more entities from one point to another one.

In order to move one or more entities:

- select one or more entities
-
- type the reference point
- type the final point

Or:
-
- select one or more entities
- type the reference point
- type the final point

This command has three options:

- Create a copy
- Sequence (Single/Multiple)
- Coordinates (Relative/Absolute)

ws you to make a copy out of the source text.

The option Multiple Sequence allows you to keep on moving the element by typing further final
points.

The option "Absolute Coordinates" allows you to stop the select geometries at a certain level
starting from a zero level of the work plane.

109
3.4.13.2 Rotate

Rotate one or more entities.

In order to rotate one or more entities:

- select one or more entities
- click on the command

Or:
-
- select one or more entities

If you rotate two-dimensional elements:

- type the reference point
- set an angle (typing the point or inserting the value)

If you rotate three-dimensional elements i :

- Select an axis or a vector or define a vector by entering two points
- set an angle (typing the point or inserting the value)

This command has two options at disposal:

- Single Sequence
- Multiple Sequence)

The Multiple Sequence option allows you to continue rotating the selected items by making a
copy each time you set a new angle.

3.4.13.2.1 3D machining axis rotation

The rotation command is also applicable to 3D flush milling, finishing, 3D milling and inclined
hole machining. If one of these machining types is selected, the command sets itself to 3D
mode and requests an axis (instead of a point) around which to rotate the machining.
If ''Single sequence'' mode is enabled, only the 3D drillings can be rotated around the axis, as
they are not associated with surfaces; if "Multiple sequence" mode is enabled, each time the
Enter key is pressed, multiple copies of the selected 3D machining will be created, each rotated
(cumulatively) around the selected axis (with the same rotation modes as a surface around an
axis) by an amount equal to the specified angle.

110
3.4.13.3 Mirror

It mirrors one or more entities compared to the axis of the centre line in the work face.

This command works only in case of standard faces.

In order to mirror one or more entities:

- select one or more entities
-
- select the mirror mode in the menu
- click on the button "Apply"

This commands has five options:

- Mirror in X
- Mirror in Y
- Mirror in X/Y
- Keep in the source form
- Invert the working process

-axis of the centre line in the

active face.

-axis in the middle of the active

face.

The option "Mirror X/Y" mirrors the geometry compared to the X and Y axis in the middle of the
active face (this mode is like a rotation of 180°)

The option "keep the source geometry" allows you to make a copy out of the source geometry.

The optio

111
3.4.13.4 Oppose

It copies one or more entities on the standard face opposite to the active one.
The command is avai

This command works only in case of standard faces.

In order to copy one or more entities on the opposite standard face:

- select one or more entities
-
- click on the button "Apply"

This command has two options at disposal:

- Keep in the source form
- Invert the working process

The option "keep the source geometry" allows you to make a copy out of the source geometry).

allows you to invert the working direction if the

command "Oppose" is used for a working process.

112
3.4.13.5 Cut

It cuts one or more geometric elements or working processes in order to put them in the buffer

The command is available in

and works only for elements of the active face.

In order to cut one or more entities from the active face.

- select one or more entities
- -x"
- type one reference point.

As a result of the geometry of the selected working process it will disappear from the display.

3.4.13.6 Copy

It copies one or more geometric elements or working processes in order to put them in the
buffer of the option "Paste)
The command is available in the menu "Home" "Clipboard" as well as the "Contextual menu"
and works only for the elements of the active face.

In order to copy one or more entities from the active face:

- select one or more entities
- click on the command "Copy -c".
- type one reference point.

You do not notice any effect but the previously selected geometry will be available to be copied

3.4.13.7 Paste

It pastes one or more geometric elements or working processes that have previously been
selec

In order to paste one or more entities on the active face:

- -v"
- type one reference point.

113
3.4.14 Dimensioning

This function is used to enter only linear or angular quotas.

To enter a dimensioning use the "Linear dimensioning" or "Angular dimensioning" commands

on the "Change" menu.

After having selected the dimensioning command, a dialogue menu will appear asking you to
enter the selections to enter the dimensioning requested.
By default the dimensionings are lost, if you want to save one or more quotas on the project,
select the "Permanent" option before entering each quota.

114
3.5 Working processes

The commands in order to insert the working processes are to be found in the menu

Every working process must be carried out combining a tool with a 2D geometry.
As a result, it is necessary to activate a Tool- Data-Base (see paragraph 12.8)

In order to set any working process, it is useful to keep this structure in mind:
1) Set the position in which you carry out the working process (Pos)
2) Set the Geometric Shape of the working process (Geo)
3) Set the Work mode (Mode)
4) Set the technology adopted (tool, speed and so on).

115
3.5.1 Boring

In order to bore, you can:

-
- select one or more 2D elements

Or:
- select one or more 2D elements
- click on the command "Bori

The selection of 2D elements can be single or multiple as the

option for boring will make bores connecting them with the
points or the circles.

3.5.1.1 Bore position

If, among the selected elements, there are points and/or

circles, the bore position is automatically set.

If no point or circle has been selected, you can set the

position of a new point in this way:
- select the reference face
- select the reference edge on the face
- fill the field X Coordinate in
- fill the field Y Coordinate in

The reference edge on the face allows programming the hole with
X and Y coordinates that are related to the user-selected
reference point. In the case of pwx100 machines, if you want to
draw holes with coordinates relative to the mechanical zero of the
machine, for the upper face holes you must select the left upper
edge.

116
It is possible to set a set of matrix bores by using the sub-

to this purpose, the nearby menu fields must be filled in.

Rotat. 1 represents the angle to set the lines
Rotat. 2 stands for the angle to set the columns compared to the
lines

By clicking on the button "Preview", you obtain a

representative table that displays the bore position as
described above.

3.5.1.2 Bore structure

In order to set the bore structure, Diameter, Depth and bore Type must be set in the menu.

In field "Depth" you will insert the value corresponding to the

thickness of the workpiece in case the option "Passer-
selected.

If the "boring" operation has been performed by selecting a

c
with the value of the circle diameter.
In this case, if you wish to change the diameter, you can

diameter.

The field "Extra depth is filled with the extent through which the bore must go beyond the
thickness of such workpiece (this heading will appear only if the option "Passer-by" has been
selected")

The type of bore must be specified when it is not linked to a drilling tool and in this case, in order
to choose the tool, you need this information.

The hole types are as follows:

- Hole with flat bottom
- Hole with tapered bottom
- Counterbored hole in top part and with tapered bottom
- Blitz hole (with two diameters)

Select the types from the "Type of hole" field

117
3.5.1.2.1 Data entry for countersunk holes

When creating a countersunk hole, it is very useful to specify the depth of the countersink;
however, it is difficult to directly measure this depth and verify
whether a hole has been made precisely or not.
For this reason, next to the Countersink depth value, the
Countersink diameter has now been inserted (text field in
read-only, non-editable) which shows the expected diameter of
the countersink for the hole being made.
The reported countersink diameter is automatically calculated
based on the specified countersink depth, its diameter and
assuming the countersink is at 45°. This value can be easily
measured with a gauge and allows you to directly check the
accuracy of the hole once it has been made in the machine.

3.5.1.3 Boring mode

In order to set how to structure the bore, you use the sub-

The bore can be performed in a single or a multiple rub.

The following can be set with multi-pass:
- the "Number of passes" required to make the hole.

- The "Pass depth" visible when selecting "Enable

pass depth" field.

3.5.1.4 Boring technology

In this step, you set all technical aspects related to tools,

spindles and machines at disposal.

See the following chapters:

3.5.15 Technological data (shared by the machining operations)

3.5.17 Advanced data (common to machining)
3.5.18 Machine data (shared by the machining operations)

A speed profile can be set by selecting it from the drop down

Speed profiles" section (the
description of the speed profile can be found in chapter
3.5.2Speed profiles)

118
3.5.1.4.1 Drilling speed

The drilling feed speed can be set in the tool definition section (chapter Errore. L'origine
riferimento non è stata trovata.)

The section where the drilling speed can be set is from the safety quota to the hole end. This
section is partly outside the wood and partly inside.
e

Examples:

Tool data set:

Example 1
Value not set:
Feed equal to the Standard downstroke speed 5 m/min

Example 2
Value set at 9 m/min:
Feed 9 m/min (as it is slower than the Maximum feed speed
parameter 10 m/min)

Example 3
Value set at 12 m/min:
Feed 10 m/min (as it is faster than the Maximum feed speed
parameter 10 m/min)

Note: there are no controls for the minimum programmed speed, except for entering
negative values when editing in Maestro CNC, that is:

the error is signalled with a red box and the datum cannot be
validated/saved.

119
3.5.1.5 Drilling deduced from the surface

If a cylindrical surface is selected which refers to a hole, all the geometric parameters of the
dialog boxes will be automatically filled.
In the case of multiple selection of coaxial surfaces of suitable shape and position, the system
can recognize flared or counterbored holes.
The user can still modify the precompiled fields.

If a through hole is recognized, if possible a lance point will be used and a depth determined to
guarantee the through hole.

The condition in which the hole is made is that the hole axis is orthogonal to one of the six
planes of the part or to a previously created user plane.

120
3.5.2 Speed profiles
When drilling there is the risk of damaging the material being machined.
To prevent this you can vary the tool insertion speed during the whole drilling phase (initial
phase, intermediate phase, final phase and countersink phase).

To set the parameters go to "Tools - Speed

profiles - Create profile". A window will
appear to create various speed profiles.

The following window will appear

to set the various parameters in the specific sessions.

3.5.2.1 General data

This section is used to enter:

- Profile name
- Gain to apply to the Jerk

121
3.5.2.2 First entry (initial phase)

This section is used to set the speed during the entry of the tool in the panel being drilled. You
can also set from when it has to have this speed (Early, e.g.: From 0.5 mm from the piece) to
when the entry phase ends (Late, e.g.: From 1 mm from the piece).

Cl
must have during the phase based on the different tool diameters.

122
3.5.2.3 Feed (intermediate phase)

This section is used to set the speed of the tool in the next phase and before the final phase
(this is the intermediate phase). Various speeds can be selected based on the tool diameter.

123
3.5.2.4 Exit (final phase)

This section is used to set the speed during the exit of the tool from the object being drilled. You
can also set from when it has to change this speed (Early, e.g.: From 0.5 mm from the piece) to
when the exit phase ends (Late, e.g.: From 1 mm from the piece). The speed can be selected
based on the tool diameter.

124
3.5.2.5 Second entry (countersink phase)

This section is used to set the speed during the entry of the countersink/blading in the panel
being machined. You can also set from when it has to have this speed (Early, e.g.: From 0.5
mm from the piece) to when the countersink phase ends (Late, e.g.: From 1 mm from the
piece). The speed can be selected based on the tool diameter.

125
3.5.2.6 Return

This section is used to set the speed of the tool path section from the machining end to the
safety quota to remove the tool from the piece.
The speed can be selected based on the tool diameter.

126
3.5.2.7 Change speed profiles

To check or change the parameters go to

"Tools - Speed profiles - Display profile".

A window will appear with the list of all the profiles created up to then.
Right click on the profile to select the following items:
- Properties
- Copy
- Delete

Select Properties to open the section 3.5.2 Speed profiles

Select Copy to create a copy of the speed profile

Select Delete to delete the selected speed profile

127
3.5.2.8 Using the speed profiles

The speed profiles created can be used in two ways:

the first method consists of setting a profile created directly in the drilling properties. (See
chapter 3.5.1.4 Boring technology)

the second method Table of profiles

To create a table of profiles go to

"Tools - Table of profiles - Create
profile".
- Create profile". A window appears
to create various tables of profiles.

By creating a table of profiles you can set the profile (created previously) based on the tool and
table used to work.

128
3.5.2.8.1 Table of profiles default

To set a table of profiles Options Preferences Files of the table of

the drilling technology and select one of the previously created Table of profiles.

129
3.5.3 Inclined drilling

To insert one or more holes we can:

- click on the "Drilling" command
- select one or more 2D elements

Or:
- select one or more 2D elements
- click on the "Drilling" command

The 2D elements selected can be single or multiple because the

"Inclined drilling" function will produce holes by associating them
only with the points or circles.

3.5.3.1 Position of the inclined hole

If the selected elements have points and / or circles, the position

of the holes is determined automatically.

If no point or circle has been selected, the position of a new point

can be defined by entering the coordinates X, Y, Z

3.5.3.2 Shape of the inclined hole

To define the shape of the hole, the Diameter, Depth, Angles A and B Type of hole must be set
in the menu.

If drilling was done by selecting a circle instead of a point, the "Hole diameter" field will
represent the value of the circle diameter.

The Type of hole must be specified when no tool is associated with the drilling, and in this case,
this information is needed to make the automatic tool selection.
The types of hole are the following:
- Hole with flat bottom
- Hole with conical bottom
- Flared hole in the upper part and with a conical bottom
- Counterbored hole (Blitz)

The types can be selected from the "Hole type" field

The angles A and B are used to determine hole inclination.

130
3.5.3.3 Inclined drilling mode

The same applies to drilling

3.5.3.4 Inclined drilling technology

The same applies to drilling

3.5.3.5 Drilling deduced from the surface

If a cylindrical surface is selected which refers to a hole, all the geometric parameters of the
dialog boxes will be automatically filled.
In the case of multiple selection of coaxial surfaces of suitable shape and position, the system
can recognize flared or counterbored holes.
The user can still modify the precompiled fields.

3.5.4 Automatic drilling deduced from the surfaces

This function recognizes all the inclined holes and holes present in the selected surfaces.

To use this function, use the "Automatic

hole recognition" command in the
"Operations-3D Machining" menu

The operating mode is similar to that described in drilling and inclined drilling with the following
additional functions:

"Create User Plan for 3D Drilling" Creates a plane

for each recognized inclined hole.

"Fast surface analysis" will only recognize

cylindrical holes and involves a low processing
time.By removing the check to this parameter, also countersunk and counterbored holes will be
recognized at the cost of longer processing time.

Once the surfaces to be analysed have been selected, the maximum diameter below which the
surfaces are recognized as holes must be set.

The generated holes will start from the work plane closer to the hole geometry.
It is advisable to check the correct assignment of the tools which will perform inclined drilling.

If more than one hole has been generated on the same user plane, it is advisable to check that
they can be implemented by switching to the safety level from the user's plane, otherwise the
programming must be corrected.

131
"Circular pocket milling for too large holes"
The automatic hole recognition command requires the maximum diameter for which a cylindrical
cavity is recognised as a hole. This new option has been introduced to indicate whether or not
you want any cylindrical cavities with a diameter greater than the maximum allowed to be
recognised as circular pocket milling.
By activating this check box, all holes with a diameter greater than the set value will be
converted into circular pocket milling applied to the most appropriate plane. The tool will be
selected from the cylindrical cutters on the basis of the diameter and a message invites the user
to view the tool together with the various technological default parameters. If an appropriate tool
cannot be identified for one or more circular pocket millings, these are still created but a
message indicates the absence of a tool and invites the user to specify a suitable tool.

132
3.5.5 Milling

In order to insert one or more milling operations you can:

-
- select one or more 2D elements

Or:
- select one or more 2D elements
-

The selection of 2D elements can be single or multiple

because the function "Milling" will perform milling operations
connecting them with lines, polylines, arcs and circles.

3.5.5.1 Miling position

If there is any line and/or polyline and/or arc and/or circle

among the selected elements, the milling position is
automatically set.

The real position of every milling is affected by the used tool

correction and the super-material.

In the following tables it is possible to understand how the different combination of options work.

The light blue line stands for the "2D geometry" and the red line represents the tool path in the
tool centre.

the effective path (red line) will be calculated by the CN.

If you mark "

and this latest will not make any correction.

133
Behaviours with left, central and right corrections without any correction in length and without
any super-material.

Behaviours with left, central and right corrections in length and without any super-material.

134
Behaviours with left, central and right correction without any correction in length and with super-
material.

Behaviours with left, central and right corrections in length and with super-material.

135
3.5.5.2 Milling form

In order to set he milling form you have to set Length and Depth in the menu.

The field Width is automatically filled when a tool is

connected with the milling.

In field "Depth" you will insert the value corresponding to the

thickness of the workpiece in case the option "Passer-by is
selected.

The field "Extra depth" sets the extent of the milling to cross
the workpiece. (This heading will appear only the option
"Passer-by" has been selected)

The field "Indivisible processing" (currently used only for CX machines) ensures that such
machining is not performed in one or more stages for those automatically generated when using
CX
If an error is generated during the optimisation phase, the operator must replace the machining
operation with the selection with two or more machining operations that produce the same
operation.

3.5.5.3 Milling modes

In order to set how to perform the milling, you use the sub-menus "Strategy" and
"Approach/Removal".

The milling can be performed only in one or more rubs.

In case of "multi-rub", you must choose between One- way or

two- ways strategy.

In the "one-way strategy", you have to establish if the rise

between two rubs must occur:
- at a safety level on the workpiece
- or in the workpiece

Use the "Tools" "Options" "Parameters" "Machining" menus to

modify these two parameters.

136
For the one-way strategy as well as for the two ways strategy,
the heading "Enable multi-

If you leave the Pass depth parameter at zero and set only the
Last pass parameter, a first pass will be made at the set depth
minus the value set in Last Pass, and a second, last pass will
be made at the final depth.
Both numerical values and user parameters can be entered in
the fields relating to the two parameters.

For uni-directional strategy with multiple passes you can

extend the multiple passes to input and output sections by
placing th
Another modification to the milling mode can be set by the menu "Advanced data" through the
parameter "Invert".(See 3.5.17 Advanced data (common to machining)

By marking this parameter, the working process can be performed starting from the final point of
the selected 2D geometry.(See 3.5.16 Approach/Retraction (shared by the machining
operations))

3.5.5.4 Milling technology

See the following chapters:

3.5.15 Technological data (shared by the machining operations)

3.5.17 Advanced data (common to machining)
3.5.18 Machine data (shared by the machining operations)

137
3.5.6 Slanted routing

To enter one or more tilting routing proceed as follows:

-
- select one or more 2D elements

Or:
- select one or more 2D elements
- Slanted routing

The 2D elements selection can be single or multiple.

3.5.6.1 Tilting routing position

The position of the tilting routing is determined automatically by the geometry selected.
The tool correction is available only if the tool is perpendicular to the right or left and the Angle A
is equal to 0.
To use the tool correction see chapter 3.5.5.1 Routing position.

3.5.6.2 Tilting routing shape

To define the tilting routing shape set the parameters in the menu:

selected (cannot be edited).

axis X

Bear in mind that the positions are considered before the setting of

angle B will rotate the tool in the X-Z plane.

After having selected this mode, setting Angle A the tool axis will
no longer be parallel to axis x.
During the whole tilting routing in this mode the tool will always
maintain the same setup.

138
right in relation to the first geometrical entity of the trajectory.
The setup will be maintained for the whole machining operation.

geometrical entity of the trajectory.

The setup will be maintained for the whole machining operation.

an inclination of Angle B set in the

plane of the first geometrical entity of the trajectory.
The setup will be maintained for the whole machining operation.

in the
plane of the first geometrical entity of the trajectory.
The setup will be recalculated in the same for each subsequent geometrical entity of the whole
machining operation.

3.5.6.3 Tilting routing mode

To define how the tilting routing is performed use

3.5.16
Approach/Retraction (shared by the machining operations)
The arc approach and retraction are disabled.

3.5.6.4 Tilting routing technology

See the following chapters:

3.5.15 Technological data (shared by the machining operations)

3.5.17 Advanced data (common to machining)
3.5.18 Machine data (shared by the machining operations)

139
3.5.7 Chamfering

To enter one or more chamfering proceed as follows:

-
- select one or more 2D elements

Or:
- select one or more 2D elements
-

The 2D elements selection can be single or multiple.

3.5.7.1 Chamfering position

The position of the chamfering is determined automatically by

the geometry selected.

3.5.7.2 Slotting shape

To define the slotting shape set:

The

The chamfer width quota measured on the plane selected.

The chamfer height (quota measured at right angles to the plane selected).

The chamfer angle is determined automatically after setting the width and height.

140
3.5.7.3 Chamfering mode

3.5.16
Approach/Retraction (shared by the machining operations)

3.5.7.4 Chamfering technology

See the following chapters:

3.5.15 Technological data (shared by the machining operations)

3.5.17 Advanced data (common to machining)
3.5.18 Machine data (shared by the machining operations)

141
3.5.8 3D routing

The geometry cannot be selected, but entered by points.

The tool inclination can be associated to each programmed point.

3.5.8.1 3D routing position

The 3D routing position is determined by all the points entered during the machining definition.
The tool correction is not available.

3.5.8.2 3D routing shape

The 3D routing shape can be a segment or a broken line of

various segments.
To define the 3D routing shape set the coordinates of the
various points of the broken line.

The tool will maintain the same setup for the whole machining
of the defined section.

To enter othe

To see the points entered use the right and left arrows to
navigate in the broken line.

To delete a point use "Z".

3.5.8.3 3D routing mode

3.5.8.4 3D routing technology

See the following chapters:

3.5.15 Technological data (shared by the machining operations)

3.5.17 Advanced data (common to machining)
3.5.18 Machine data (shared by the machining operations)

142
3.5.9 Scoring

The scoring is used to create a machining identical to the geometry in the project, even if it has
sharp edges.
To do this use only conical or trimming-conical tools.
Another limit is that it can only be applied to a closed geometry.
Another limit is that the maximum scoring depth will be equal to the
height of the conical part of the tool.

To enter a scoring use the "Scoring" command in the "Routing sub

menu.

3.5.9.1 Scoring position

The scoring position is determined implicitly by the position of

the geometry selected.

3.5.9.2 Scoring shape

The scoring shape is determined by the geometry selected and

by the value set in the "Offset" field that lets you create a
machining with a parallel geometry greater or smaller than the
original one.

3.5.9.3 Scoring execution mode.

The scoring processing can be divided in three parts:

- Internal trimming
- Corner Cleaning
- Pocketing

The internal trimming, selected with the "Profile only", performs

a machining inside the geometry selected at the maximum
depth equal to the one set.
If two sides of the geometry are very close the depth will be
reduced progressively to follow the shape of the geometry
being machined.
In other words the machining is performed with a dynamic
diameter correction.

By selecting the Pocketing option, all the area inside the

geometry selected will be machined with the depth set.
The "Only corner cleaning" option is used to machine the parts
remained filleted by a previous machining with a trimming-
conical tool.

143
Selecting this item will display the request for the smaller diameter of the trimming-conical tool
used in the previous machining.
The machining will clean only the parts that will were left filleted.

Using the "Complete machining" option will perform the internal profiling and pocketing phases
at the same time.

3.5.16
Approach/Retraction (shared by the machining operations)

3.5.9.4 Scoring technology

See the following chapters:

3.5.15 Technological data (shared by the machining operations)

3.5.17 Advanced data (common to machinings)
3.5.18 Machine data (shared by the machining operations)

144
3.5.10 Channel

The channel is a milling process with one limit and some added-values compared to the general
milling process.

The limit is due to the fact that the channel can be applied only for a line.
The added-values will be showed in the menu explanation.

In order to insert one or more channels, we can:

-
- select one or more 2D elements

Or:
- select one or more 2D elements
-
The selection of 2D elements can be single or multiple because the function "Channel" will
perform milling cutters associated with the lines.

3.5.10.1 Channel position

if there is any line among the selected elements, the channel

position is automatically set.

If no line has been selected, the position of a new line can be

set in this way:
- select the reference face
- fill the X field initial point
- fill the Y field initial point
- fill the X field final point
- fill the Y field final point

The real position of every milling is affected by the used tool

correction and the super-material.

In the tables in paragraph 3.5.5.1(milling position) it is

possible to understand how the different combinations of
options work.

145
We can also change the channel position by using the
in the sub-menu "Advanced data".
By using this function, the selected segment will be stretched
until it crosses the panel edges.

You can also have a channel extension if you activate the

3.5.10.2 Channel structure

In order to set the channel structure, Length and Depth

must be set in the menu.

The field Width is automatically filled when a tool is

connected with the channel.

In field "Depth" you will insert the value corresponding to the

thickness of the workpiece in case the option "Passer-
selected.

It si possible to set a "Final Depth (associated with the final

point of the geometry) different from the one associated with
the final point).
Enter the channel's inclination value, varying from 0° to
180° (not included) in the "Angle °" field. (90° =
perpendicular channel to face)

3.5.10.3 Channel execution mode

The channel execution mode looks like the milling mode

(see paragraph 3.5.5.3).

3.5.10.4 Channel technology

See the following chapters:

3.5.15 Technological data (shared by the machining operations)

3.5.17 Advanced data (common to machining)
3.5.18 Machine data (shared by the machining operations)

3.5.10.5 Channel deduced from surface

If a flat surface is selected, all the geometric parameters of the dialog boxes will be
automatically filled.
The user can modify the precompiled fields and must insert the blade to be used.

146
3.5.10.6 Channel wider than disc thickness

A channel with a width greater than the thickness of the disc can be created using the "Parallel
passes" pass generating strategy

Example:
1) A channel is created in any plane by defining all the dimensions

2) Select a blade tool:

3) The Parallel passes strategy is set,

unlocking the box to set the channel width:

4) The desired channel width can be set

147
5) Proceed to define the other processing parameters:
- By enabling Length correction in the Tool correction section, Maestro also
takes into account the size of the disk radius for the length of the channel.
- Cutting direction in the Parallel passes section''
o From left to right: the path starts from the left of the longitudinal symmetry
of the channel and moves to the right

o From right to left: the opposite direction

148
3.5.11 Blade cut

In order to insert one or more blade cuts you can:

-
- select one or more 2D elements

Or:
- select one or more 2D elements
-

The selection of 2D elements can be single or multiple because the option "Blade cut" will
performs cuts associated with the lines.

149