Technology page
This page enables you to define the technological parameters of Edge Deburring Recognition.
Chamfer parameters
Cutting diameter
This field enables you to define the starting cutting diameter of the tool.
Depth cutting type
This parameter enables you to define the order of rough passes cutting.
With the One way option, all cuts are machined in the same direction.
With the Zigzag option, the machining direction changes from cut to cut.
Direction
This option enables you to define the direction of the machining.
The options of Climb and Conventional set the tool path direction in such a manner that the climb or conventional milling is performed. The default option is Climb.
Change feed in internal corners
This section enables you to control the feed rate used for machining internal corners. When this check box is selected, the following parameters can be defined:
Previous tool diameter button – enables you to choose the previous tool from the Tool Table or enter the value in the text field.
Previous wall offset – defines the wall offset remaining after a previous operation.
Extension/Overlap – defines the overlap distance that you would like to start and end from the previous larger end mill.
Feed in corners – defines the feed rate you would like the tool to travel when cutting in corners (G2).
Offsets
In the Wall offset field, enter the offset that will remain on the wall after the roughing cut.
For geometries that consist of open chains, Safety offset is the offset that prevents the tool gouging with the vertical wall.
SolidCAM automatically calculates the optimal value of the Safety offset.
Cutting
This section enables you to define parameters of chamfering performed in a number of cutting passes.
Equal step down
When the Equal step down check box is not selected, the distance between each two successive Z-levels is determined by the Step down parameter. If the machining depth is not divisible exactly by the Step down value, the depth of the last cut is smaller than the Step down value.
When the Equal step down check box is selected, an equal distance is kept between all Z-levels. Using this option, you have to specify the Max. step down parameter instead of the Step down parameter. According to the Chamfer depth defined in the operation and modified with the Delta parameter, SolidCAM automatically calculates the actual step down to keep an equal distance between all passes, while taking into account the specified Max. step down so that it is not exceeded.
Step down
Chamfering is performed in constant Z passes. The Step down value defines the distance between each two successive Z-levels.
Copies of the last cut
This parameter defines how many times the last and deepest cut is repeated.
Extension/Overlap
For closed chains, the overlap is the distance that the tool cuts twice: one time at the beginning and one time at the end of the cutting.
Compensation
If the Compensation check box is selected, the tool radius compensation options G4x of the CNC-controller are used in the GCode.
Minimum Edge Length
When a value greater than 0 is entered in the corresponding text field, SolidCAM ignores the chamfering of edges having a chain length less than the specified Minimum Edge Length. The Preview button enables you to display on the solid model the edges that are ignored relative to the geometry chains. The Resume button enables you to return from the preview state to the Operation dialog box.
More...