Check below the specifications and configurations available in the Tech 99L plugin:
Available from version: Plugin Builder 1.60.17.4
Machine Type: CNC Machining Center
Manufacturer: Morbidelli | SCM
Generated file extension: .Prg
Manual: for more information, contact the manufacturer.
Main features
- Holes
- Slot
- Machining
Settings
To check the settings on CNC Machines, click here.
Máquina 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
Integration System
Integration System: defines for which integration system Genio programs will be generated. Maestro or maestro with label.
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.
Feed rate (mm/min): speed at which the tool performs the cut.
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.
Working faces: faces on which the tool will be used to perform operations.
Tool Alignment
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.
Saws
The saws are used for the execution of slots.
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.
Feed rate (mm/min): speed at which the tool performs the cut.
In offset (mm): transfer between the passes of the hardware to avoid leftover material.
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.
Rotation speed (rpm): tool rotation speed in RPM.
Thickness (mm): thickness of the saw.
Working faces: faces on which the tool will be used to perform operations.
Restrictions
Maximum thickness of the saw: maximum saw blade thickness in millimeters.
Minimum thickness of the saw: minimum saw blade thickness in millimeters.
Setups
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 clickhere.
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.
Variable usage field distance, in the X axis: distance from the end of the part on the X axis, which determines the area (blue area on the image) where operations should take variable part size minus the distance from the operation under consideration to the end.
Variable usage field distance, in the Y axis: distance from the end of the part on the Y axis, which determines the area (red area on the image) where operations should take variable part size minus the distance from the operation under consideration to the end.
Invert variable fields: by checking this option, when a rotated part is generated, the fields invert as shown in the picture.
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.
Slot process: through the Plugin Builder, it is possible to create and determine types of processes for tears registered in the library, thus making it possible to use a certain tool for a certain tear. For more information click here.
Overcut
Sum edge band overcut: when this option is unchecked, the border thickness is subtracted from the final part size. Uncheck this option if you don't want to use the router. When this option is checked, the edge thickness is subtracted and the edge overcut added to the final part size. Check this option if you want to use the router.
Sum plate overcut: adds the sheet overcut to the final size of the part.
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.
Contour tool: tool used to make contours.
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.
File .inf
Detail all programs operations: detail operations not performed in the .inf file in all programs (A,B,C....).
Generate empty parts info: generate .inf file of parts without operations.
Holes
Drill bits for blind hole operation: option for normal drilling. Normal drilling is considered normal when it is not through or marking drilling.
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 drilling depth (mm): maximum depth the drill bit can drill.
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.
Machining
Execute multipass millings into a single milling command: enables multi-pass command in a single command.
Slots
Maximum slot depth: maximum depth of the slot (groove) in millimeters.
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.