Roughing Parameters

Click Roughing then the geometric components to be machined.

A number of strategy parameters are available:

• in the Machining tab:

• the Machining mode,
• the Tool path style,
• Distinct style in pocket,
• the Machining tolerance,
• the Cutting mode,
• the Helical movement,
• the Always stay on bottom and Part contouring options,
• the Fully engaged tool management,
• 3/5-Axis Converter.

• in the Radial tab:

• the Stepover with the Max. distance between pass and the Tool diameter ratio.

• in the Axial tab:

• the Maximum cut depth.

• in the Zone tab:

• the Small pass filter,
• the Pocket filter,

• the Bottom tab:

• the Automatic horizontal areas detection with the offset on areas and the Maximum angle.
• the Same offset on bottom as on part.

• the High speed milling option,
• its Corner radius.

Specify the tool to be used (only end mill tools are available for this operation)
and speeds and rates .

You can also define transition paths in your machining operations by means of NC macros as needed.
These transition paths are useful to:

• optimize retract distances,
• set the Approach and Retract parameters.

Only the geometry is obligatory, all of the other requirements have a default value.

Roughing: Machining Strategy tab

The roughing strategy parameters are distributed into 6 tabs.
By default, all 6 tabs are displayed with all their parameters.
However, current operations only require a reduced list of those parameters.

Click <<Less to display only those current parameters.
The Zone and the Bottom tab are hidden, as well as the Variable cut depths button in the Axial tab.
Click More>> to re-display all parameters.

You can also use the modal option User Interface Simplified mode
in the Tools > Options > Machining > Operation tab.

By default, all tabs and all parameters are displayed:

Click <<Less to display a reduced list of tabs and parameters:

Roughing: Machining tab

All parameters remain displayed in the <<Less mode.

Machining mode

 Defines the type of area to be machined:

• By plane: the whole part is machined plane by plane, 
• By area: the whole part is machined area by area,

then

• Pockets only: only pockets on the part are machined,
• Outer part: only the outside of the part is machined,
• Outer part and pockets: the whole part is machined outer area by outer area
  and then pocket by pocket.

Please note that horizontal areas are always defined as pockets (no distinction outer part/pocket).
To mill them as Pockets only or Outer part areas, please use a limiting contour.
See also Definition of Pockets and Outer part.

Tool path style

Indicates the cutting mode of the operation:

• One-way next:
  the tool path always has the same direction during successive passes and
  goes diagonally from the end of one tool path to the beginning of the next.
• One-way same: the tool path always has the same direction during successive passes
  and returns to the first point in each pass before moving on to the first point in the next pass.
• Zig-zag: the tool path alternates directions during successive passes.
• Spiral: the tool moves in successive concentric passes from the boundary
  of the area to machine towards the interior.
  The tool moves from one pass to the next by stepping over.
• Contour only: only machines around the external contour of the part.
• Concentric: the tool removes the most constant amount of material possible at each concentric pass.
  The tool is never directly in the heart of material. It also respects the given cutting mode in all cases.
  The approach mode with this style is always Helix. 
• Helical: the tool moves in successive concentric passes from the boundary of the area to machine
  towards the interior. The tool moves from one pass to the next by stepping over.

  	The difference between Spiral and Helical style is most obvious when using high speed milling options. Helical has a rounded tool path in the corners of pockets whereas a  Spiral tool path will form loops. Spiral Helical
  	The cutting mode (Climb/Conventional) is respected on the contouring tool passes generated by the Helical tool path style. Machining mode: Inward Helical, Cutting mode: Climb

• By Offset on part with One-Way
  
• By Offset on part with Zig-zag
  

  With these two tool path styles, the part is machined by contouring passes, offset from the part, with high speed milling capability. This is useful for: progressive milling from stock to part, island machining in high speed milling, optimized contouring tool path. These styles are available for outer part areas only. Therefore, when the Machining mode is set to Outer part and pockets, the Distinct style in pocket option is automatically selected. The user Start point is not used as an imposed start point but is taken into account to define the path start point. Finish passes are done after rough passes, and finish passes on islands are done before those on sides. The Cutting mode is respected for: each pass in By Offset on part with One-Way mode, the last pass (side finish pass if it exists) in By Offset on part with Zig-zag mode. The option Always stay on bottom is not available for these styles.

Distinct style in pockets

Available only for the Machining mode Outer part and pockets.
When this option is selected, you can apply a different tool path style to pockets.

The icon icon is updated accordingly, for example:

Machining tolerance

Maximum allowed distance between the theoretical and computed tool path.
Consider the value to be the acceptable chord error.

Cutting mode

Specifies the position of the tool regarding the surface to be machined. It can be: 

Climb	or Conventional.

Helical movement

Specifies the way the tool moves in a pocket or an external zone. It can be:

• Inward: the tool starts from a point inside the zone and follows inward paths parallel to the boundary.

• Outward: the tool starts from a point inside the zone and follows outward paths parallel to the boundary.

• Both: 

For pockets, the tool starts from a point inside the pocket and follows outward paths parallel to the boundary.

For external zones, the tool starts from a point on the rough stock boundary and follows inward
paths parallel to the boundary.

In Helical mode, the control of the Non Cutting Diameter (Dnc) has been enhanced, in particular in the computation of the ramping approaches. This improvement may cause a computation failure, resulting in this specific message: The tool core diameter is not compatible with some ramping motions.

Always stay on bottom

This option becomes available when at least one tool path style is set to Helical.

When machining a multi-domain pocket using a helical tool path style,
this parameter forces the tool to remain in contact with the pocket bottom when moving from one
domain to another.
This avoids unnecessary linking transitions.

• Always stay on bottom is not selected:
• Always stay on bottom is selected:

Part contouring

Only used with the zig-zag and helical tool path styles. 

With Part contouring selected, the tool goes round the outside contour of the part before continuing
to zig-zag.
Clearing this check box allows you to gain machining time.
The tool that you are using and the part you are working on must be such that contouring the
rough stock is superfluous.

• With Part contouring selected. Note how the tool went round the area to machine first:

• With Part contouring cleared and exactly the same parameters.
  Note that the tool goes straight into zig-zag mode:

• each area is machined,
• then there is a contouring pass around each areas,
• followed by a contouring pass around the whole part when the remaining material is less than the tool radius,
• approach and retract motions are computed for all those tool paths.

Starting with R17, when Part Contouring is selected, all the tool paths around the part are chained, thus reducing the number of air cuts as there are fewer approach and retract motions.

Fully engaged tool management

This parameter is available when:

• the Machining mode is set to:
  • Pockets only
  • Outer part and pockets
• the Tool path style is set to:
  • Helical
  • Concentric
  • By Offset on part with Zig-Zag
  • By Offset on part with One-Way

It is used to manage full material cut in hard material roughing, where the stepover is not always respected and where the tool can be damaged. This can be avoided by switching to a trochoid motion that reduces the stepover, or by adding machining planes to reduce the load on the tool.

Full engagement is detected when:

• more that 75% of the tool diameter is engaged in the material,
• or more than 120 degrees of the tool is in contact with the material
• or if the actual radial stepover is more than 75% of the theoretical volume of material.
  

It can be set to:

• None: no management of the tool engagement.
• Trochoid: adds a trochoid motion in areas where the stepover is not respected. The trochoid motion is managed by the Minimum trochoid radius, given in percentage of the tool diameter:
  • the arrows show where full material milling is detected
    
  • the arrows show where full material milling is replaced by trochoidal motions
    
   

  The maximum diameter of the trochoid motion is equal to the radial stepover. If the minimum diameter of the trochoid motion is higher than the nominal radial stepover, or if the actual radial stepover is smaller than the nominal radial stepover, the trochoid motion will cover the bordering passes. In this case, it is possible that the bordering passes do not remove any material.

• MultiPass: adds machining planes in areas where the stepover is not respected. The distance between those additional planes is managed by the parameter Maximum full material cut depth.

  In previews and replays, a warning is displayed if Maximum full material cut depth is greater than the Maximum cut depth. The MultiPass mode may be de-activated on a given portion of the tool path when the curvilinear length of this portion is smaller than the radial stepover value. This de-activation avoids unnecessary approaches and retracts, when the radial plunge of the tool into the full material is not significant.

Roughing: Radial tab

All parameters remain displayed in the <<Less mode.

Stepover

It can be defined by:

• the Overlap ratio, i.e. the overlap between two passes,
  given as a percentage of the tool diameter
  (Tool diameter ratio),

• the Overlap length between two passes given by the Max. distance between pass,

• the Stepover ratio, i.e. the stepover between two passes,
  given as a percentage of the tool diameter
  (Tool diameter ratio),

• the Stepover length between two passes given by the Max. distance between pass,

See also Minimum thickness to machine

Roughing: Axial tab

By default, or when the More>> button is pressed:

When the <<Less button is pressed:
 

Axial strategy/Maximum cut depth

Depth of the cut effected by the tool at each pass

Variable cut depths

Hidden when the <<Less button is pressed.

When the dialog box opens the distance between passes from the top to
the bottom of the part is constant and is the same as Maximum cut depth.

Change the Distance from top value and the Max. cut depth value and
then press Add to give a different depth value over a given distance.

In the example below the cut depth: 

• from the top of the part to 15mm from the top is of 2 mm,

• from 15mm from the top to 25mm from the top is 5mm,

• and from 25 mm from the top to the bottom of the part is 10 mm.
  

Roughing: Zone parameters

This tab is hidden when the <<Less button is pressed.

Small pass filter 

Select this check box to activate the filter for small passes.
Then type the Tool section (%) value, which will be used to define the smallest area
to machine according to the tool used.
This information is given below the data field.

Pocket filter

Select this check box to activate the filter for small passes.
The non-cutting diameter of the tool can be entered in the Tool tab,
(click More). It is given as an information only in the Zone tab.

Not all pockets will be machined if there is not enough depth for the tool to plunge. A null value means that tool is allowed to plunge in pockets. The size of the smallest pocket is given below the data field. However, the smallest area to machine is taken into account only if the area detected has no impact on larger areas beneath. The Tool core diameter is taken into account: in pockets (default operating mode), also for outer parts when limiting contours are used. When areas are filtered (i.e. not machined) with the Tool core diameter, the areas beneath those areas are not machined.

Roughing: Bottom tab

This tab is hidden when the <<Less button is pressed.

Automatic horizontal areas detection

• When this check box is not selected, the only way to ensure that a cutting plane corresponds with
  an horizontal area is to define an imposed plane crossing the area.
  This means that you have to consider the offset on part.
  This plane applies to the whole part (which is not necessary).
  If there are several horizontal areas to consider at different levels you have to define all of
  the corresponding imposed planes.
  

• Select this check box to:

  • detect automatically horizontal areas on the part,

  • limit the cutting plane effect to these areas,

  • apply a dedicated offset on the part for these areas.
    

Then type the value of the offset to apply on the areas (Offset on areas).
The Maximum angle that can be considered as horizontal is displayed for information only.

• If the machining mode is By area, the tool path will look like this:
• If the machining mode is By plane, the tool path will look like this:

The cutting planes in green are the Standard roughing tool paths,
the red ones are those computed for the horizontal areas detected.

• The computation of horizontal areas is not possible if the part is made of a cloud of points (STL).
• This option is not compatible with the use of offset groups.
• Horizontal areas are always defined as pockets (no distinction outer part/pocket).
  To mill Pockets only or Outer part areas, please use a limiting contour.
• When only Outer part areas are to be machined, no specific tool path style is given for the pockets. As a consequence, if the tool path style used for the Outer part areas is not compatible with pockets (e.g. By Offset on part with One-Way), horizontal areas are machined with a default tool path style (Concentric).

Roughing:High Speed Milling tab

All parameters remain displayed in the <<Less mode.

Select the check box High speed milling to activate and define the parameters for High speed milling. 

Corner radius

Applies to Concentric, Helical, By Offset on part with One-Way and By Offset on part with Zig-Zag tool path styles.

Defines the radius of the rounded ends of passes when cutting with a Concentric tool path style
and the radius of the rounded end of retracts with Helical and Concentric tool path styles. 
The ends are rounded to give a smoother path that is machined much faster.

• This is what a tool path will look like if you do not use high speed milling parameters:

• Here is the same tool path with the High speed milling check box selected. Note how the round tool path ends.
  In both cases a  Concentric tool path style is used.

• Similarly, here is what retracts look like without the high speed milling option:
• And here is the same tool path with high speed milling switched on:

  With HSM and helical mode, the corner radius must be less than half the stepover distance. It will be forced to this value. The corner radius is no longer applied to the finish path. With the Spiral mode, the tool path is cornered only when the value of the parameter Max. distance between pass  is higher than the radius of the flat tool tip + 10%. The HSM loops are generated only when the flat tool tip does not cover the previous tool path in the corners.

Corner radius on part contouring

When available and active, defines the corner radius of all the tool paths in contact with the part.

Roughing: Geometry

You can also specify the following geometry:

• Part with possible offset.
• Rough stock. If you do not have a rough stock you can create one automatically.
  You must define a rough stock if you have not already defined one in the Part Operation.
  See the Machining Infrastructure user's guide for further information.
• Check element with possible offset.
  The check element is often a clamp that holds the part and therefore is not an area to be machined.
• Area to avoid if you do not wish to machine it (the small light brown corner near the part selection area).

• Safety plane. The safety plane is the plane that the tool will rise to at the end of the tool path in
  order to avoid collisions with the part.
  You can also define a new safety plane with the Offset option in the safety plane contextual menu.
  The new plane will be offset from the original by the distance that you enter in the dialog box
  along the normal to the safety plane.
  If the safety plane normal and the tool axis have opposed directions, the direction of the safety plane normal
  is inverted to ensure that the safety plane is not inside the part to machine.

• Top plane which defines the highest plane that will be machined on the part,
• Bottom plane which defines the lowest plane that will be machined on the part,
• Imposed plane that the tool must obligatorily pass through.
  Use this option if the part that you are going to machine has a particular shape
  (a groove or a step) that you want to be sure will be cut.

  If you wish to use all of the planar surfaces in a part as imposed surfaces, select Search/View ... in the contextual menu to select them.  When searching for planar surfaces, you can choose to find either:  all of the planar surfaces in the part, or only the planes that can be reached by the tool you are using.  Here is an example with the gets2.CATPart. To use planar surfaces of a part as imposed planes: Select the planar surfaces, Select Offset in the contextual menu and enter a value equal to the machining tolerance + the offset value on part (if any): If the machining tolerance is 0.1 mm, and there is no offset on part, you will enter 0.1 mm as offset for the imposed plane. If the machining tolerance is 0.1 mm, and the offset on part is 1 mm, you will enter 1.1 mm as offset for the imposed plane. This ensures that the imposed planar surface is respected  to within the offset and tolerance values.

• Start point where the tool will start cutting. There are specific conditions for start points:

  Start points only concern external contours but not contouring passes. They must be outside the machining limit. Examples of machining limits are the rough stock contour; a limit line, an offset on the rough stock, an offset on the limit line, etc. They must not be positioned so as to cause collisions with either the part or the check element. If a start point for a given zone causes a collision, the tool will automatically adopt ramping approach mode. The distance between the start point and the machining limit must be greater than the tool radius plus the machining tolerance. If the distance between the start point and the machining limit is greater than the tool radius plus the safety distance, the start point will only serve to define the engagement direction.  If there are several start points for a given area, the one that is used is the first valid one (in the order in which they were selected) for that area. If there are several possible valid points, the nearest one is taken into account. One start point may be valid and for more than one area. If a limit line is used, the tool will approach outer areas of the part and pockets in ramping mode, towards the outside of the contour. The tool moves from the outside towards the inside of this type of area. In this case, you must define the start point.
  	If you use a limit line or if you use an inner offset on the rough stock, the start point may be defined inside the initial rough stock. The rules concerning the domain of the contour line or the offset on the rough stock contour line above must be applied.
  	Concentric tool path style: Start points are automatically defined. In this case, the start point is the center of the largest circle that can be described in the area to machine. Lateral approach modes cannot be used. Spiral and Helical Tool path styles: Whenever possible, the end of the engagement associated to the start point corresponds to the beginning of the sweeping path. If this is no possible, the path will be cut to respect the constraint imposed by the start point.

• Inner points (only active if the Drilling mode has been selected in the Macro data tab).
  There are specific conditions for inner points:

  They are usable for pockets only, They must not be positioned so as to cause collisions with either the part or the check element. If an inner point for a given pocket causes a collision, the tool will adopt a new inner point generated automatically. The inner point must lay inside the pocket and inside the portion of the pocket that is machined. When you look at the part from the tool axis direction, the inner point must lay inside each pocket tool end contour for every cutting plane. If there are several inner points for a given pocket, the one that is used is the first valid one (in the order in which they were selected) for that pocket. A point can not be valid for several pockets.

• Limiting contour which defines the machining limit on the part, with the Side to machine parameter.

 Please refer to the Selecting Geometric Components to learn how to select the geometry.

Appears when invalid faces have been detected.
This message disappears when you close the dialog box or when the next computation is successful.

Appears when invalid faces have been detected and when you have decided to ignore them.
This message remains displayed as a warning.

Pick the text to switch from one status to the other.

Roughing: Tool/Rough Stock parameters

Position 

Defines where the tool center stops:

• Outside stops the tool outside the rough stock.
  The toolpath is computed as if the rough stock is increased by a value equal to 50% of the tool diameter in each cutting plane,
• Inside stops the tool inside the rough stock.
  The toolpath is computed as if the rough stock is reduced by a value equal to 50% of the tool diameter in each cutting plane,
• On stops the tool on the rough stock.
  This is the default (recommended) option.

Offset 

Defines the distance that the tool can overshoot the Position.
It is expressed as a percentage of the tool diameter.
This parameter is useful in cases where there is an island near the edge of the part and the tool diameter
is too wide to allow the area behind the island to be machined. 
This parameter can only be used if the Position is inside or outside.

Minimum thickness to machine

Specifies the minimum material thickness that will be removed  when using overshoot or in a rework operation.

• The red arrow points to the Minimum thickness to machine,
  the green arrows point to the material that is not removed,
  the black arrow points to the material removed,
  the grey arrow points to the part to machine.
  
• In red, the Minimum thickness to machine,
  in green, the material that is not removed,
  in black, the material removed,
  in grey, the part to machine.
  

In a given level, the thickness of material left can amount up to the value of the Minimum thickness to machine + twice the value of the tolerance. Therefore, on a level below you may have to mill a thickness amounting to the value of the  Minimum thickness to machine + twice the value of the tolerance of one or several levels above. Minimum thickness to machine leads to select areas to be machined depending on a specific thickness value. However, in a roughing operation collisions with stock must be controlled and passes are added to avoid any over height situation. Over height situations are detected with a straight tool, as shown in the picture below:

Defines what area of the part will be machined with respect to the limiting contour(s).
It can either be inside or outside. In the pictures below, there are three limiting contours on the rough stock.
The yellow areas will be machined.

Side to machine: Inside

Side to machine: Outside

• If you are using a limiting contour, you should define the start point so as to avoid tool-material collision.
• The use of limiting contours is totally safe is the limiting contour is fully contained by the roughing rough stock.
  Example of use: restricting the machining to a group of pockets.
• But we strongly advise against using a limiting contour that is partly outside the roughing or
  residual rough stock.
  Example: roughing rework or a first roughing with a complex rough stock).
  In that case, we recommend that you define a surface with holes or a mask to define the
  machining zone to work on.

Stop position

Offset

Specifies the distance that the tool will be either inside or outside the limit line depending on the stop mode
that you chose.

Force replay button is only used for reworking operations. 

Its purpose is to compute the residual rough stock remaining from operations preceding the current one,
providing a rough stock has not been defined for this operation. Use it before clicking Tool Path Replay .

Roughing: Feeds and Speeds

In the Feeds and Speeds tab page, you can specify feedrates for approach,
retract, machining and finishing as well as a machining spindle speed.

Feedrates and spindle speed can be defined in linear or angular units.

A Spindle output checkbox is available for managing output of the SPINDL instruction in the generated NC data file.
If the checkbox is selected, the instruction is generated. Otherwise, it is not generated. 

Feeds and speeds of the operation can be updated automatically according to tooling data and the Rough or
Finish quality of the operation. This is described in Update of Feeds and Speeds on Machining Operation.

Feedrate management is possible for Helical, By Offset on part with One-Way and By Offset on part with Zig-Zag
tool path styles only.

Feedrate Reduction in Corners

You can reduce feedrates in corners encountered along the tool path depending on values given in
the Feeds and Speeds tab page: reduction rate, maximum radius, minimum angle,
and distances before and after the corner.

Feed reduction is applied to corners along the tool path whose radius is less than the
Maximum radius value and whose arc angle is greater than the Minimum angle value.

When machining pockets, feedrate reduction applies to inside and outside corners for
machining or finishing passes. It does not apply for macros or default linking and return motions.

Corners can be angled or rounded, and may include extra segments for HSM operations. 
1=Machining feedrate or Finishing feedrate
2=Reduced feedrate
A=Distance after corner
B=Distance before corner

Slowdown Rate

You can use Slowdown rate in the Feeds and Speeds tab page to reduce the current feedrate
by a given percentage. 

In Helical tool paths, the reduction is applied to the first channel cut.

Combining Slowdown Rate and Feedrate Reduction in Corners

If a corner is included in a Slowdown path, the general rule is that the lowest percentage value
is taken into account.

For example, if the Slowdown rate is set to 70 % and Feedrate reduction rate in corners is set to 50%,
the feedrate sequence is: 
100%,
70% (entry in slowdown),
50% (entry in corner),
70% (end of corner, still in slowdown),
100% (end of slowdown).

If Feedrate reduction rate in corners is then set to 75%, the feedrate sequence is: 
100%,
70% (entry in slowdown),
70% (entry in corner: 75% ignored),
70% (end of corner, still in slowdown),
100% (end of slowdown).

Roughing: Macro data

For more information on how to save or load an existing macro,
please refer to Build and use a macros catalog.

Optimize retract

This button optimizes tool retract movements.
This means that when the tool moves over a surface where there are no obstructions,
it will not rise as high as the safety plane because there is no danger of tool-part collisions.
The result is a gain in time.

• The parameter Optimize retract takes the rough stock left by the previous operation into account.
• If you have defined a safety plane, you should deactivate the Optimize retract option.
  If you do not, the safety plane will be ignored.

Axial safety distance

Maximum distance that the tool will rise to when moving from the end of one pass to the beginning of the next.

Mode

Specifies the engagement of the tool in the material:

• Plunge; the tool plunges vertically,
• Drilling; the tool plunges into previously drilled holes. You can change the Drilling tool diameter,
  Drilling tool angle and Drilling tool length,

  Helix retracts are inserted into the toolpath when using Helical mode (only when retracts begin on the part). But when a Drilling macro is selected, not all Helix retracts are inserted.

• Ramping; the tool moves progressively down at the Ramping angle,
• Helix; the tool moves progressively down at the ramping angle with its center along a (vertical)
  circular helix of Helix diameter.

Those four approach modes apply to pockets.

• If the tool Path is Concentric, the approach is always Helix, either on outer areas or pockets.
• Ramping approach mode applies to pockets but also outer areas in given conditions: 

  If a limit line is used, the tool will approach outer areas of the part and pockets in ramping mode. If a lateral approach is not possible (due to the check element), the approach is made in ramping mode.

Approach distance

Engagement distance for plunge mode.

Radial safety distance

Distance that the tool moves horizontally before it begins its approach.