www.kxcad.net Home > CAM Index > EdgeCAM Index >
Note that some of the options in this tab may be unavailable, depending on your licence.
Approach Type - Choose from:
Automatic - The cycle automatically applies an appropriate ramp method.
Pre-Drill - Specify a pre-defined drill point as the point of entry. The tool will plunge down the nearest hole to the start point in a region. When no valid point is available the tool will ramp instead. The tool will rapid down the hole to the desired depth unless it is within the safe distance of the pre-drill point where it will feed to depth from the safe distance above the point. If Feed When Plunging is checked the tool will feed down the hole at the Plunge Feedrate.
To ensure that a valid point is available, create a point
or a set of points that represent the XY position of the hole at full
diameter depth (see diagram).
Prior to using the Roughing cycle, drill the points you have created.
When choosing a tool for the drill cycle, we would recommend you select
the Full Diameter Depth Type option on the More tab of the tool change
dialog.
Helix - Helical approach to the pocket. The cycle will always attempt to place a helical approach in pocket areas before any other approach type.
Ramp - Ramp approach to the pocket. The cycle will always attempt to place a ramp approach in pocket areas before any other approach type.
If Maximum Plunge Depth
is set to 0 the tool cannot plunge or ramp. Therefore, the cycle can only
machine external areas or pocket areas that have pre-drilled holes.
Maximum Plunge Depth - Specifies the maximum distance in the Z-axis that the tool can plunge feed. The value will be used to check that the ramp move does not exceed this value. The maximum plunge is assumed to be equal to the Cut Increment when modifier is left blank.
Ramp Angle - Sets the angle of the ramp move into the stock material. The maximum ramp angle is calculated from the Maximum Plunge Depth and Centre Cut modifiers. This value will automatically be used if is found to be less than the specified Ramp Angle. If the modifier is left blank the calculated ramp angle will be used.
Centre Cutting Tool - Denotes whether a tool is capable of centre cutting, i.e. plunge cutting. This can affect the ramp moves. When this option is checked, the roughing cycle will allow the tool to plunge into position. When unchecked, and the tool cannot apply a ramp move the cycle will stop at that level.
Percentage Feed - The feedrate for approach moves is specified as a percentage of the feedrate on the General tab.
Links
Links are moves between the end of one cut increment and the start of the next. Links are also moves between 'regions'. For example where the tool has to jump over geometry (to enter a pocket within a boss for example), or where the profile has collapsed into loops.
Link Method - Choose from:
Always Ramp – There is a retract for the link move. (The height of the
retract is set by 'Type', below).
Here is an example where the profile has collapsed into loops:
Always Stay At Depth – The tool stays at the same depth; there is no
retract. (Note that this does not apply to links that clear geometry;
for these links there is always a retract, to avoid gouging.)
Continuing with the example above, this
may cause excessive full width cutting; as shown in red (overloading the
tool or increasing cycle time if 'adaptive feedrates' (see below) are
used):
Optimised – The fastest of the two methods above is automatically selected.
Type - When there is to be a retract for the link (see Link Method above), this setting controls the retract height. Choose between:
Optimised - For the link, the tool retracts to the previous cut increment height plus 'Safe Distance'. If needing to clear selected geometry (a boss or web for example) the tool retracts up successive cut increments until the geometry is cleared, plus 'Safe Distance'. If the cycle level is reached before the geometry is cleared, the tool will retract to the Clearance plane, as there are no further increment slices to check against.
Note that this setting only applies to moves within the same machined out volume (as in a pocket in a boss in a pocket). For links that move between two separate volumes (two separate pockets for example), the tool always retracts to the Clearance height.
These moves will be at the maximum feedrate specified in the code generator.
Clearance - For the link the tool always retracts to the Clearance height.
Note that the tool can only clear geometry that has been digitised for the cycle.
Safe Distance - Specifies the safe distance above the part from which the tool will feed into position at the end of link moves.
Cut Increment Stand Off - The height above the material (as left by the previous cut increment) at which to switch to feedrate and start ramping down to the next cut increment (that is following a 'clearance link', rather than a 'stay at depth' link - see 'Link Method' above).
Feed When Plunging - When checked, the tool will use the feedrate when moving down in the Z axis during the cycle. This is a safe option when the amount of stock material is unknown. When unchecked, the tool will rapid to the safe distance above the model then feed into position.
XY StandOff - This allows you to specify the distance between the stock and the tool when approaching from outside. Previously, a hard coded value of 1mm (or 0.03937 inches) was used.
Full Width Cut Moves
A full width cut move exceeds the specified % stepover. This potentially overloads the tool, so EdgeCAM detects when a cut would be full width and offers you this option:
Trochoidal - Apply a trochoidal path to the cut.
Feedrate
Adaptive - Adjusts the feedrate to even out loading on the tool. For example in a narrow channel the loading could be higher as the actual stepover increases above the specified Stepover value; in this case the feedrate would be reduced. Conversely for smaller cuts at less than the specified %Stepover, the feedrate would be increased to reduce machining times.
Note that the adjusted portions of the toolpath are indicated by a colour
change; a darker colour indicates a reduced feedrate.
Also note that the adjustment is only made to XY feeds; it is not applied
to any 'end cutting' plunge (ramp) moves.
Minimum Feedrate - This is the % of the original specified feedrate to be used in a full width cut (where the effective stepover = 100%). At intermediate effective stepovers, the feedrate is adjusted proportionally. For example, specify 10 for a specified feedrate of 100 to be reduced to 10 in a full width cut. If the specified %Stepover was 50, then in a 75% effective stepover cut, the feedrate would be reduced to 55. Specify a value of 1 or 99 or any number in between.
Maximum Feedreate - The % of the original specified feedrate to be used as the effective stepover reduces towards 0. For example, specify 300 for a specified feedrate of 100 to be increased towards 300 as the cut size reduces towards 0. If the specified %Stepover was 50, then in a 25% effective stepover cut, the feedrate would be increased to 200. Specify a value of 1 or 500 or any number in between.
Feedrate Increment - The feedrate can only be adjusted to certain values. This Feedrate Increment is the size of the steps between these values, as a percentage of the original feedrate.
Specifying low values helps produce tighter control over the feedrate, but with potentially more CNC code and slower processing. Specifying high values helps reduce the CNC code and speed processing, but with less accurate control over the feedrate.