Coons Parameters tab

Use the Coons Parameters tab to enter the toolpath parameters for a Coons patch wireframe toolpath. This toolpath divides the area bounded by across and along curves into a series of patches.

The first picture below shows a series of contours oriented in across and along directions. The other picture shows the Coons patch toolpath Mastercam creates from this geometry.

A series of contours oriented in across and along directions. A series of contours with the Coons patch toolpath overlayed in red.

Follow these steps:

  1. Select a cutting direction—either across the calculated surface, or along it.
  2. Enter the step sizes for each cutting pass. See Across and Along Cut Distances for Coons Toolpaths.

  3. Select a cutting method. This determines the pattern that the tool follows over the part surface.

    NOTE

    The 5-axis cutting methods work only if 5-axis tool motion is supported in the current machine definition. They are not supported in Mill-Turn.

  4. Enter other toolpath dimensions and compensation options.

Along cut distance

Sets the distance between cuts in the along direction. Stepover is applied to the longest along boundary. This parameter determines surface smoothness. A smaller increment takes longer to process, but works well for more extreme surface curvatures. The more drastic the curvature on the part, the smaller the step size should be. On a fairly flat surface, you can use a larger cutting distance (for example, 0.150).

Across cut distance

Sets the distance between cuts in the across direction. Stepover is applied to the longest along boundary. This parameter determines surface smoothness. A smaller increment takes longer to process, but works well for more extreme surface curvatures. The more drastic the curvature on the part, the smaller the step size should be. On a fairly flat surface, you can use a larger cutting distance (for example, 0.150).

Cutting method

Sets the tool motion during the lofted toolpath. Select Zigzag, One way, Circular, or a 5-axis strategy.

The 5-axis options are not supported in Mill-Turn.

Blending

Determines the type of patches created for the Coons toolpath. Linear blending is recommended on single patch surfaces. Cubic with slope matching blending is recommended for multiple patch surfaces. Parabolic and cubic blending tend to produce flat spots on the surface.

Stock to leave

Enter the amount of material to leave on the part model when the operation is finished.

Rapid depth (abs)

Sets the height from which the tool plunges at the rapid speed before it machines the part at the feed rate. The tool also retracts to this height when moving between toolpath segments. This parameter is an absolute value.

Compensation in computer

Generates a toolpath with compensation for the tool radius, but does not allow for tool wear adjustment at the control. Left and Right offset the tool by its radius; Off causes the tool to cut the center line of the geometry.

Tip compensation

Sets amount of offset to the tool's center or tip for bull-nose and ball (spherical) tools. Used for touching the tool off the part. For multiaxis toolpaths, Tip compensation outputs the tool tip offset as either the tip or the corner radius distance from the tip.

Sync option

Lines up the across and along boundaries. Selecting Manual or Manual/density requires additional data input.

Along

Cuts in the along direction stepping over in the across direction.

Across

Cuts in the across direction stepping over in the along direction.

Learn more