Check below the specifications and configurations available in the Rover 22 plugin:
Available from version: Plugin Builder 1.60.16.18
Machine Type:CNC Machining Center
Manufacturer:Biesse
Generated file extension:.bpp , .Cid and .Cix
Manual: manual available for the manufacturer, click here.
Main features
- Holes
- Slot
- Machining
- Profile machining
- External machining
- Automatic tool change
Settings
To check the settings on CNC Machines, click here.
Machine 1
General
Name: define the name for the machine.
IMPORTANT: The name set in this field also changes the name of the folder where the generated files will be saved.
Length X (mm): the value entered in this field indicates the maximum usable length of the machine.
Width Y (mm): the value entered in this field indicates the maximum usable width of the machine.
IMPORTANT: From version 1.60.18.2 of Plugin Builder, the PAN format for file generation has been added.
Others
Program format: When the PAN format is selected, the NC500 tool definition file name option is enabled.
Integration System
Inform the name of the NC500 tool definition file: must be informed the corresponding name that is already in use on the machine.
NOTE: When selecting the PAN format, it is important to remember that it will not be possible to perform profile machining, as well as machining on the profile face.
Tools
To check the settings about CNC Tools, click here.
Mills
The mills are used to perform slotting and machining.
Contour Machining
Contour machining start: defines where contour machining starts, at one of the corners or in the middle of one of the workpiece edges. This option is applicable only to external contour machining.
External contour cut direction: defines whether contour machining has to be done clockwise or counterclockwise.
Internal Milling
Internal contour machining start: it defines internal machining to be made in a non-clockwise or anti-clockwise direction.
Internal milling cut direction: defines where internal contour machining starts, at one of the corners or in the middle of a machining edge.
Use cutting direction in single line operations: when you mark this setting, single-line machining operations follow the cutting direction of the mills.
For more information click here.
Lead in
Input type in linear machining: defines the type of input the tool will use when machining and contouring linear forms. Options Ramp, vertical, circular.
- Circular: in this type the tool descends outside the part and then starts cutting tangentially before entering the part.
- Vertical: in this type the tool descends vertically onto the workpiece and begins cutting.
- Ramp: in this type the tool descends by making a ramp until it reaches the maximum depth of operation.
Lead in extension (mm): extension of the entrance before the contour cutting starts, equivalent to the red line in the image.
Lead in/ Lead out
Tool descent angle (A): the angle of descent of the tool defined by dimension A.
Step height during machining (B): this option is only available when the Linear Machining Input Type selected is Ramp. It defines the step height during machining.
Step lenght during machining (C): step length during machining.
Distance between lead in and lead out (mm): distance the tool exits and enters the part. It is advisable that this value be greater than zero so that the cut does not leave any fragments (burrs).
Lead Out
Lead Out extension (mm): output extension after machining/contouring is finished, equivalent to the red line.
Lead Out Type: defines the type of output that the tool will use when machining and contouring.
- In the vertical type, the tool descends vertically onto the workpiece and begins cutting.
- In the circular type, the tool descends outside the part and then starts cutting tangentially before entering the part.
- In the ramp type, the tool descends as a ramp and starts cutting.
Properties
Code: the code defined in this field must match the registration defined on the machine so that the tool can be located correctly.
Diameter (mm): tool diameter.
Name: the name defined in this field must match the registration defined on the machine so that the tool can be located correctly.
Overlap (mm): overpass between tool passes to avoid material leftovers.
Step depth (mm): depth of tool step.
Through plunge and milling offset (mm): compensation of the drilling and machining of the part.
Slots
Cutting direction for milled slot: defines whether the cut must be clockwise or counterclockwise.
Tool Alignment
Milling alignment: defines whether the tool has an offset in the center, left or right according to the direction of the Cutting direction option for contour machining.
Conical Mills
Contour Machining
External contour cut direction: it defines the machining of contours to be made in a non-clockwise or anti-clockwise direction.
Internal Milling
Internal contour machining start: defines where the internal contour machining starts, at one of the corners or in the middle of one of the machining edges.
Internal milling cut direction: it defines the machining of contours to be made in a non-clockwise or anti-clockwise direction.
Properties
Code: the code defined in this field must be the same as the one defined on the machine so that the tool can be located correctly.
Cutting Angle: tool cutting angle.
Diameter (mm): tool diameter.
IMPORTANT: in the image below, in blue it represents the tool zero point.
Height (mm): tool height.
Horizontal step depth (mm): depth value per horizontal pass of the tool, depending on this value and the depth registered on the part, the number of times the tool will pass on the part until reaching the desired depth in the horizontal is defined.
Machining Compensation: drilling compensation and through machining. For more information click here.
Name: the name defined in this field must match the registration defined on the machine so that the tool can be located correctly.
Vertical step depth (mm): value of the depth per vertical tool stroke, depending on this value and the depth entered on the workpiece, the number of times the tool will pass on the workpiece until it reaches the desired vertical depth is defined.
IMPORTANT: To maintain compatibility and standard operation, the value for Depth of vertical pass uses the same value as the tool height.
Saws
Saws are used to make slot.
Properties
Alignment: alignment of the saw, center, left or right.
Code: the code defined in this field must match the registration defined on the machine so that the tool can be located correctly.
Diameter (mm): tool diameter.
In offset (mm): transfer between the passes of the hardware to avoid leftover material.
Invert direction: uncheck the option to have the cut start at the measurement closest to the machine zero point. Check the option to have the cut start at the measurement opposite the machine zero point.
Name: the name defined in this field must match the registration defined on the machine so that the tool can be located correctly.
Orientation: tool orientation, vertical or horizontal.
Out offset (mm): saw output compensation for performing the cut, in millimeters. This setting is only applied if the slot ends outside or on the endpoint of the part.
Overlap (mm): input compensation of the saw to perform the cut, in millimeters. This setting is only applied if the slot starts outside or on the starting point of the part.
Thickness (mm): thickness of the saw.
Set Ups
General
Name: the name set in this field also changes the name of the folder where the generated files will be saved.
Alignment by face: defines whether the alignment face registered on each part is considered when generating programs. If yes, this face will be aligned according to the selected configuration. For more information click here.
Perform drilling: machine is enabled to drill holes.
Make slots: with the option checked the registered slot will be generated in the machine programs.
Perform machining: with the option checked the registered machining operations will be generated in the machine programs.
Perform profile machining: with the option checked, the registered profile machining will be generated in the machine programs. For more information click here.
Machining processes: through Plugin Builder, it is possible to create and determine types of processes for machining registered in the library, thus enabling the use of a particular tool for a particular machining. For more information click here.
Perform machined contour: defines the contour of which parts will be generated.
- None: contour machining will not be generated for any part;
- All: contour machining will be generated for all parts;
- Only marked: contour machining will be generated only for parts that have the Machined Contour property enabled in the library register.
Simmetry: execute symmetrical holes simultaneously.
Version: version of the generated program. It must be compatible with the software that will open the files generated by the plugin.
Machine
Priorization order: defines the order of prioritization of operations for program generation. According to the order indicated in this field the plugin will prioritize in program A the selected option.
Example: In a part that has holes on one side and tears on the other side, the order indicated in this field will determine which of them will be prioritized in the A program.
Slot tool: tool used for slots. IMPORTANT: This option is available when the Make Slots option is selected.
Machining tool: tool used for machining. IMPORTANT: This option is only available when the option Machine Process is selected.
Operations ordering: order that the machine performs operations.
Example: in a part that has holes and tears on the same face the order indicated in this field will determine the sequence in which they will be executed by the machine.
Profile Machining Tool: this option will only be available when the Perform profile machining option is checked. More information click here.
Holes
Drill bits for blind hole operation: option for normal drilling. Normal drilling is considered normal when it is not through or marking drilling.
Minimium diameter to use Forstnet Bit (mm) | normal drill (mm): this option will only be available when Normal Drill is chosen in the Normal Drill option. Drillings with a diameter smaller than the one registered will use a normal drill. Drillings with diameter greater than or equal to the registered diameter will use a large normal drill.
Drill Bits for through hole operations: type of drill for through hole drilling - Normal Drill, Spear or Reaming Drill.
Drill bit for marking hole operation: type of drill bit for marking drilling – Normal Drill, Lance or Reamer
Depth of marking hole operation (mm): maximum depth to be a marking hole. When the hole is smaller or equal it will automatically be considered a marking hole.
Drill bit angle used in through holes: determine the drill bit end angle for through hole usage (from 25 to 90 degrees). This value is used in the calculation to determine the increment in the through-hole depth to ensure that the hole passes completely through the part.
Drill GAP in through hole operation (mm): determine the clearance of the drill for use in through holes.
Drill Bits Type: defines the codes used for each drill type. The codes are defined in the fields, reamer drill type, lance drill type, normal drill type, and large normal drill type.
Maximum diameter of horizontal drill bit (mm): maximum diameter of horizontal drills.
Maximium diameter of vertical drill bit (mm): maximum diameter of vertical drills.
Maximium horizontal drilling depth (mm): maximum depth the drill bit can drill horizontally.
Maximium position of lateral drilling in (Y): maximum position where the machine can drill lateral holes in (Y).
Maximium position of vertical drilling in (Y): maximum position at which the machine can drill vertical holes in (Y).
Maximium vertical drilling depth (mm): maximum depth that the drill can drill vertically.
Minimium diameter of Drill bit (mm): minimum drilling diameter.
Number of horizontal drill bits (X): the number of drills, for each horizontal face, present in the machine.
Number of lateral drill bits (Y): number of drill bits, for each side face, present in the machine.
Number of vertical drill bits (Z): number of vertical drills present in the machine.
Machinings:
Inverted pass: Reverse pass used in edge-out operations.
- None: The cutter will follow the normal machining path entering one edge and exiting the other.
- One pass: The cutter will enter one edge of the part making only a small entry. Then the cutter will climb, go to the other end of the machining, and then follow the normal machining path.
- Double pass: The cutter will enter one edge of the part making only a small entry and return to the starting point. Then the cutter will climb, go to the other end of the machining, and then follow the normal machining path.
Slots
Maximium position for sawed slots in (Y): maximum position at which the machine can make (Y) saw cuts.
Technical specifications
Minimum Length(X): minimum length of the workpiece for the machine to perform operations.
Technical Data
Maximum thickness(Z): maximum thickness of the part that the machine can perform operations.
Minimum length (X): minimum thickness of the part that the machine can perform operations.
Minimum thickness (Z): minimum thickness of the part that the machine can perform operations.
Minimum width (Y): minimum part length for the machine to perform operations.