When using the
Lace strategy the clean up stepover is limited to 20% to avoid leaving
behind pegs of material. www.kxcad.net Home > CAM Index > EdgeCAM Index >
Note that some of the options in this tab may be unavailable, depending on your licence.
Model Type - Select the type of geometry that makes up the shapes you are to machine, from the options 'Wireframe', 'Surface' and 'Solid'. If you are to machine features, select 'Solid'. (Note that 'Solid' is only available with a solid model open.)
Rest Rough - Check this box to apply a rest roughing cycle. When checked, the cycle uses the information from the previous roughing cycle. If no appropriate cycle precedes the rest rough cycle an error message will be displayed.
Note that some modifiers, such as Offset, become unavailable (greyed out) when you check Rest Rough. This is because they automatically use the value from the previous Roughing cycle (that is being rest-roughed).
Digitize Roughing - Allows you to select which of the previously created cycle toolpaths you want to base your rest roughing on.
Strategy - Select a roughing strategy. Choose between:
Concentric - Repeatedly follows the profile in a series of loops, each with a discrete offset. See an illustration.
Lace - Moves the tool in a series of straight lines. See an illustration. This is always followed by a final pass which follows the profile (which subject to the Minimum Radius setting).
Spiral - Repeatedly follows the profile with a smoothly changing offset.
See an illustration.
Note that in some circumstances the Spiral setting will be overridden and
a concentric toolpath produced. This may occur for large stepover values,
for example, where a spiral toolpath would leave pegs of uncut material
in corners.
Also note cycle time changes (as opposed to a concentric toolpath). Rectangular
shapes generally improve by the length of one link, while circular shapes
increase by a small factor.
Mill Type - The cutter can move along a profile on the left or right-hand side. This, combined with the spindle direction, gives the type of cutting to be either Climb or Conventional.
Climb - Tool cuts on the left of the profile (i.e. material is on the right).
Conventional - Tool cuts on right of the profile
Optimised - Cycle is optimised to reduce link moves. The tool may cut on the left or right side.
%Stepover - Specifies the tool stepover distance between each pass as a percentage of the tool diameter.
Offset - The distance between the final machined profile and the geometry that the cycle is based on. Bosses may be left slightly oversize, for example. This is a 3D offset, as shown in this illustration (which also shows Z Offset and XY Offset). This is unavailable with Rest Rough checked (when the value from the cycle being rest roughed is used). This is unavailable if an XY Offset value is set.
Z Offset - Specifies the Z offset for the cycle. See this illustration (which also shows Offset and XY Offset).
When set to a non-blank value, this acts as a limit on the Offset value's Z component, as shown in the illustration. You could set this to 0, which would limit the offset to being purely XY, but this would be different to making an actual XY Offset parameter setting; see this illustrated.
This is unavailable with Rest Rough checked (when the value from the cycle being rest roughed is used).
Please note that in 2D Roughing the Depth will be adjusted by the Z Offset (if specified). For example, Z Offset = 1, Depth = -20 and Cut Increment = 5 will produce cuts at -5, -10, -15, and -19.
XY Offset - An offset in the XY plane. See this illustration (which also shows Offset and Z Offset). This is unavailable if an Offset value is set.
Tolerance - Controls the accuracy to which the surface is machined. A small value results in a more accurate surface finish but takes longer to generate the toolpath. This is unavailable with Rest Rough checked (when the value from the cycle being rest roughed is used).
Lace Angle - (Only available if strategy is Lace) Specifies the angle between each pass and the X axis of the Initial CPL.
Minimum Radius - For the final pass, nearest the profile, a blend arc with this specified radius is inserted into toolpath internal corners (for non-final passes see 'High Speed Cornering' below). This helps maintain tool speed and reduce cutting forces. You can also use this setting to prevent the tool entering a channel where the cut would be full width and there is no room for a trochoidal path.
Cut by Region - Check this box to force the cycle to machine the profiles in regions. All levels within a region will be completed before the cycle moves to the next region. Otherwise all profiles on a level are machined before moving on to the next level.
High Speed Cornering - When checked a radius is introduced into sharp toolpath corners. This helps maintain toolspeed for example. When unchecked all toolpath corners have an angle from the profile, however sharp. This reduces the amount of CNC code. This setting only affects non-final passes; for the final pass see 'Minimum Radius' above.
Close Open Pockets - (Concentric strategy only) Allows you to specify how to machine open areas.
When unchecked, the tool will work from the outer edge inwards.
When checked, all open pockets will be treated as closed pockets and the tool will start in the middle and work outwards.
Clean Up % Stepover - Specifies
the stepover for the clean up pass (the outermost pass of each pocket)
as a percentage of the tool diameter. If this field is left blank the
main % Stepover will be used. Please note that the stepover for the clean
up pass cannot exceed the main stepover, if a larger value is entered
this will be clamped to the main stepover. When using the
Lace strategy the clean up stepover is limited to 20% to avoid leaving
behind pegs of material.
Stock
Stock Type - Allows you to define the stock volume for the roughing cycle. Choose between the following options:
None - With Stock Type set to None the Roughing cycle will only machine closed pockets. No digitised input required.
3D Model - You can digitise a solid model, surface(s) or an STL model to represent the stock volume. It is recommended that the entities representing the stock are placed on a separate layer for easy selection and show/hide. You will be prompted to digitise surfaces, solid or STL entities that represent the stock volume. This option is useful when a stock model is available which represents a casting, forging or pre-machined material that is not a simple offset of the finished part.
Thickness - The entities selected for machining are offset by the Stock Offset value and used as the stock definition. Note that this option can only be used when machining surfaces, solids or STL models. This feature is useful for casting and forging that form a constant wall thickness.
Bounding Box - A bounding box is a rectangular box that is placed around the extents of the 2D or 3D entities selected for machining. This box (not displayed) is used to define the stock envelope. This option is used when machining rectangular parts that contains pockets and/or open sided pockets.
Profile - Select a 2D geometric profile to represent the stock edge. When selecting this option, you will be prompted to digitise the stock profile. Digitised Input: Lines, arcs, continuous, boss or pocket feature that form a closed 2D boundary. This option can be used with any flat faced straight walled stock shape.
Stock Type is unavailable with Rest Rough checked (when the value from the cycle being rest roughed is used).
Stock Offset - Specifies a 3D
offset. This can optionally be applied to all Stock Types, but is required for the Thickness type.
Feed
Feedrate - Specifies the rate of movement in the workplane.
Plunge Feed - Specifies the rate of movement in the direction of the tool axis.
Speed - Specifies the tool spindle speed.