www.kxcad.net Home > CAM Index > EdgeCAM Index >
|
Coord Input |
Only appears on re-opening the dialog to edit. Check this to re-specify (digitise) the cycle's geometry, such as the Drive and Check surfaces. You need to check this if your edits require new geometry selection, such as digitising a new curve if you change to the 'Parallel to Curve' cutting strategy. |
|
|
Strategy |
Choose from: |
|
|
|
Parallel Slice |
The cuts are where a series of parallel planes intersect the drive surface. The Cut Distance sets the distance between the planes. The 'Angle In XY' and 'Angle From Z' (see below) sets the orientation of the planes. |
|
|
Normal to Curve |
The cuts are normal to a curve you specify. See an example where the curve is one of the trim curves of the surface... |
|
|
Blend between Two Curves |
Cuts blend between two curves you specify. See an example where the curves are the trim curves of the surface... |
|
|
Parallel to Curve |
Cuts are parallel to a specified curve. This is suitable for SWARF cutting, where the tool is 90° to surface. |
|
|
Project onto Curve |
Projects a curve onto a surface and generates a cut along the intersection. Note that the curve needs to run quite closely along the surface. |
|
|
Blend between Two Surfaces |
Cuts blend between curves where two surfaces you specify intersect the drive surface. See an example where the blend surfaces are the 'sidewall' surfaces... |
|
|
Parallel to Surface |
The cuts are parallel to a specified surface. |
|
Mill Type |
Choose from: |
|
|
|
Clockwise |
The tool travels in a clockwise direction round the cuts, looking down the Z axis of the initial CPL. |
|
|
Anti-Clockwise |
The tool travels in an anti-clockwise direction round the cuts, looking down the Z axis of the initial CPL. |
|
|
Climb |
For a clockwise rotating spindle, the material is on the right-hand side of the tool, in the direction of travel. |
|
|
Conventional |
For a clockwise rotating spindle, the material is on the left-hand side of the tool, in the direction of travel. |
|
|
Optimised |
Cycle is optimised to reduce
link moves. Milling may by Climb or Conventional |
|
Cutting Range |
Choose from: |
|
|
|
Standard Cuts |
The distance between cuts is solely determined by the 'Cut Distance' setting. Cuts may not coincide with the drive surface edges. |
|
|
Exact Surface |
The distance between cuts, as determined by the 'Cut Distance' setting may be adjusted so that there are cuts along the drive surface edges. |
|
|
Number of cuts |
As for 'Standard Cuts', except that cutting stops after the 'Number of cuts' value (see below) is reached. |
|
|
Limit cuts |
There are only cuts between two points you digitise. |
|
Start Margin |
Reduces the area that will be machined. There will be a protected area of this specified width around the edges of the 'normal' area (that would be machined if this value was 0). For the 'Blend between Two Curves' and 'Blend between Two Surfaces' Strategy settings (see above), this is the margin for the 'First Curve/Surface'. Note that only the centre of the tool is excluded from the margin, so you might want to specify a value that allows for the radius of the tool. This is not available for all 'Strategy' settings; it is unavailable for the 'Parallel Slice' strategy, for example. |
|
|
End Margin |
As for 'Start Margin' above, except that for the 'Blend between Two Curves' and 'Blend between Two Surfaces' Strategy setting, this is the margin for the 'Second Curve/Surface'. |
|
|
Angle In XY |
Sets the orientation of the slices for the 'Parallel Slice' strategy - see above. |
|
|
Angle From Z |
Sets the orientation of the slices for the 'Parallel Slice' strategy - see above. |
|
|
Number Of Cuts |
Used when 'Cutting Range' is set to 'Number of Cuts' - see above. |
|
|
Reverse Cuts |
Reverses the start and end points of the cutting pattern. When checked for example, the cycle might finish at your specified 'Start Point'. |
|
|
Cut Order |
Choose from: |
|
|
|
Standard |
The tool works across the surface from one edge to the other. |
|
|
In to Out |
Tool starts in middle of surface and moves outwards. |
|
|
Out to In |
Tool starts at outer edges of surface and moves inwards. |
|
Enforce Closed Contour |
Makes toolpaths form complete loops. See an example.... |
|
|
Start Position |
When checked you are prompted to digitise a point, and the cycle starts as close to this as possible. |
|
|
Helical |
When checked the toolpath consists of one continuous spiral, rather than a series of individual cuts. See an example.... The toolpath would initially need to consist of nested loops; for example as produced by a 'Parallel to Curve' Strategy following a closed loop curve. |
|
|
Rotate Start Point |
An offset angle for the start of each cut, relative to the last cut. See an example... |
|
|
Tool Contact Point |
The tool is moved normal to its axis to change the contact point with the surface, according to your choice from: |
|
|
|
Automatic |
The contact point on the tool is allowed to move so that the tool does not gouge.
|
|
|
Centre |
The centre of the tool end contacts the surface. Note that gouging by the tool edges is possible, so you might need to make settings in the 'Check' tab. See an illustration (note the gouging in the 'concave section')... |
|
|
Flat Radius |
As for 'Automatic' above, except that only the radius edge of the tool can be in contact (see the green area in this illustration), not the flat end portion. To achieve this the tilt of the tool may be adjusted from that determined by the 'Tilt Strategy'. |
|
|
Front Edge |
The tool axis tilt is adjusted just sufficiently so that the edge of the end flat section that is leading in the cut direction contacts the surface. Note that gouging by the tool edges is possible, so you might need to make settings in the 'Check' tab. |
|
|
User Defined |
As for Centre, except that you can shift the contact point from the centre of the tool end. You can shift the tool by the 'Front Shift' value in the direction of the cut, and by the 'Side Shift' value in a direction normal to the cut. See an illustration (showing Front Shift, Side Shift is 'in and out' of the screen)... |
|
Front Shift |
The distance between the centre of the tool's end face and the contact point, measured in the direction of the cut. |
|
|
Side Shift |
The distance between the
centre of the tool's end face and the contact point, measured in a direction
normal to the direction of the cut. |
|
|
Round Corners |
Use this setting to remove 'fishtails'. Fishtails are extra sharp corners that are introduced into the toolpath as the tool rounds a corner, and switches from the surface at one arm of the corner to the surface at the other arm. The Round Corner value is a radius value at which to trim back the toolpath from the surface corner. This leaves a gap, which is then treated according to the 'Gap Link' settings in the Links tab. You might want to leave a blank setting to disable fishtail removal:
|
|
|
Offset |
A 3D offset for the toolpath from the surface. Leaves machined parts oversize in relation to their design geometry, for example. See an illustration... |
| |
|---|---|---|---|
|
Tolerance |
Controls the accuracy of the fit between the geometry (surfaces) and toolpath. Choose small values (more points are inserted into the toolpath) for a more accurate finish at the expense of longer processing times. |
| |
|
Maximum Point Separation |
In areas of less curvature the toolpath will contain fewer points. More points are inserted where necessary (in flatter regions for example) to bring down the distance between points to this maximum setting. See also Maximum Angle Change (in the Tool Axis Control tab). |
| |
|
Cut Distance |
The distance between cuts. |
| |
