Machining Order: Automatic or As on Layer

The order in which contours are machined affects cycle time, and on sheet material it affects whether the parts are still where you left them. CamDRAW handles it at two levels: within an operation, and between operations.

Within an operation: the Sequence setting

Every contour-based operation has a collapsible Sequence section in its dialog. Click the header to expand it. Two options.

Automatic tool path optimization works out the order itself, sorting the individual contours by shortest path. Travel between cuts is minimised, which reduces the time the machine spends moving without cutting.

As on layer follows exactly the order the drawing objects sit in on the CorelDRAW layer. You control the sequence directly by controlling the stacking order of the objects.

Automatic is the right default. Use As on layer when the order matters for a reason the software cannot know.

When you need manual control

The usual case is parts coming loose. On a sheet where the outer contour is cut before the inner cutouts, the part is already free when the last cuts happen, so it can shift and the cut wanders.

The rule is inner features first, outer contour last. Automatic optimisation sorts by distance rather than by that rule, so on nested parts it is worth checking the result and switching to As on layer if it is wrong.

The other case is process order: engraving a plate before cutting it out, or drilling before pocketing so the drill has a flat surface to start on.

Controlling the order on the layer

With As on layer selected, the sequence comes from the CorelDRAW object stacking order.

Open the Object Manager or Objects docker in CorelDRAW to see the order, and use the arrange commands to move objects up and down within the layer. What is at the top of the stack is machined first.

This gives you exact control at the cost of managing it yourself, which is why it is not the default.

Between operations: the toolpath list

Operations run in the order they appear in the list in the Toolpaths section of the docker, from top to bottom.

Two small arrow buttons sit above the list, to the right of the toolpaths checkbox. Select an operation and use them to move it one position up or down.

This is the level at which you decide that the engraving happens before the cut-out, or that all the drilling is done before any pocketing starts.

Why it matters for tool changes

On a machine with an automatic tool changer, every switch between operations using different tools costs a tool change. Grouping operations that use the same tool together removes the unnecessary ones.

On a machine without a changer, the postprocessor writes a separate G-code file per tool, and the order within each file follows the same list.

Switching operations off without deleting them

Each operation in the list has its own checkbox. Unticking it excludes that operation from the generated program while keeping its settings.

This is useful for running a job in stages: switch on the engraving, generate and run it, then switch it off, switch on the cutting and generate again. The checkbox at the top of the list switches all operations on or off at once.

Checking the result

Generate the program with the G1 G2 button in the NC program section, then use the slider below the 3D view to step through it. Toolpaths are blue and rapid moves red, so the actual sequence is visible before the machine runs it.

The two arrows next to the slider step forward and backward one line at a time, which is the quickest way to check what happens at a specific point in the program.