Pocketing, 2½ Axis

Pocketing, 4 Axis

This is the allowable deviation from the actual part geometry plus the Stock allowance (if any).  In 2 Axis methods, this Tolerance is applied to XY motions only.

Tolerance

How to Increase Tool Path Accuracy Tolerances play a vital role in both design engineering and digital manufacturing.  In design, the goal is to allow the broadest tolerance range possible while meeting your design specifications. This is because, generally speaking, there is a direct correlation between tighter tolerances and higher manufacturing costs. Read the full article...

Stock

This is the thickness of the layer that will remain on top of the part after the toolpath is complete. Roughing operations generally leave a thin layer of stock.  For finishing operations this value is zero.

Stock

This enables cutter compensation.  The compensation direction, left or right, is determined by the Cut Direction selected (Climb or Conventional).

Select Offset and the tool will traverse in successive uniform offsets of the part shape starting from the Inside or Outside depending on the Start Point selection.

Offset

Island Offset

Select Offset Spiral and the tool will traverse in a spiral pattern with successive offsets of the part shape starting from the Inside or Outside depending on the Start Point selection.

Offset Spiral

Select Linear and the tool will traverse in a Linear cut beginning at the Top or Bottom depending on the Start Point selection.

Linear

Select Circular Spiral and the tool will follow a circular path starting from the Inside or Outside depending on the Start Point selection.

Spiral Cut Pattern

Select Radial and the tool will cut in a radial pattern starting from the Inside or Outside depending on the Start Point selection.

Radial

Select High Speed to add progressive arc-shaped passes that reduces tool pressure and keeps chip load more consistent, allowing for higher cut feedrates.

High Speed

When the High Speed cut pattern is selected with a Start Point defined, a trochoidal motion is added between the Start Point and the start of the High Speed motion cut pattern.

Trochoidal Start Cut Motion

Select Climb (Down Cut) and the tool will be maintained in a downward motion into the stock.

Climb (Down Cut)

Select Conventional (Up Cut) and the direction of the tool will be maintained in an upward motion out of the stock.

Conventional (Up Cut)

Select Mixed and the direction of cutting is alternated between each parallel plane.  This is a mixture of both Climb and Conventional cutting of the stock.

Mixed

Understanding Climb vs Conventional Milling One of the basic concepts to understand in any milling operation is Cut Direction.  It can be characterized by how the flutes of the cutting tool engage the stock material and form the chip that is removed during cutting. In many of MecSoft CAM’s 2½ & 3 Axis toolpath strategies you will see that Cut Direction is defined by selecting one of three options, Climb, Conventional or Mixed.  Let’s take a look at the characteristics of each option. Read the full article...

Specify the Angle of Cuts (0-360) measured from the X Axis.  This additional parameter is available for some operations when a linear cut pattern is used.

Lift Cut

During the High Speed cut pattern use this parameter to lift the cutting tool during transfer motions.  0 (Zero) means that the tool will not list.  Enter a positive value and the tool will lift this amount in +Z prior to executing a cut transfer motion.

Feedrate Factor

During the High Speed cut pattern use this parameter to control the feed rate when the cutting tool is lifting and plunging before and after each cut transfer motion.  The value is a percentage of the Cut Feed (Cf) parameter for this operation (i.e., 50 = 50% of the (Cf) feed rate).

Select this option if you want the starting locating for the cut pattern to begin at the bottom of the cut pattern (i.e., min Y).

Start at Bottom

Choose where you want the cut pattern to begin, Inside the pattern or Outside.

Inside

Outside

Specify the stepover distance for the current operation as a percentage of the active tool diameter (% Tool Dia) and then enter the percentage value.

% Tool Dia.

Specify the stepover for the current operation as an exact Distance and then enter the distance value in the field provided.

Distance

Add cleanup loops at the corners of pocket areas.  Select None, Inside or Outside.  Refer to the illustrations below.

Inside

Outside

Automatically detect corners that the tool could not reach between cut level and add a toolpath based on the uncut area detected.  Either Linear or Offset cut patterns are used in these areas.

Cleanup Pass

No Cleanup Pass

When checked, the system tries, when possible, to keep the cutter in contact with the cut level plane while connecting all areas within a single machining region.  Otherwise the cutter will retract and re-engage.