Check the specifications and configurations available in the Cyflex S e SR - CX100 plugin below:
Available from version: Plugin Builder 1.60.17.5
Machine type: CNC Machining
Manufacturer: Morbidelli
Generated file extension: pgmx e .xcs
Main Features
- Drilling
- Canals
- Machining
Setup
General
Name: define the name for the machine.
IMPORTANT: the name defined in this field also changes the name of the folder where the generated files will be saved.
Length X (mm): length of the machine.
Width Y (mm): width of the machine.
Program extension: extension of the generated program (pgmx or xcs).
Apply suction command: enable suction command.
T value for defined default working area: T command in the header for individual area job fields.
IMPORTANT: Starting from version 1.60.18.2 of the Plugin Builder, the PAN format has been added for file generation.
Others
Clamp size, in millimeters: collet size in millimeters.
Model: machine model.
Integration System
Change the file path for Xilog Maestro tools: this option defines the configuration file path for tools. Accepts only *.tlgz files from Maestro.
Change the path for Xilog Maestro: this option defines the Xilog Maestro path.
Xcs to pgmx convertion limit: the amount of programs that can be converted at a time from xcs to pgmx.
Tools
To check the settings about CNC Tools, click here.
Mills
The mills are used to perform slotting and machining.
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.
Use cutting direction in single-line operations: when selecting this configuration, single-line machining will start to follow the cutting direction of the cutter.
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.
Ramp lead in extension (mm): input extension used to calculate the ramp input of the tool, equivalent to the red line in the image.
Lead in/ Lead out
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.
Ramp lead out extension (mm): extension of the outlet after machining/contouring is complete, equivalent to the red line in the image.
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.
Height (mm): tool height, in millimeters.
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.
Suction hood position: this value ranges from 0 (no hood positioning) to the value corresponding to the lowest hood position.
Through plunge and milling offset (mm): compensation of the drilling and machining of the part.
Tool Alignment
Milling alignment: defines if the tool has an offset, Automatic, Center, Left or Right according to the direction of the Cut direction option for contour machining. For more information click here.
Saws
Saws are used to make slot.
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.
Input compensation (mm): saw input compensation to perform the cut, in millimeters. This configuration is only applied if the tear starts outside or on the starting point of the part.
Name: the name defined in this field must match the registration defined on the machine so that the tool can be located correctly.
Output compensation (mm): output compensation of the saw to execute the cut, in millimeters. This configuration is only applied if the tear ends outside or on the end point 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.
Suction hood position: this value ranges from 0 (no hood positioning) to the value corresponding to the lowest hood position.
Thickness (mm): thickness of the saw.
Restrictions
Maximum saw thickness: maximum saw thickness.
Minimum saw thickness: minimum saw thickness.
Setups
General
Name: the name set in this field also changes the name of the folder where the generated files will be saved.
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.
Align 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.
Execution area: Program Execution Area.
Unloading of the workpiece: Defines where the workpiece will be unloaded after the processes.
Clamp can be disabled: With this option selected, the clamp can be disabled according to the groove restrictions or if the workpiece has any type of contour. If the option is not selected, the clamp will always be enabled.
Machining processes: By clicking the Machining Processes button, a new window with the registered processes will be opened.
There are three configuration options:
Enabled with Machining Tool: Operations linked to this process will be executed using the tool selected in the Machining Tool option;
Enabled with Process Machining Tool: Operations linked to this process will be executed using the tool selected in the Process Machining Tool option;
Disabled: Operations linked to this process will not be executed, generating a .inf extension file indicating that such operation will not be executed because its process is configured as disabled.
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.
Rotations
Evaluate minimum width for rotation: defines whether, in the generation of programs, the minimum dimension of the piece will be evaluated to be rotated in the width direction. If yes, pieces with a face dimension smaller than the defined one will be rotated, and these will have this face aligned with the width axis of the machine.
Minimum length allowed for rotations (mm): defines the minimum allowed length for rotations, in millimeters. If the length of the piece is less than the defined value, the largest dimension of the piece will be placed in X.
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 Machining option 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.
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.
Technical Specifications
Minimum Length (X): minimum length of the piece for the machine to perform operations.
Maximum Thickness (Z): maximum thickness of the piece for the machine to perform operations.
Minimum Thickness (Z): minimum thickness of the piece for the machine to perform operations.
Minimum Width (Y): minimum width of the piece for the machine to perform 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.
Maximium diameter of horizontal drill bit (mm): maximum diameter of horizontal drills.
Maximium diameter of vertical drill bit (mm) :maximum diameter of vertical drills.
Minimum diameter of drill bit (mm): minimum drill 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.
Drill Type: defines the codes used for each type of drill. The codes are defined in the fields, countersink drill type, lance drill type and normal drill type.
Minimum position of the center of side holes in (Y): Minimum position of the center of side holes on the Y-axis where the side drills can operate, in millimeters.
Minimum position of the quadrant of horizontal holes in (Y): Minimum position of the quadrant of horizontal holes on (Y) that the machine can operate, in millimeters. To calculate the quadrant's position, the hole's center at (Y) - the hole's radius is considered. The quadrant cannot exceed the minimum position defined in this property, with reference to the start of the piece.
Minimum position of the quadrant of side holes in (X): Minimum position of the quadrant of horizontal holes on (X) that the machine can operate, in millimeters. To calculate the quadrant's position, the hole's center at (Y) - the hole's radius is considered. The quadrant cannot exceed the minimum position defined in this property, with reference to the start of the piece.
Minimum position of the lower quadrant of vertical holes (Qmin) on the Y-axis: The lower quadrant of the hole must be at the Qmin position from the bottom edge of the piece, with dY being the height of the piece. To calculate the quadrant's position, the hole's center at (Y) - the hole's radius is considered.
Maximum depth of horizontal drilling (mm): Maximum depth the drill can drill horizontally, in millimeters.
Maximum depth of vertical drilling (mm): Maximum depth the drill can drill vertically, in millimeters.
Grooves with Milling Cutter
Minimum Position in Y: Minimum position in Y, in relation to the center of the milling cutter. The position of the suction hood will be considered.
Grooves with Saw
Minimum groove position in (Y) considering the center of the saw: Minimum position in Y, in relation to the center of the milling cutter.
Maximum depth of the saw: Maximum depth the saw can operate.
Clamp Restrictions
Minimum thickness of the groove remnant (mm): Minimum thickness of the groove remnant, in millimeters.
Minimum upper position of the groove (mm): Minimum upper position of the groove, in millimeters.
Machining with Support Bridges
Length of the bridges (CP): Length of the support bridges in machining, in millimeters.
Distance between bridges (DP): Machined distance between the bridges, in millimeters.
Thickness of the bridges (EP): Thickness machined between the bridges, in millimeters. If this value is greater than the thickness of the piece, the value sent to the program will be the thickness of the piece. If this value is zero, the bridges will not be executed.
Machinings
Reverse Pass: Reverse pass used in exit operations on the side with an edge.
Machining Type: Defines the behavior of pass-through machinings. Standard follows the operation's registration:
- Force emptying: removes all material;
- Force contour: performs only the contour of the operation.