www.kxcad.net Home > CAM Index > EdgeCAM Index >
Use the Five Axis Milling cycle when you need to control the tool movement through (a maximum of) 5 axes within one cycle. Typical applications include swarf cutting, where the side of the tool is driven along the surface, and machining complex cavities such as inlet manifolds.
Drive and Check Surfaces
The toolpath is controlled two types of surface that you digitise:- 'Drive' surfaces that produce the basic toolpath and drive the tilt of the tool, and by 'Check' surfaces that are not to be machined, or gouged, and so modify the basic toolpath.
Note however that the machined surface need not necessarily correspond to the Drive surface; you could use the Check surface instead, see more information...
The surfaces may be surfaces you have created within EdgeCAM, or derived from external parts; that is face features that you have created from a supplied solid model. You might also derive line geometry from the solid for controlling cutting patterns. (For associativity to the model, instead of using wireframe geometry from the Solids menu ► Geometry, command use features from the Solids menu ► Edge Loop Features command.)
Angle Settings Reference
The are many angle and orientation type settings in the cycle, such as 'Tilt Axis' in the Tool Axis Control tab. These are relative to the current tool orientation on the cycle starting (so the vertical (Z) axis is parallel to the tool's axis). The tool orientation can be changed by, for example, a Move menu ► Index, command, and also by Five Axis cycles themselves - see Step 3 below.
Main Steps in Using the Cycle
Here is a general overview of the setup:
Make sure your code generator is based on one of the adaptive templates.
If you are in the Mill/Turn environment (CY or CYB code generator) make sure you are in Planar mode (M-Functions menu ► Planar mode).
To isolate the cycle from tool orientation changes caused by previous Five Axis cycles, we recommend you use Move menu ► Index, so the CPL you index to gives the tool a known orientation. See more information...
Click Mill Cycles menu ► Five Axis. to open the Five Axis dialog.
In the General tab set up the cutting strategy parameters. For example whether the cuts will be along parallel slices or follow curves (such as drive surface edges).
In the Depth tab set up the clearance parameters. In Five Axis machining, having a clearance 'plane' is just one of the choices. Rather than a plane it may be more appropriate to have a cylinder or a sphere, so that the tool does not simply retract in Z, but in other vector directions.
In the Tool Axis Control tab set up the parameters controlling the tilt of the tool. For example whether to tilt the tool so it always points to a fixed position, so that you can machine out a pocket through a narrow opening.
In the Check tab set up the parameters controlling the gouge avoidance strategy, for example whether to tilt the tool, or stop the machining. You can check for gouges caused by any combination the tool and/or its holder, in drive and/or check surfaces.
Set up the leads and links.
Click OK to close the dialog, then follow the prompts for digitising geometry in the Status Bar.
Note that Granite (Pro/ENGINEER) faces/surfaces produce a warning dialog that they are not supported. The cycle still completes if you have also digitised some valid geometry.
