Like the high speed offset 2D cut operation, the rough offset 2D cut is used for 2D area clearance of explicitly defined rough stock. The tool path is first calculated and then projected onto the CAM component geometry.

 

 

Sample Rough Offset 2D Cut operation

 

 

 

Like the lace cut, the rough lace cut operation is a parallel milling technique controlled by stepping parameters. It is used for the removal of explicitly defined rough stock. The tool path is first calculated and then projected onto the CAM component geometry.

 

Sample Rough Lace Cut operation

 

 

 

The rough plunge cut operation is a method used to rough out large parts. These can include deep cores and cavities, high shoulder slots and straight or sloped walls. Those requiring long tools will benefit from this operation. The process is an axial (vertical) drilling and milling operation performed in a single tool sequence.

 

Sample Rough Plunge Cut operation

 

 

 

The rough drill cut operation is used to create access holes to pocket features on the part to be machined.

 

 

 

 

The offset 3D cut operation is used when a smooth and continuous tool path is required in the vicinity of steep walls, milling in uncut or uncutable places or when milling the entirely part as a whole. This is a finishing operation designed to achieve an equal cusp condition over the entire tool path.

 

 

 

The lace cut operation is a parallel milling technique controlled by stepping parameters. The tool path is first calculated and then projected onto the CAM component geometry.

 

 

 

The drive curve cut operation is similar to the offset 3D cut that starts from a custom set of curves. The starting curves can be open or closed. In general it is used like the flowing cut for milling along features. The tool path is first calculated and then can be projected onto the CAM component geometry using the Project Drive Curve parameter.  See QuickMilling Operation Form Parameters for a definition of each parameter.

 

 

 

The z level cut (also referred to as side cut) is used to machine steep walls.

 

 

 

The pencil cut operation is used to clear corners as a follow up to other QuickMilling operations.

 

 

 

The Flow 3D cut operation will "morph" a pattern between pairs of guiding curves. Like the High Speed Flowing Cut, the curve pick sequence when defining the profile features is very important. The pick sequence is maintained during tool path calculation. The Flow 3D Cut could follow a Bulge Cut in a tool path sequence.

 

The cutting pattern can be automatically generated or set between inside and outside patterns. The cutting mode can be zigzag, unidirectional or top/bottom combinations.

 

Requirements include a CAM component (class = Part) or CAM features (class = Surface or Solid). Also required are CAM features (class = Profile) for the flowing projection curves. Optional CAM components (class = Stock, Clamp or Table) are supported as well as CAM features (class = Profile and Type = Containment).

 

 

 

 

This is a 2 axis surface engraving operation (i.e., characters on flat parts). You can use VX True Type Fonts for this operation. After creating the text, use the Explode Text & Dimensions command to create the curves to select for the CAM features.

 

Requirements include a CAM component (class =Part) or CAM features (class = Surface or Solid). Also required are CAM features (class = Profile and Type = Containment) for the profiles to be engraved.  Optional CAM components (class = Stock, Clamp or Table) are also supported.

 

 

 

 

This operation creates a network of bulges on a surface using two intersecting curves referred to as a drive curve (Directrix) and a generator curve (Generatrix). This operation is useful in dispersion networks for automotive lighting parts or as an artistic hammer-paint effect. The Generatrix is used as a pattern generator that is guided by the Directrix.

 

The step size along the Directrix and Generatrix can be specified. The cutting mode can be set to "zigzag" or "unidirectional" and the depth and % of bulge can also be controlled. Bulge noise (a shift in bulge position) in X,Y and Z can be specified at appropriate location when necessary.

 

The requirements for this operation include a CAM component (class = Part) or CAM features (class = Surface or Solid).  Optional CAM components (class = Stock, Clamp or Table) are supported as well as CAM features (class = Profile and Type = Containment).

 

Bulge Cut Tool Path

Bulge Cut Solid Verify

 

 

 

High Speed Machining (HSM) means milling with light depths-of-cut at high feed rates. Milling at lighter depths was always possible, but high speed makes it practical. Now, light cuts do not have to stretch out the tool path cycle time. As a result, the machining center can do more.

 

Through HSM, the machining center can reduce the need for polishing. It can deliver EDM electrodes more efficiently and can even eliminate the need for EDM in some cases. HSM can let a machining center produce complex tooling competitively in a single setup.

 

The smoothness of the machined surface is determined in large part by the height of the cusps between adjacent passes with a ball nose tool. Take a small stop over and cusp height goes down. Continuity and smoothness are primary concerns during HSM tool path operations.

 

VX QuickMilling has taken great care to address geometric related HSM issues. Geometric issues are related to tool path smoothness, continuity and flowing. Geometric issues are generally accepted guidelines in HSM independent of the spindle, holder, tools, material or the machining center.

 

HSM concepts are useful, in general for classic milling as well by increasing machine life, decreasing sound levels, reducing vibrations (good surface quality) and reducing the machining time.

 

Following are some of the concepts implemented in VX QuickMilling for High Speed Machining.

 

• Minimize full width cuts - The ordering of each raster area clearance tool path is determined to minimize occasions when the tool cuts full width. This allows the use of higher feed rates, reducing tool wear and damage particularly during Offset 2D Cut operations.
   

• Smart Clearance - As the work piece is machined, this option will retract the tool as little as is necessary before moving across to another area, rather than retracting above the block each time. This cuts down the number of moves to safe Z and results in reduced milling times.  Smart clearance can be activated by leaving the Clearance parameter of the QuickMilling Lead In/Out Parameters Form blank.
   

• Offset Area Clearance - Toolpaths calculated using an offset area clearance strategy will contain fewer sudden changes in velocity than conventional raster machining - an essential requirement for high speed machining during Offset 2D Cut and Offset 3D Cut operations.
   

• Break after time, length or quantity of material milled - A very important problem that appears in HSM (that will improve any tool path operation in general and roughing in particular, is the splitting tool paths after time (a popular value is 15 min) or after the length of feed moves.
   

• Cusp Height Control - Maintaining constant material removal volume rate is desirable for High Speed Machining. This condition is achieved using cusp height control with constant Z finish machining. In general the Offset 3D Cut operation supports these constraints.
   

• Spiral and Projection Milling - For some shapes, the combination of a spiral strategy with projection milling provides a smooth and continuous cutting path which is ideal for High Speed Machining.
   

• Leads and Links - By selecting the most appropriate lead and linking strategy it is possible to increase the speed of the tool. This increases the surface cutting speed, provides and even loading on the tool and eliminates dwell marks.
   

• Tangential arc or spline - The tool moves onto and off the job in an arc or smooth spline motion. This allows the tool to move smoothly without having to slow down. Lead in and out.
   

• Tool path evaluation - Rapid calculation of toolpaths gives users the ability to modify toolpaths and evaluate a number of different strategies to ensure that the optimum tool path is selected.
   

• Advanced linking - The High Speed Lace Cut, Offset 2D Cut, Offset 3D Cut and Flowing Cut operations contain routines that allow advanced continuity and linking. This allows the tool to stay in contact with surface as much as possible.
   

• Smooth Factor - All HSM operations contain a parameter called Smooth Factor (of step) that allows a smooth stage after tool path construction. This will remove all irrelevant sharp corners inside the tool path.
   

• Classic cycle can have HSM behavior - Classic tool path operations like Lace Cut and Z Level Cut (i.e., Side Cut) do not have the Smooth Factor parameter but they can be converted to HSM operations using the Corner Radius parameter and smooth links and leads. Corner Radius reduces the number of potential undercuts in Side Cut. Corner Radius can be implemented only in operations that have a planar behavior (Lace Cut and Z Level Cut) allowing a smoother tool path.

 

 

 

The high speed offset 2D cut operation is used for 2D area clearance. The tool path is first calculated and then projected onto the CAM component geometry.

 

 

 

This is a more advanced version of the lace cut operation suited for high speed machining. Like the lace cut, the tool path is first calculated and then projected onto the CAM component geometry.

 

 

 

The high speed flowing cut operation will "morph" (only a linear interpolation) a pattern between pairs of guiding curves. Flowing can be along, across or spiral for closed guiding curves. The tool path is first calculated and then projected onto the CAM component geometry.

 

Multiple CAM profile features can be defined for this operation.  Each feature group is considered one span.  The curve pick sequence when defining the profile feature is very important for this operation.  The pick sequence is maintained during tool path calculation.