Remachine

Remachine Milling performs Finish operations on areas where the previous cutter could not finish and is designed for the very final stages of machining. These areas are known as Remachining Areas.

Remachining Areas are created when material is left in areas where the finishing tool has not been able to remove all Surface Stock (such as in angles with a radius smaller than the radius of the previous cutting tool).

After the executing Remachining toolpaths, the part will generally be in a finished state. You may be required to use a number of Remachining toolpaths with a series of smaller tools, in order to remove all the material from Remachining Areas.

Remachine Technologies

The following Remachine technologies are available in Cimatron:

Remachine procedures

Cleanup	Identifies and cleans unmachined areas that remain after previous machining operations.
Cleanup Contours Only	To enable the use of any cutter combinations, this procedure enables the creation of auxiliary contours in the Cleanup procedure, without creating motions. These contours can then be used later as input to any other procedure. This procedure displays a limited number of the parameters that appear in the Cleanup procedure. This procedure is only displayed in the Remachine subselection dropdown list if the checkbox option Cleanup - "Create Contours Only" Option is selected in the Preferences > General > General NC.
Corners Plunge	Create plunging motions with a plunge cutter at rounded corners of pockets. The pockets are created by the Pocket Manager. The plunging motions are parallel to the cylinder of the corner that may be vertical or slanted. The approach is parallel to the cylinder and the retract is horizontal.
Guided Cleanup	The Guided Cleanup procedure ignores the direction vectors from the Remachine Segments Table. Each segment or group of segments are milled from the Z direction. In this case a Cleanup procedure is created for each direction. This is a 3X procedure.
Multi Axes Guided Cleanup	The Multi Axes Guided Cleanup procedure uses the direction vectors from the Remachine Segments Table. This procedure tilts all motions created by a pencil curve to the vector direction of that curve. Each segment or group of segments are milled by the direction associated with it, making it a 3+2 Axis procedure. This is a 5X procedure.
Pencil	Machine one pass along all internal sharp corners in the part, as well as areas with radius of curvature smaller than the cutter radius. The results of this procedure are clean and smooth internal corners.
Rest Milling	Calculates the milling regions based on the Previous Cutter, allowing any cutter combination and milling those regions using the Finish Mill by Limit Angle procedure technology.

Legacy Procedures:

Along Contour All Area on Surf.	Create alternating passes, tangent to the milling surface. This allows for true Climb or Conventional milling. In addition, approach and retract motions are surface tangent arcs, providing smooth approach and retract. In Along Contour All Area On Surface, both horizontal and vertical areas are milled the same way, on surface.
Along Contour Only Horiz on Surf.	Create alternating passes, tangent to the milling surface. This allows for true Climb or Conventional milling. In addition, approach and retract motions are surface tangent arcs, providing smooth approach and retract. In Along Contour Only Horizontal On Surface, only horizontal areas are milled, on surface.
Along Contour Split Horiz. / Vertical	Create alternating passes, tangent to the milling surface. This allows for true Climb or Conventional milling. In addition, approach and retract motions are surface tangent arcs, providing smooth approach and retract. In Along Contour Split Horizontal / Vertical, the horizontal areas are milled on surface, and vertical areas are milled in Constant Z down steps.
Along Contour Vertical + All on Surf.	Create alternating passes, tangent to the milling surface. This allows for true Climb or Conventional milling. In addition, approach and retract motions are surface tangent arcs, providing smooth approach and retract. In Along Contour Vertical + All On Surface, all surfaces are milled on surface. In addition, the vertical areas are also milled in Constant Z down steps.
Legacy Pencil	Machine one pass along all internal sharp corners in the part, as well as areas with a radius of curvature smaller than the cutter radius. The results of this procedure are clean and smooth internal corners. Legacy Pencil is a type of finish milling that smoothes the corners of the geometry. Legacy Pencil supports any kind of cutter with a ball / bull nose (including a taper and shank cutter).
Only Vertical Area	Only vertical areas are milled, in constant Z down steps.
Parallel All Area on Surf.	The cutter moves in parallel motions. In Parallel All Area On Surface, both horizontal and vertical areas are milled the same way, on surface.
Parallel Only Horiz. on Surf.	The cutter moves in parallel motions. In Parallel Only Horizontal On Surface, only horizontal areas are milled, on surface.
Parallel Split Horiz / Vertical	The cutter moves in parallel motions. In Parallel Split Horizontal / Vertical, the horizontal areas are milled on surface, and vertical areas are milled in Constant Z down steps.
Parallel Vertical + All Area on Surf.	The cutter moves in parallel motions. In Parallel Vertical + All On Surface, all surfaces are milled on surface. In addition, the vertical areas are also milled in Constant Z down steps.
Spiral All Area on Surf.	The cutter moves in spiral motions. In Spiral All Area On Surface, both horizontal and vertical areas are milled the same way, on surface.
Spiral Only Horiz on Surf.	The cutter moves in spiral motions. In Spiral Only Horizontal On Surface, only horizontal areas are milled, on surface.
Spiral Split Horiz. / Vertical	The cutter moves in spiral motions. In Spiral Only Horizontal On Surface, only horizontal areas are milled, on surface.
Spiral Vertical + All on Surf.	The cutter moves in spiral motions. In Spiral Vertical + All On Surface, all surfaces are milled on surface. In addition, the vertical areas are also milled in Constant Z down steps.

Workflow

The workflow for NC Technologies consists of the following steps:

- Machine Definition. More:More:

This application enables you to construct a machine definition for the Machine Simulator. It enables defining the kinematics tree structure, the axes, and the displayed components of the CNC machine. This enables you to simulate the G-Code motions on a virtual machine that imitates the real machine behavior.

Important! This application is for use by qualified personnel only. Contact your Cimatron Provider or Reseller to get a machine definition for the Machine Simulator.

- NC Setup and Configuration. More:More:

The NC Setup enables you to predefine multiple project-related options in a single place. The NC Setup contains the general data associated with a project, such as the part material, part geometry, machining orientations, fixtures, initial stock, machine name, and post processor. The data defined in the NC Setup is later used as the default for various NC operations. For example, the defined part material is used to set different machining parameters in the cutter definition. The NC Setup parameters can be edited as required.

- Stock definition and update. More:More:

Stock is a 3X procedure used to represent the stock material from which the final part will be produced. Remaining stock is calculated after each procedure so that cutter motions can be optimized upon the current stock status. Stock is also used by the Simulator and Verifier. The remaining stock can be displayed at any time after any executed procedure (the procedure must have a status flag).

- Cutters and Holders definition. More:More:

Select a cutter for a procedure, define cutters and holders, and set machine and motion parameter defaults for specific cutters.

Example:Example:

- Procedure selection. More:More:

Create a Procedure in the active toolpath. A Procedure is a set of cutter movements that conform to a specific machining technology. One or several Procedures can comprise a toolpath.

See Technologies, below.

- Geometry definition. More:More:

The Geometry Parameters define the geometrical entities to be used during the procedure operation.

- Review and output of the toolpath. More:More:

Once the toolpath is created and the procedure has been executed, perform operations on the toolpath to display and analyze the toolpath or edit cutter motions (Navigator, Global Filter, Motion Editor).

- Simulation. More:More:

The Machining Simulation tools offer a combined environment for machining simulation that includes the following capabilities: material removal simulation, machine simulation, and verifier. These tools enable you to simulate and verify your NC toolpaths and procedures before implementing them on the shop floor.

- Report. More:More:

The NC Report is a file that provides various information about a set of selected procedures. This information includes details about the project and provider, as well as toolpaths, procedures (including multi-cutter information), and parameters.

- Post Process. More:More:

A Cimatron Post Processor is a program that translates Cimatron NC (Numerical Control) data (toolpaths and procedures) into specific CNCCNC(Computer Numerical Control) machine tool commands (machine code). These commands are known as Posts or G-Code programs (see the Glossary for additional information on G-Code).

Important: This application is for the use of qualified personnel only. Contact your Cimatron Provider or Reseller to create the appropriate G-Code.

Some functionality may be dependent on the product package. Contact your Reseller if you require a license.