Contour Milling in CamDRAW: Centre, Inside and Outside

Contour milling follows the outline of a drawing object with the tool. It is the operation most jobs start with, and the one setting that matters most is which side of the line the tool runs on.

Open and closed curves are both supported: a freehand line as well as a rectangle.

Creating the operation

Select your drawing objects in CorelDRAW first. The operation is applied to whatever is selected when you create it.

In the Toolpaths section of the CamDRAW docker, the third of the four sections, click the first icon in the row of six. The contour machining window opens, and a preview of the toolpath appears on the CorelDRAW page. Every change you make updates the preview immediately.

Name and Tool

Name labels the operation in the list. Giving it something meaningful pays off on a job with a dozen operations.

Tool selects from the tool library. All stored tools appear in the dropdown. The icon to its right opens the tool list if you need to add or edit one. Selecting a tool brings its cutting data, feed rates and diameter into the operation automatically.

Contour adjustment

Tool center is the field that decides whether your part fits. Centre runs the tool along the line, so half the tool width is removed from each side. Inside or left keeps the tool inside the contour. Outside or right keeps it outside.

For a part you want to keep, cut outside. For a hole or pocket opening, cut inside. Cutting on the centre line makes a part smaller by exactly the tool diameter, which is the single most common reason a first attempt is scrapped.

Machining direction sets climb or conventional milling.

Both directions allows the toolpath to use both, which reduces travel on multi-pass work.

Show tool diameter draws the contour path with the thickness of the tool instead of as a thin line. It is a display aid, not a machining setting, and it makes it obvious at a glance how much material is being removed and where.

The collapsible sections

Four sections below are collapsed by default. Click a header to expand it.

Leads & Transitions adds entry and exit moves to the contour, linear or tangential, set separately from each other.

Sequence controls the machining order. Automatic optimises by shortest path. As on layer follows the order the objects sit in on the CorelDRAW layer, which gives you direct control.

Allowance offsets the contour by a set distance, for roughing and finishing passes.

Cutting data - Tool data shows the feed rates and spindle speed inherited from the selected tool, where they can be adjusted for this operation.

Machining parameters

Four Z values, and they are easier to keep straight if you picture them stacked from top to bottom.

Safety height is where rapid moves happen, clear above the workpiece and any clamps.

Plunge height is where the tool switches from rapid to the plunging feed rate. Set it just above the material.

Starting height is where machining begins. Usually zero, when the Z zero point is on the workpiece surface.

Final depth is the bottom of the cut. A negative value cuts into the material.

The depth per pass comes from the tool, not from this window. It is set as Cutting depth on the Cutting data tab of the tool list, and CamDRAW steps down to the final depth in increments of that size.

Curve precision

The last field. All curves are approximated by straight segments, and this value is the length of those segments. A larger value means longer segments and lower precision; a smaller value means shorter segments, higher precision and a longer program.

Fine lettering wants a small value. A large plaque outline does not.

Combined objects and text

Combined curves are handled by their intersections, so a shape made of several combined objects produces contours that follow the resulting outline rather than each original piece.

Text objects work like any other curve, with centre, inside and outside all available.

After clicking OK

The operation appears in the list in the Toolpaths section. Hovering over it shows its settings as a tooltip. Left-clicking highlights its toolpath in red on the page. Right-clicking opens Edit, Generate and Delete.

Use Generate after moving or editing the underlying drawing objects, to recalculate the toolpath against the new geometry.