3/5-Axis Converter

	`3/5-Axis Converter` may generate 5-axis tool paths. In this case, the post-processor must be able to process 5-axis tool paths.
	The `3/5-Axis Converter` is a process that can be included in the computation of the tool path to convert a 3-axis machining operation into a 5-axis one to avoid collisions. Two axis strategies are available to modify the tool axis of a tool path resulting from a machining operation without changing its contact point either by changing a 3-axis tool path into a 5-axis tool path or by modifying a 5-axis tool path, or avoid the collisions of the tool or the tool assembly within a 5 axis machining strategy, collision checking is performed with the selected geometry, not with the rough remaining from the previous operation.
	It is available for the following tools: All End Mill Tool (spherical and torical), TSlotter and Lollipops (TSlotter with Spherical shape). It is not available for conical tools.
	and for the following commands: Roughing, Sweeping, Pencil, ZLevel, Contour-driven, Spiral Milling, Isoparametric Machining, Profile Contouring, at the bottom of the machining strategy tab.
	Note that for all tools available, the mode `Normal to part` requires contact points. In the operations having no contact points (Pencil, Contouring and Roughing), this mode is not available.
	Select the check box `3/5-Axis Converter` to activate this option. `More...` starts the `3/5-Axis Converter` dialog box with: a machining strategy tab with: a global modification tab and a collisions checking tab. a macro tab Global Modification By default, the global modification is not active. Select the `Activate global modification` check box to replace all the tool axes of the tool path with the one selected in the Tool axis mode list. The dialog box turns into the following: The upper part of the graphic zone of the dialog box represents the initial tool path whereas the lower part represents the modified tool path.
	`Tool axis mode` Lets you select a new tool axis mode from the drop-down list. `Fixed axis` Place your cursor over one of the tool axis arrow and choose `Select` to define the tool axis. `Analyze` starts the `Geometry Analyser`. `Thru a point` The tool axis passes through a specified point. The tool axis can be oriented `To` the point or `From` the point (Click the label `To` to switch to `From` and vice versa). Click the point in the sensitive icon and select a point in the graphic area.
	`Thru a guide` The tool orientation is controlled by a geometrical curve (guide), that must be continuous. An open guide can be extrapolated at its extremities. Click the red curve in the sensitive icon and select a curve in the 3D viewer. The tool can be orientated `From` or `To` the guide (Click the label `To` to switch to `From` and vice versa). `Angle`Lets you specify a lead angle:
	`Normal to part` The tool axis is normal to the part. `Angle`Lets you specify a possible frontal angle between the tool axis and the normal to the part. `Fixed angle` The new tool axis forms an angle with the initial tool axis. `Angle`Lets you specified this fixed angle. `Privileged angle with the tool path` Defines the angle a plane defined by the direction of motion (`Frontal angle`) or in a plane normal to the direction of motion (`Lateral angle`).
	`Normal to drive surface`The new tool axis is normal to the drive surface. `Angle` Lets you specify a possible lead angle: Note that we recommend you use a smooth surface as the drive surface. `Max discretization angle` Specifies the maximum angular change of tool axis between tool positions. It is used to add more tool positions (points and axis) if value is exceeded.
	Collisions Checking The collision checking is active by default. Clear the check box if you do not want to perform a collision checking. The left part of the graphic zone in the dialog box represent the initial tool path whereas the right part represents the modified tool path that will avoid collisions. Decide on which geometry you want to perform the collisions checking: `Part` (selected by default), `Check` (selected by default), `Design Part` of the Part Operation (not selected by default). In that case, make sure that you have selected a valid `Design Part` in the Part Operation. Note that in a Profile contouring operation, you cannot select a part. You must select the `Design Part (PO)` check box and make sure it exists in the Part Operation. `Tool axis mode` Lets you select a new tool axis mode from the drop-down list. It will be applied to the points in collision found. `None` The tool axis is not modified, the tool path stops before the collision point, and the corresponding portion of tool path is removed. `Fixed axis` See Fixed axis above. `Thru a point` See Thru a point above. `Thru a guide` See Thru a guide above. `Normal to part` See Normal to part above. `Fixed angle` See Fixed angle above. `Automatic` The tool axis is automatically computed to avoid collisions.
	`Normal to drive surface` See Normal to drive surface above. Note that we recommend you use a smooth surface as the drive surface.
	You can access more parameters for the above tool axis modes by clicking More>>: For all tool axis modes except `None`: `Max discretization angle` Specifies the maximum angular change of tool axis between tool positions. It is used to add more tool positions (points and axis) if value is exceeded. `Minimum length` Specifies the minimum distance that must exist between two collision points to allow the modification of the tool axis between those two points. For the tool axis mode `Normal to part`: `Angle` Lets you specify a possible angle between the tool axis and the normal to the part. For the tool axis mode `Fixed angle`:`Angle`Lets you specified the fixed angle. `Privileged angle with the tool path` Defines the angle a plane defined by the direction of motion (`Frontal angle`) or in a plane normal to the direction of motion (`Lateral angle`). For the tool axis mode `Automatic`: `Minimum angle` and `Maximum angle` defines the range within which the tool axis can vary. `Step angle` defines the computation step used to find the optimal angle to avoid collisions. The smaller the `Step angle`, the longer the computation time. `Offset on tool` Defines the offset applied on the shank of the tool to avoid collisions. `Offset on assembly` Defines the offset applied on the tool assembly to avoid collisions.
	Optimize Associated Operation This check box is available only for a ZLevel operation with a TSlotter tool, and if `Collision Checking` is activated. It is not selected by default. The ZLevel operation takes the tool body into account to compute the tool path. In this case: the tool with its body cannot machine more material: the tool body is in collision. `Optimize associated operation` computes the tool path with a quasi-null tool body. Optimized ZLevel + 3To5-Axis Converter:
	Macros When collision points found on the tool path are removed, the tool path must be closed. This tab lets you do that with Approach, Retract and Clearance macros.