The "Common cutlines" command is used for separating parts with only one cut. This cutting method is much faster than traditional cutting.
The command support three main different methods.
The following settings are common for all methods:
Part distance
Common cutline generates a toolpath without kerf information. The coordinates in the CNC-file always describe the center position of the jet.
The tool center is located between the parts to be separated.
It is important that the distance between the parts is the same as the dimension of the jet. If the distance between the parts (C) is closer, then no toolpath is generated between the parts. If the parts have a larger distance, then (A) and (B) will be cut separately and the (C) portions will be cut two times. The tolerances for the distance are approximately plus/minus 0.01 to 0.05 millimeters.
Info button
By clicking on the Info button, you will have information if some parts are to close to each other.
By activate the checkbox "Use tool diameter" the actual tool diameter will be used. The tool diameter is set in the "Cutting parameters"
Min length
This controls how where the common cutline controls will be applied.
All the yellow lines will be cut with common cutline
Leadin and piercing
The leadin and piercing is simplified in common cutline. The leadin always go 90 degrees perpendicular to the geometry. The settings above will at least be used once when it starts to cut. If it's needed to turn on/off the jet several time, then it will try to start in an existing toolpath using the piercing type "Air start".
Ignore hole
If it's already toolpaths attached to the holes, then this checkbox has no affect. The command does never add toolpath in holes if it already has a toolpath.
Run "Contour" on separated parts
If you select parts that are completely separated from other parts, then you can automatically run the "Contour" on these parts.
Cutting quality
The cutting quality is inherited from the parts. When cutting between two parts that have different cutting quality the toolpath which is common for the part will have the best quality.
Trim to sheet
If the tolerance of a part is not critical, possibly save time by using the edge of the sheet as the edge of the part.
To use this, the parts must be nested close to the edge of the sheet. Check the "Trim to sheet" box.
Sheetwise
This method needs material free from stresses when there is no risk that the sheet will be moved during the cutting.
Cross ramping quality
If the material is thick, then the jet will make a jump when crossing a path that is already cut. There is a risk that the material will not be cut at these points.
Set the cross-ramping quality to a finer value and the cutting speed will slow down at these points (A).
Cutting order
Sheetwise method cuts all holes in all parts and then cuts the lines between the parts. Then the external geometries are cut.
Mix between normal cutting and sheetwise
When internal geometries already have a toolpath, the command will skip these holes. Cut holes with another command before using the common cut.
Partwise
This method cuts each part before starting to cut the next part. There are some settings that differ from the sheetwise option.
Sorting
With this setting you can control in which order the selected parts will be cut.
Gap
Gap is a nice feature that make micro-joints between the parts.
Lines
This method only adds CAD objects between the parts and does not add any toolpath. These objects can later be used by other commands like the "Quick" or "Manual" commands.
Common cuts only
When this checkbox is activated then the command will only generate the lines that should be cut with