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 allows you to define the plateau Angle (A). This angle controls which regions will be machined. The system identifies all areas of the part that are shallower than this angle from the horizontal and creates machining regions that are used in the subsequent machining process.

This section allows you to define the type of cut pattern that the tool will follow when it is at each Z level.  There are two types of cuts that you can choose. The first one is an Offset cut type (2D offset) and the second one is a Linear cut type.  In the Offset cut type, the cut regions are successively offset until there is nothing left to machine. This type of cutting is sometimes called spiral machining. You can specify the cut start point to be either the inside of the cut regions or from the outside.

Part 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...

Offset Start Point  
This is enabled when Cut Pattern (see above) is set to Offset.  Choose from Inside or Outside for the offset.

Inside

Outside

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.