Check below the specifications and configurations available in the Weeke ABL 210 B plugin:
Available from version: Plugin Builder 1.60.17.4 or superior
Machine Type: CNC Machining Center
Manufacturer: Weeke
Generated file extension: .mpr
Manual: manual available for the manufacturer, click here e here.
Main features
Machining centers meet all demands for parts and operations such as milling, drilling, reaming and threading.
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.
Several
Program format: the format defined in this field will define the extension of the generated file: .bpp , .Cid or .Cix.
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.
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.
Step depth (mm): depth of tool step.
Overlap (mm): overpass between tool passes to avoid material leftovers.
Step depth(mm): the speed at which the tool moves forward through the workpiece. The default value is STANDARD.
Rotational speed: rotational speed of the tool. The default value is STANDARD.
Through plunge and milling offset (mm): compensation of the drilling and machining of the part.
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. For more information, click here.
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 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.
Distance from variable usage field on 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.
Distance from the variable use field on 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.
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.
Rotations
Evaluate minimum width for rotation: defines if in the generation of the programs the minimum dimension of the part to be rotated in the length direction will be evaluated. If yes, parts that have a face with a dimension smaller than the one defined will be rotated, they will have this face aligned to the machine width axis.
Minimium length allowed for rotations (mm): defines the minimum length allowed for rotations, in millimeters. If the part's length is shorter than defined, the largest part dimension will be set to X. (displayed value is 400)
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.
Process machining tool: machining tool, where we can select milling.
File .inf
Generate empty parts info: generate part .inf file without operation. (is selected as True by default).
Holes
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.
Maximum diameter of horizontal drill bit(mm): maximum diameter of the horizontal drills.
Maximum diameter of vertical drill bit (mm): maximum diameter of the vertical drills, in millimeters. Maximum value: 35.
Maximum horizontal diameter (mm): maximum diameter of the horizontal drills, in millimeters. Maximum value: 12.
Maximum side diameter of the tools(mm): maximum diameter of the side drills in millimeters. Maximum value: 14.
Maximium position of the center of the horizontal holes opposite axis Y: maximum center position of the horizontal holes opposite the Y-axis. Value: 9.5.
Maximium vertical drilling depth (mm): maximum depth that the drill can drill vertically.
Minimium depth of horizontal drilling (mm): minimum depth that the drill can drill horizontally. IMPORTANT: As of version 1.60.17.5, the Minimum Diameter field has been removed and replaced by the Minimum Horizontal Drill Depth (mm) field.
Minimium depth of vertical drilling (mm): minimum depth that the drill can drill vertically. IMPORTANT: As of version 1.60.17.5, the Minimum Diameter field has been removed and replaced by the Minimum Vertical Drill Depth field (mm).
Minimum horizontal diameter(mm): minimum diameter of the horizontal drills. IMPORTANT: as of version 1.60.17.5, the Minimum Diameter field has been removed and replaced by the Minimum Horizontal Diameter (mm) fields.
Minimium position from the center of lateral hole in (Y): minimum center position of the horizontal holes opposite the Y-axis. Value: 6.
Minimium position of the lower quadrant of the vertical holes (Qmin): the bottom quadrant of the hole must be in position Qmin from the bottom edge of the part. DY being the height of the part. To calculate the quadrant position, consider the center of the hole at (Y) - the radius of the hole. Value: 0.
Minimum vertical diameter (mm): minimum drilling diameter, in millimeters. Minimum value: 0. IMPORTANT: as of version 1.60.17.5, the Minimum Diameter field has been removed and replaced by the Minimum Vertical Diameter (mm) field.
Non-through drilling mode: drilling mode for through holes. Value: Slow-Fast-Slow.
Number of horizontal drill bits(X): number of drills, for each horizontal face, present in the machine. Value: 0.
Number of lateral drill bits (Y): quantity of drills, for each side face, present in the machine. Value: 2.
Number of vertical drill bits (Z): number of vertical drills present in the machine. Default value: 13.
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.
Minimium face area for machinings (mm²): minimum face area in mm² for machining operations to be performed. Minimum value: 360000.
Slots
Minimium face area for slots (mm²): minimum face area in mm² for tearing operations to be performed. Minimum value: 360000.
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.