SimplyCam V3. Documentation

SimplyCam V3
- Introduction
Interface
- Zoom and Pan
- Status Bar
- Snap
- Layer
Toolbars
Vectorization
- Vectorize
Settings
- Settings
Toolpath Manager
- Simulation
- PostProcessor
Mill Toolpaths
- Contour
  - Tools
  - Profiles
  - Parameters
    - Lead In/Out
    - Tabs
- Pocket
  - Tools
  - Profiles
  - Parameters
    - Lead In/Out
- Drill
- Parallel
Laser, Plasma, Waterjet Toolpaths
- Cut
  - Tools
  - Profiles
  - Parameters
    - Lead In/Out
    - Tab
- Laser Engraving
  - Tools
  - Parameters
Lathe Toolpaths
- Lathe Rough
- Lathe Finish
Mill tutorials
Laser, Plasma, WaterJet tutorials
Lathe tutorials

Cut Parameters

This dialog contains the parameters specific for the Cut toolpath.

Feed Plane
The parameter sets the Z coordinate at which the tool moves at rapid traverse (G0).

Stock to leave
Sets the value of material to leave (or remove) on the profile; example, to perform a subsequent finish pass with another tool.
A positive value leaves the material.
A negative value removes material.

Lead In / Lead Out
This parameters controlling how the tool approaches the part at the start of each pass and how the tool retracts from the part at the end of each pass in the toolpath.
More information ....

Tab
This parameter allows, in case the machining removes all the material around it, to set the supports in the chained geometry, to avoid the detachment of the part.
More information ....

Method of calculation:
Defines the algorithm used in the calculation of contour machining. There are three modes:

- Standard:: Each profile is calculated individually.
Fast calculating with complex contours by a lot of information.
Are allowed Tab
Is allowed the starting point.
Use the machining tolerance for the calculations.
Only one profile at a time is controlled and maintained intact.
- Group profiles:: All profiles defined for the machining, are grouped as a single object before the calculation.
The adjacent profiles defined in the selection, are controlled and maintained intact.
Fast calculating with complex contours by a lot of information.
Use the machining tolerance for the calculations.
Are still not allowed Tab
We currently do not use the starting point defined in the chain.
- Pairwise Algorithm:: Very precise toolpath generation, does not use the approximation of the machining tolerance.
Each profile is calculated individually.
Are allowed Tab
Is allowed the starting point.
Slower in the calculation with complex contours by a lot of information.
Fails with lots of small entities, overlapping or self-intersecting.
Only one profile at a time is controlled and maintained intact.

Cutting Rules
This parameter determines the type of optimization in the execution of the cuts, when multiple profiles are defined.

- None: No optimization is applied to the toolpath.
- Shortest path:: With this option, SimplyCam creates the shortest path between the various profiles.
- All inside first:: SimplyCam performs before cuts inside profiles and then cuts outlines. Useful when the whole piece, composed of more than one profile, is cut and would lack external support.
- Layer priority:: SimplyCam performs the cuts, in the increasing order, with which the geometric profiles are stored on graphic layers. First will be cut profiles lying on Level 0, then the profiles lying on level 1, etc.. etc..

Transform
This option allows you to arrange multiple parts on the same workpiece.

Calculate button
Performs the calculation process of the toolpath, using the profiles chained and the current parameters defined.