2013 R1 is a release combining new strategies with an improved user interface across many aspects of the software. The strategies will make creating tool paths effortless and the improvements to the user interface will get your result much faster than before.


EDGECAM Wire Erosion

EDGECAM’s new Wire Erosion product is based on the industry leading Hexagon PEPS Wire product and offers an intuitive environment for the comprehensive programming of all Wire EDM machine tools. Including a comprehensive library of proven post-processors and knowledge-based cutting schemes as standard. Users can select from one of the pre-defined machining strategies such as 'Unattended night runs' and 'Attended day runs' or, alternatively, define their own.

Features inlude :

  • Pre-configured code generators, optionally configurable.
  • Knowledge-based cutting schemes.
  • Roughing and finishing cuts easily applied to multiple punches / dies.
  • Reverse cutting with offsets and cutting technology changes.
  • Multiple strategies for corner types; including square ISO and conic.
  • Toolpath display indicators showing thread wire, cut wire and program stop positions.
  • No-core pocket destruction of round and irregular shapes.
  • No-core pocket destruction considers pre-hole diameter to eliminate air cuts and reduce cycle time.

New Rough Profile Cycle

This is a new cycle that replaces the Rough Profile cycle. It is available with all Turning and Production Licenses.

The Rough Profiling cycle removes material in a series of cuts parallel to the input profile and is typically used for roughing free form profiles from free form stock billets. It is also useful for cutting materials where it is beneficial to minimise re-entrant cutting as it keeps the tool in contact with the material for longer.

Benefits of the new cycle include:

  • Cycle is optionally stock aware to eliminate air cuts and reduce cycle time.
  • Intelligent stock entry and exit.
  • Support for controller tool offset i.e. G41/G42.
  • Possibility to enter a constant cut depth or different cut depths for X and Z.
    Specify ZX or Constant Offset finishing allowance.
  • Possibility to enter different offsets for each face element.
  • Option to stop after a specified no. of cuts, return to a safe swarf clearance position, stop the machine, clear the swarf then carry on.
The old Rough Profile cycle has been removed from the default user interface but can be retrieved using Customise -> Commands -> Turn Cycles.

Roughing - Waveform Improvements

Waveform roughing has been improved to include the following enhancements :

  • The Waveform strategy now has the ability to set the Approach Type; Helix and Pre-drill are possible. It works in the same way as the other strategies. A 10% bigger drill tool is expected for the pre-drill option.
  • Waveform pattern has been improved to avoid unnecessary cutting interruptions when opening the initial 'virtual pocket'. The transition between this area and actual toolpath is much smoother.
Percentage Plunge Feed added to Approach Options
The Plunge feedrate for approach moves can now be specified as a percentage of the Plunge feedrate on the General tab. This option is available for all Roughing strategy types.
Clean Up Final Pass added to Control Options
Some machines tools, due to the "Look Ahead" calculation and the high feeds, may leave pegs in the material showing unmachined areas. These pegs would be removed if the feeds were reduced, meaning that the toolpath is correct but, due to the "Look Ahead" calculation, the machine tool is avoiding those areas. Clean Up Final Pass has been added to the Control options which will add a pass at the end of the area to ensure that all material has been removed.

Moving the Sub-spindle - Option to Return Home without the part

The sub spindle can be docked to support the part for a machining process after which it may be sent back to its home position without the part. Previously, the stock was always returned home with the sub spindle - this is now optional.

There is an additional code constructor:

  • Sub Spindle Retract Empty. This is used to format the NC code for the Return Home Without Part option.

Turning Tool dialog - Machining of Internal Holes & Reverse Radial Tools

Machining of internal rotary holes has been improved to provide better access and handle situations which were previously not possible. Two situations have been improved:  

  • Correctly handle internal holes when using a Radial tool.
    Typical work for very large parts where the whole turret can sometimes go inside the component to do machining.
  • Load a Reverse Radial tool. which on an Index type turret will allow for two situations (driven by machine parameter).
    Either load the tool at the front of the turret (with special holder / mounting mechanism) or load the tool at the back of the turret.

Five Axis Milling dialog - Direct Picking on Model

Previously, the Five Axis cycle had to use geometry created from the solid, for example, Edge Loops and Face Features. The cycle can now pick edges and faces directly from the model without having to create Edge Loops or Face Features.

Improved Collision Avoidance (3 to 5-Axis and Five Axis Cycles)
In EDGECAM 2013 R1, a new Remove Remaining Collisions option has been introduced. This option, when checked, will remove any collisions remaining after the main checks have been completed by retracting the tool away from the surface.
New Advanced Five Axis Options
In EDGECAM 2013 R1, new Chaining Tolerance and Slow and Safe Path Creation options have been introduced on the General tab:
  • Chaining Tolerance is an internal value, greater than zero, used for the toolpath generation. The Chaining Tolerance might have an effect for a flat or slightly curved face where, since less tool path points are generated, the toolpath has less information. In this situation the chaining tolerance makes the toolpath accurate. However, if a smaller tolerance is selected, more computing time is required.
  • When Slow and Safe Path Creation is checked, the Chaining Tolerance will be set to an interval not longer than the maximum stepover distance. As with the Chaining Tolerance, activating this parameter requires more computing time.
5 axis cycle - separate process and 64-bit support
In EDGECAM 2013 R1, a 5 Axis cycle will always be moved into a separate process, regardless of whether Set Safe Start Point (SSSP) has been set.
A 64-bit version of the application has also been created (EdgeSrv5Axis64.exe).
This will improve situations where the cycle previously ran out of memory during calculation.

Profiling - Break Corner options for Profiling Cycle

The Profiling cycle has been updated to include options to break sharp corners with either a radius or chamfer. This will reduce secondary de-burring operations.

Set Safe Start Point for Mill/Turn (Background processing)

Set Safe Start Position is now available in the Mill/Turn environment. Turning cycles are not affected.

The Safe Start Point can now be set up using the options in the new Background Processing tab:

  • Two safe points can be defined for each turret when there is a Sub Spindle. Only one is required when no Sub Spindle is present.
  • Only Main Spindle points need to be defined; Sub Spindle points will be created automatically.

Automatically Finding Features - Feature Finder recognises U and V style grooves

Feature finder now recognises U and V style grooves and sets appropriate attributes. This is useful for machining of such features using strategies.

The new Groove Type Attribute defines:

  • V style grooves need to have equal side wall angles.
  • U and V Style Grooves need to start and end at same level.
  • U and V style grooves can include a lead in corner radius or chamfer.
  • U style grooves need to have a full
  • 180 degree base radius.
  • V style grooves can include a blend radius at its base.
  • V style grooves have Included Angle attribute.
  • U and V style grooves have Groove Width attribute. This is the distance across the top of the groove.

Feature Finder - Holes

It is now possible to find holes from a "dumb" model, add them to the model tree and edit them, if required, within Part Modeler.
This new introduction will :

  • Allow ALL "dumb" holes in the solid model to be defined and edited within Part Modeler.
  • Allow users to add extra information to "dumb" holes, e.g. thread data.
  • Allow similar holes to be processed as a group.
  • Allow similar holes to be processed individually.

Feature Ordering Enhancements

Feature Finder internally groups features with similar attributes prior to performing a nearest next sort.

Nearest Next
Mill features on the same solid that share the same CPL level are now ordered using a "nearest next" logic. This ensures that the features are in a reasonable machining order for use by Strategy Manager and Planning Board. This is primarily needed in the milling environment where you have a plate with many pockets.
Feature Find internally groups features with similar attributes before performing a "nearest next" sort and automatically ordering the features:
  • Closed Pockets, Open Pockets and Open Mill features are considered together for the purpose of internal grouping. The feature attributes that are considered for internal grouping are MaxXyRadius (range +/- 50%), Depth (range +/- 50%), Lower Radius (exact) and MinimumXYRadius (exact). Each feature group starts at the bottom left.
  • In the example, all attributes are identical except for the MaxXyRadius (The radius of the greatest circle fitting inside the top contour).
  • Internal groups have been identified by colour and these groups would typically be roughed / rest roughed with different tooling sets. However, all of these features have the same MinimumXYRadius and would, therefore, be finished with the same tool. The feature order used for roughing is, therefore, not necessarily useful for finishing.
Features on Parallel CPLs (Z axis) are considered together
The predefined manufacture ordering now groups all mill / hole features on CPLs which share the same Z same direction together. This ensures that the order of features is highest level first irrespective of CPL. Previously, mill and hole features were sorted by CPL and then CPL level.
Previously, if Feature Find was run more than once on different CPLs, features could be identified on different CPLs which shared the same Z direction. In this situation, ordering features by CPL could lead to features on a lower level being ordered before features on a higher level.

Planning Board – Automatic Ordering

Feature Find automatically orders features into a logical order for manufacture. Machining Strategies can subsequently be assigned to each feature. Typically, a feature will be assigned a minimum of one roughing and one finishing strategy. The Planning Board can now be automatically ordered based on the priority setting assigned to each strategy. Strategy Manager (File Properties) is used to assign a priority to a strategy.

Automatic Ordering has been added to the Planning Board:
  • In Strategy Manager, File Properties specify a priority for each strategy. When the planning board is populated, it is automatically ordered based on this priority setting.
  • In the sample set of EDGECAM strategies, priorities have been set so that all rough turning is done before finish turning and rough milling is done before finish milling.
  • Automatic Ordering is enabled by selecting Auto Sort Planning Board on the General tab of the Preferences dialog or can be done by pressing the Sort by priority button.