Profile-NEST Module > 2 Axis Profiling

This Cut Parameters tab is similar for the Mill operations listed below. It allows you to define the cut parameters for the current Profiling operation. You can set Global Parameters, Cut Direction and the Stepover Distance via this tab of the operation dialog. 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 also be specified here. Refer to each option below.

Dialog Box: Cut Parameters tab, Profiling Operations

Cut Parameters tab, Profiling Operations

Global Parameters

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

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

Compensation

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

Cut Direction

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

Understanding Cut Levels in 2½ Axis Machining 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

Cut Start Point for Closed Curves

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

Cutting Side

Specify

Select this option to activate the Cutting Side parameters in this dialog.

Right of Curve / Left of Curve

Right or Left determines the side of the curve to cut. This can be set for both open and closed curves. Right or Left is determined by the start point and direction.

Cut Start Side

Use Inside/Outside for Closed Curves

Select this option if you have a closed curve region. Then select Inside or Outside to have the tool cut on that side.

Inside

Outside

Alternate using Nesting

If your control geometry has nested curves, check this box to alternate the cut side (i.e., Outside/Inside or Inside/Outside). You can use the Sort Parameters tab to sort clustered profiles.

Off

Stepover Control

This is how wide your cut should be. The Step/Cut determines your stepover. For example if Total Cut Width is set to 1.0 and Step/Cut is set to 0.25, there will be 4 passes created.

Total Cut Width

This will determine the stepover for each cutting pass beginning at your total cut width and ending at your control geometry.

Total Cut Width

Corner Cleanup

Check the Corner Cleanup box to automatically detect corners that the tool could not reach between each pass. The system will then add a toolpath based on the uncut area detected.

Perform Global Gauge Check

With this parameter checked, the cutter will not violate any of the selected control geometry. This option only works with closed curves as shown in the illustration below.

Gauge Check ON

Gauge Check OFF