Turning Operation Turning OperationThis operation enables you to turn a longitudinal or face profile. The resulting tool path can either use the turning cycles of the CNC machine, if they exist, or it could generate all the tool movements. In case the tool movements are generated by the program, then minimum tool movements length is generated taking into account the material boundary at the start of the particular operation. The profile geometry is adjusted automatically by the program, if needed because of the tool shape, to avoid gouging the material.
The geometry must start and end either at the material boundary or outside it. In case the geometry starts or ends inside the material, the geometry is extended by lines that are drawn from the ends of the geometry up to the material boundary; these lines are either parallel to the X or Z axis, depending on the Process type.
This field has two options:
This option enables you to execute longitudinal turning (principal working direction is the Z-axis direction).
This option enables you to execute facial turning (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 is active only if the machine supports compensation and the tool's origin is of Tangential type; if the tool's origin is of Center or Define type, this field is unavailable. It has two options:
The radius of the tool nose is not taken into account when calculating the tool movements. No tool nose radius compensation (G41/G42) is used in the G-Code.
The radius of the tool nose is not taken into account when calculating the tool movements. However, the tool nose radius compensation (G41/G42) is used in the G-Code.
This field enables you to control the turning type by choosing between three main options:
This field is available only in case of Work Type set to Rough or Copy.
This field defines the type of the step down. It is relevant only in case of Work type is set to Rough or Copy. It can have two options:
Constant
If this option is chosen, you have to enter the constant step down value in the Value field.
Single
If this option is chosen, the turning is executed in one step down.
The Data button enables you to set additional Rough/Copy parameters. The Rough or Copy dialog box will be displayed depending on your Work type setting.
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:
This option is active only if the tool is of Groove type. 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. Moreover, the tool will not move continuously on the geometry.
The 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 job. This field has three options:
No finish pass is executed.
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. Moreover, the tool will not move continuously on the geometry.
A 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 has the following two functions:
- It defines the length with which the tool paths are extended outside the material at the end of every tool path. The tool paths are extended only when needed in order to make sure that the tool does not drop in Rapid mode into the material between one step down to the other.
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 option enables you either to define the tool start position for the Rough, Semi-finish and Finish passes or to let SolidCAM choose it automatically. This field has two options:
The tool start positions for all the passes will be automatically decided by SolidCAM. You should check this position through the simulation, especially in case of Cycle set to Yes, to make sure that the start position chosen by SolidCAM is suitable for the type of cycle in your machine.
You will be prompted to pick the Tool start positions for all the passes.
You must make sure that the tool, when located at the chosen start position, is out of the material because the tool arrives to the tool start position in Rapid (G0) mode.
The tool start position has a big effect on the tool paths when (Use Cycle is set to Yes). In this case the tool paths in the CNC-controller are calculated as follows: from the tool start position a line is drawn to the first point of the geometry. All the tool paths then start from this line. When (Use Cycle is set to No) the tool path calculations are not affected by the tool start position since the tool simply moves from this point to the start position of the first tool path.
This field enables you to decide whether the turning cycles of the CNC machine are used (choose Yes) or the tool path movements are generated by SolidCAM (choose No).
In case of Yes, 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.
In case of No, 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.
|
|
The simulation in case of Yes might be slightly different from the actual machine cycle. |
This field enables you to define extra parameters that are not needed for the calculation of the tool paths but are needed for generating 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:
turn_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.
