Drilling and Retraction Cycles in CamDRAW

The drilling operation places a hole at the centre of each selected drawing object. It is the quickest way to produce a set of holes, and it treats combined objects differently from every other operation, in a way that is worth knowing.

How drill points are placed

CamDRAW puts one hole at the centre of each drawing object, using the object's outer boundary to find that centre.

All object types work: open curves, closed curves, circles, rectangles, combined curves. The object does not have to be a circle. If you draw a square, the hole goes at its centre.

Creating the operation

Select the objects in CorelDRAW, then click the third icon in the row of six in the Toolpaths section of the CamDRAW docker.

The drilling window opens and the drill positions appear on the CorelDRAW page as small blue dots, so you can see exactly where the holes will go before confirming.

Combined curves behave differently here

In contour and pocket machining, combining objects merges them into one shape to be machined.

In drilling it does the opposite in effect: a drill point is created at the centre of each individual object within the combination, not one at the centre of the whole.

This is deliberate and useful. On a part with forty holes, selecting forty separate circles is tedious and easy to get wrong. Combine them once in CorelDRAW and they behave as a single object everywhere else, while drilling still produces forty separate points.

Machining parameters

The same four Z values as other operations.

Safety height for rapid moves above the workpiece and clamps.

Plunge height where the feed rate changes to the plunging rate.

Starting height where machining begins, usually zero when the Z zero is on the surface.

Final depth the bottom of the hole. Remember to allow for the point angle of the drill if the hole has to break through.

Feed rates and spindle speed come from the selected tool and can be adjusted in the Cutting data - Tool data section of the window.

The three retraction cycles

The Drilling cycle / return plane section offers three options. Which you want depends on the material and the depth.

No return drills the hole in a single pass with no retraction. Fastest, and appropriate for shallow holes in material that clears chips easily.

Return to plunge height retracts to the plunge height each time a new cutting plane is reached. This is the default, and the right answer for most work: it clears chips from the flute without wasting time on a full retract.

Return to the previous cutting plane retracts only to the last plane reached rather than all the way out. A compromise between the two, useful on deeper holes where a full retract each time costs noticeable time.

For deep holes in material that packs chips, such as acrylic or aluminium, the deeper retraction is what prevents a broken drill.

Selecting the right tool

The tool determines the hole diameter, so it has to be stored with the correct diameter in the tool library. Choose the drill from the Tool dropdown, or open the tool list with the icon beside it to add one.

After creating it

The operation appears in the Toolpaths list. Left-click it to highlight the drill points in red on the page. Right-click for Edit, Generate and Delete.

If you move or add objects afterwards, use Generate to recalculate the drill positions against the current drawing.