Use the Vortex page to create 3-axis toolpaths which machine at the specified cutting feed rate almost all of the time. This page contains the following:
Style — Choose how toolpath offsets are generated for the vortex toolpath:
- From model — Generates toolpath offsets from the outside inwards. This style is better suited for simple models, open spaces, and removing large amounts of bulk stock.
- From stock — Generates toolpath offsets from the inside outwards. This style is better suited for complex models and thin channels.
Cutting feed rate — Displays the Cutting feed rate specified on the Feeds and Speeds dialog.
The Cutting feed rate is critical for a tool to operate under optimum conditions. It depends on the combination of the tool and material properties. Use the feed rate that the tool manufacturer recommends, for side cutting (or profile cutting), as the minimum cutting feed rate. Testing shows these recommended values to be conservative when Vortex machining. This means, you can increase either the recommended feed rate or the recommended stepdown quite significantly.
For most toolpaths, entering a sharp internal corner increases the tool engagement angle and causes tool overload. To avoid this tool overload, you must reduce the feed rate. For Vortex toolpaths, there is no need to reduce the feed rate, because the tool changes to a trochoidal path when entering sharp internal corners, and avoids the overload situation.
Feeds and Speeds — Click to display the
Feeds and Speeds dialog which enables you to change the
Cutting feed rate.
Target radius (r) — Enter the radius of the arcs that the strategy uses, unless larger or smaller arcs are required. For example, accessing corners may produce arcs with a radius smaller than this value. As the feed rate increases, the recommended target radius increases. This prevents large accelerations on the tool, which can cause the machine to slow down.
Minimum point spacing — This is the minimum point spacing at which the machine tool can move at the specified feed rate. By default, PowerMill uses a value suitable for a typical machine tool at the specified feed rate. If the machine tool has too many points to process, it cannot sustain the specified feed rate.
Lift on return moves — When selected, raises the height of the back of the trochoids (the portion of the toolpath which is air-cutting). When deselected the whole trochoid is at the cutting level.
- Z distance (z) — Enter the lift height (the height above the cutting level).
Increase feed rate for non-cutting moves — Select to allow PowerMill to speed up non-cutting moves.
- Non-cutting feed rate — By default, PowerMill uses a non-cutting feed rate of 2*cutting feed rate, but you can enter a different value in the Non-cutting feed rate field.
If the machine tool exhibits any undesirable behaviour, such as jerking or vibrating, you can prevent this by:
- specifying a lower non-cutting feed rate;
- increasing the size of the target radius; or
- increasing minimum point spacing.
If PowerMill identifies any non-cutting moves that are too short for the machine tool to accelerate to the (faster) non-cutting feed rate and then decelerate back to the (slower) cutting feed rate, PowerMill completes these non-cutting moves at a percentage of the non-cutting feed rate.
Retract on non-cutting moves — Specify whether PowerMill replaces non-cutting moves, which exceed a certain length, with more time-efficient lift moves.
- Never — PowerMill keeps all non-cutting moves.
- Automatic — PowerMill replaces non-cutting moves that exceed an automatically-determined length with lift moves.
- Longer than — Enter the maximum length of non-cutting moves.
For more information see Vortex machining, Vortex and step cutting example, and Vortex machining of 2D features.