Grooving Operation Grooving OperationThis operation enables you to perform a groove either on a longitudinal geometry (internal or external) or a face geometry. The resulting tool path can either use a single machine cycle, generate all the tool movements (G0, G1) or generate several machine cycles.
The geometry for this operation must start and end either at the material boundary or outside it. In case the geometry starts or ends inside the material then the geometry is extended by lines that are drawn from the ends of the geometry, either parallel to the X or Z-axis, depending on the Mode, up to the material boundary.
This field has two options:
This option enables you to execute longitudinal Grooving (principal working direction is the Z-axis direction).
This option enables you to execute facial Grooving (principal working direction is the X-axis direction).
This field has two options. These two options are different, depending on the process type.
This field enables you to choose between the following three options:
A semi-finish pass is a single pass that is executed before the finish pass, at an offset from the geometry. This field has three options:
No semi-finish pass is executed.
This option is active only if the tool is of type Groove. A semi-finish pass is executed; the tool movements are generated in such a way that only the bottom of the tool cuts the material. This can cause the tool to move opposite to the direction of the geometry and also there will not be a continuous movement of the tool on the geometry.
A semi-finish pass is executed; the tool moves in the direction of the geometry.
When you click on the Data button, the Semi-Finish dialog box is displayed.
A finish pass is a single pass that is executed at the end of the operation. This field has three following options:
No finish pass is executed.
Turn_Groove_Method
This option is active only if the tool is of type Groove. A finish pass is executed; the tool movements are generated in such a way that only the bottom of the tool cuts the material. This can cause the tool to move opposite to the direction of the geometry and there will not be a continuous movement of the tool on the geometry.
The finish pass is executed; the tool moves in the direction of the geometry.
SolidCAM recognizes the rest material areas left unmachined after the previous operations.
SolidCAM enables you to produce semi-finish or finish paths with the two following options:
• Entire geometry;
• Rest Material only.
In this case SolidCAM removes the rest material with the tool path based on the entire profile geometry.
SolidCAM machines only the rest material area.
SolidCAM enables you to define the start and end extension in order to overlap the rest material area.
This field affects the start and end position of the tool. It defines the safety distance from the material, at which the tool box is positioned, at the start and end of the operation. You are prompted to enter the Safety Distance value.
This field defines a tool offset number in the machine tool table. This specifies the offset number of the other side of the tool, and is used for a groove cycle for a single line groove geometry. If the Second Offset number is equal to the tool number, then the groove line is shortened by a length equal to the parameter G of the grooving tool; otherwise the whole line is handled by the machine cycle.
|
|
|
|
Second offset is equal to the tool number |
Second offset is not equal to tool number |
The Modify profile parameters Offset X and Offset Z enable you to define an offset for the Machining Geometry. The machining will be performed on the profile modified by the specified offsets.
This field enables you to choose among three following options:
The program updates the geometry according to the tool shape and generates the G-Code for the CNC-controller cycle including the parameters needed to execute the cycle and the G-Code of the updated geometry.
The program updates the geometry according to the tool shape and then calculates the minimum tool movements needed taking into account the material boundary at the start of the operation.
Machine groove cycles are used for every vertical cut step.
This field enables you to define extra parameters that are not needed for the calculation of the tool paths but are needed for the generation of the G-Code (e.g. Gear that decides whether the gear should be High or Low). These parameters are defined in the GPPTool general post processor module (through the *.mac file). Each such group of extra parameters can be defined as one line in the *.mac file:
groove_type = <group-name> Y Parm1 Parm2 .... Parm8
The way these parameters are then passed to the G-Code file is defined through the *.gpp file for the particular controller.
