Cutting Data in CamDRAW: Feeds, Speeds and Path Spacing

The Cutting data tab of the tool library holds the numbers that decide how a tool actually behaves. They belong to the tool rather than to an operation, so setting them properly once means every operation using that tool inherits them.

To reach them, open the tool list from the Toolpaths section of the CamDRAW docker, select a tool on the left, and click the Cutting data tab.

Path spacing

The distance between neighbouring passes when clearing material, used by pocket machining and area engraving. It is expressed as a percentage of the tool diameter.

Keep it at or below 50 percent. Above that, the passes no longer overlap enough and uncut ridges are left standing between them. On a 6 mm cutter, 45 percent means the passes sit 2.7 mm apart.

Lower values give a cleaner surface and a longer program. On finishing work in soft material a smaller spacing is worth the time; on roughing it rarely is.

This value has no effect on contour operations, which follow a single line.

Cutting depth

The depth taken per pass, sometimes called the stepdown or increment.

The total depth of an operation comes from its Final depth field, and CamDRAW steps down to it in increments of this size. A final depth of 6 mm with a cutting depth of 1.5 mm gives four passes.

This is the field people look for in the operation window and do not find. It lives here, with the tool, because how deep a tool can cut per pass is a property of the tool and the material rather than of the job.

Engraving and cutting operations ignore it, since neither steps down.

The four feed rates

Normal feed rate is the standard feed for the tool, used for ordinary cutting moves.

Finishing feed rate applies to finishing passes, usually slower for a better surface.

Roughing feed rate applies to roughing, usually faster where surface quality does not matter yet.

Plunge feed rate governs movement in Z when entering the material. This is the one to get right: plunging at the cutting feed is how cutters break, because a flat-bottomed end mill is not designed to drill. As a starting point, a third to a half of the normal feed is common.

All four are in the document unit per minute, so millimetres per minute in a millimetre document.

Spindle speed

The rotational speed in revolutions per minute, written into the program for rotating tools. For a laser, plasma or waterjet tool it is not relevant.

Adjusting values for one operation only

Every operation window has a collapsible Cutting data - Tool data section showing the values inherited from the tool. Expanding it lets you change them for that operation alone, leaving the library entry untouched.

Use this for a one-off: a difficult material, an unusually deep pocket, a test cut. For anything you will do again, change the library instead.

What happens to existing operations

Changing a value in the library affects operations created afterwards. Operations that already exist keep the numbers they were given when they were made.

To bring an existing operation up to date, right-click it in the toolpath list, choose Edit, reselect the tool from the dropdown and confirm.

Where to get the numbers

Tool manufacturers publish recommended feeds and speeds for their cutters in common materials, and those are the right starting point. Adjust from there based on the sound of the cut and the finish, not on what a table says in isolation.

Save the numbers that work into the library as you find them. A tool library that reflects two years of real jobs is worth considerably more than one filled in from a catalogue on the first afternoon.

Remember to click Save at the bottom left of the tool window. Closing it or clicking Cancel discards the changes.