The Global Parameters section allows you to set the tolerance value to be used in machining. A uniform thickness or stock that needs to be left around the part can be specified here.

Tolerance  

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

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

Compensation  

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

•Geometry at Top
Use this option if the selected machining region for the chamfer is at the top edge of the part.

•Geometry at Bottom
Use this option if the selected machining region for the chamfer is at the bottom edge.

Geometry At Top

Geometry At Bottom

•Chamfer Width / Height

Select Width to define the chamfer by width and then enter the width value.  Make sure your tool diameter is large enough to encompass the width of the chamfer as shown below.  If you need stepover, use the Profiling operation instead. Chamfer Width

•Tooltip Clearance

This is a vertical depth value that you can add to make sure the tip of the tool clears the bottom edge of the chamfer.  This will remove any possible material and/or witness lines.   Tool Tip Clearance

•Max. Depth/Cut  

This tells the system how deep to cut at each pass.  If this value is smaller than the total chamfer depth, multiple passes will be used to achieve the final depth.  This is a stepdown, not a stepover.  If you need stepover, use Profiling instead. Max Depth/Cut

Climb (Down Cut)  

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

Climb (Down Cut)

Conventional (Up 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)

Mixed  

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...

For Z Level Cuts

When Mixed is selected, zigzag motions are applied between step downs to eliminate tool retracts between z levels.  If Climb or Conventional is selected, retract between z levels are applied.  Refer to the images below:

Climb or Conventional

Mixed

This determines the side of the curve to be cut.

Right / Left  
This can be set for both open and closed curves.  For example, for a clockwise arc/circle, the right side would be inside the arc/circle and the left side would be outside the arc/circle.

Cut Start Side – Right

Cut Start Side – Left

Use Outside or Inside for Closed Curves  
For closed curves, you can set the Cut Start Side by selecting Use Outside or Inside for Closed Curves and select Outside or Inside.

Determine using the 3D model  
If a 3D model is being used, check this box to automatically determine the Start Side.  This option may not be available for all 2½ Axis operations.

Note: This feature is not available in Xpress configuration.

Use Mid-Point of longest side

Check this box to move the cut start point to the mid-point of the longest side of a closed curve.

Use Midpoint of Longest Curve

Specify the Total Cut Width for the operation.  This width is measured from the tool center (not from the edge of the part).  The Step/Cut is a stepover distance for each pass within the Total Cut Width.

Stepover