Parallel Lace dialog - Control tab

www.kxcad.net Home > CAM Index > EdgeCAM Index >

Note that some of the options in this tab may be unavailable, depending on your licence.

Minimum/Maximum Contact Angle - At a point on a surface the contact angle is the angle between the normal to the surface and the tool axis (vertical). ('Surface' being used in the generic sense; includes surfaces within solid models.)

Only the regions where the contact angle is within the Minimum and Maximum values are machined.

You can specify angles between 0 and 90, except for Minimum Contact Angle which can only be up to 85. The defaults are 0 (min) and 90 (max). The minimum and maximum contact angles cannot be the same value, and they are automatically switched if you specify a Maximum value lower than the Minimum value.

If these settings break the toolpath into separate regions, the normal rules for leads, links and ordering are applied to each region and the move between the regions.

Exclude Flat Areas - This option allows you to optimise the Parallel Lace toolpath by excluding flat areas. These can be machined separately using the Flat Land Finishing cycle.

Ignore External Edges - When checked the toolpath will automatically ensure that any roll overs on the external edge of the part are removed by finishing the toolpath at the tangent point between the tool radius and the edge of the part before applying any lead moves.

 
Perpendicular Lace

The Perpendicular Lace option automatically re-machines the steep regions on the model that would normally leave a poorer finish compared to the rest of the model. This is achieved by using two Parallel Lace toolpaths to machine the part. The first toolpath machines the flatter areas, while the second Parallel Lace cycle is applied at 90 degrees to the primary cut direction.

Perpendicular Lace - Choose from the following options:

Off - Disables the Perpendicular Lace option.

Primary Bounded - The primary parallel lace toolpath is excluded from the steep regions leaving these areas to be cut only with the secondary, perpendicular toolpath.

Primary Unbounded - Uses the Perpendicular Lace option but allows the primary toolpath to machine the entire model first. The perpendicular toolpath then re-cuts the steep regions.

Contact Angle - Specifies the angle to control the extent of primary and secondary toolpaths.

Up-Down Mill

Strategy - You can choose whether you want the parallel lace stripes to be broken into portions to maintain Up Mill or Down Mill cutting, as the angle of the surface changes from horizontal.

Off - Normal stripes.

Down Mill - The stripe may be broken into portions of reversed toolpath direction, to maintain Down Mill cutting whatever the angle of the surface (along the direction of the stripe).

Up Mill - The stripe may be broken into portions of reversed toolpath direction, to maintain Up Mill cutting whatever the angle of the surface  (along the direction of the stripe).

Filter Angle - An angle you can specify to prevent undue breaking of the stripes at each slight undulation. For the surface to cause a break, it must be tilted at more than this angle from the horizontal, along the direction of the stripe.

Corners

Strategy - The tool normally rolls around any external corner and maintains contact. In some cases this causes the corner to be eroded, so EdgeCAM offers several corner control methods:

Round – Tool radius rollover that maintains tool contact with the corner.

Sharp – Replaces the rollover with a sharp corner. The toolpath extends past the corner until it intersects with the next section.

Twizzle - Replaces the round with a twizzle move.

High Speed - Replaces the rollover with a sharp corner. The toolpath extends past the corner until it intersects with the next section, where it is then blended with a radius of 75% of the tool radius to maintain toolpath tangency and will help the machine tool maintain its velocity.

Twizzle Radius - Specifies the radius of the twizzle move.

Check Surfaces

Use Check Surface - Allows you to digitize a surface or face feature that the toolpath must not cut (even if only as an accidental gouge resulting from the cutting of an adjacent face, for example). Note that if, as a check surface, you select a surface or face feature that is already selected for machining, then it will be treated as a check surface.

Check Offset - Allows you to control how much the toolpath stands off the check surfaces; it is a 3D offset applied to the check surfaces/faces.

Boundary Control