Global Parameters, 3 Axis Operations

The Global Parameters section allows you to set the tolerance value to be used in machining. Intol and Outol are allowable deviations (tolerances) from the actual part geometry plus the Stock layer (if any).  A uniform thickness or stock that needs to be left around the part can be specified here.

Intol / Outol
Inward tolerance - the maximum thickness of material that can be removed from the Stock layer.  Outward tolerance is the maximum thickness of material that can remain above the Stock layer.

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  
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, but for finishing operations this value is zero.

This section allows you to define the type of cut pattern that the tool will follow when it is at each Z level.  Depending on the operation being used, one or more of these patterns are available for selection in the dialog. 2D Offset is a 2D offset facing pattern.  The cut regions are successively offset until there is nothing left to machine. This type of cutting is sometimes called spiral machining. Stock Offset is a pocketing pattern derived from the stock geometry. Linear creates a straight linear pattern regardless of part or stock geometry.  In each Offset cut type, you can specify the cut start point to be either the Inside of the cut regions or from the Outside.

2D Offset

Linear

This can be controlled by specifying either Climb (Down Cut), Conventional (Up Cut) or Mixed.

Climb

Conventional

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...

Check this box to use a spiral cut pattern for pocketing.

Spiral Pocketing

Pocket Start Point can be set to inside or outside. This is applicable for Part offset and Stock Offset cut patterns.

Inside

Outside

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.

The Linear controls are only enabled when Cut Pattern (see above) is set to Linear.  Select from the following:

Start at Top / Start at Bottom  
Allows you to specify the start point for the Mixed cut pattern.

Angle of Cuts  
Allows you to specify the Angle of the Mixed cut pattern.

Cleanup Pass  
Check this option to cause automatic detection of all the corners that the tool could not reach between each pass. It will then add a toolpath based on the uncut area detected; either a linear cut in case of smaller areas or a cut that travels along the shape of the uncut area, when the area is large. This is applicable for Linear cut patterns.

Cleanup Pass unchecked

Cleanup Pass checked

Stepover Control, 3 Axis Operations

This allows you to define the spacing between the cuts.  Select from the following options:

% Tool Diameter  
Enter the stepover distance as a percentage value of the tool diameter.

Distance  
Enter the exact stepover distance preferred.

Scallop

(not available for all operations)
Enter the scallop height to determine the spacing between cuts.