Use the Vortex page to create toolpaths that machine at the specified cutting feed rate almost all of the time.
Cutting feed rate — By default, PartMaker uses the feed rate specified in the Cutting feed rate field in the Vortex page of the Surfacing Defaults dialog. However, you can enter a different value, if required.
The Cutting feed rate is a critical value to ensure the tool operates under optimum conditions. The feed rate depends on the tool and material combination. You should use the feed rate that the tool manufacturer recommends for side cutting (or profile cutting) as a minimum cutting feed rate. Testing has shown these recommended values to be conservative when Vortex machining. This means you can normally increase either the recommended feed rate or the recommended stepdown significantly.
For most toolpaths, entering a sharp internal corner increases the tool engagement angle and causes tool overload. To avoid tool overload, you have to reduce the feed rate. For Vortex toolpaths, there is no need to reduce the feed rate, as the tool changes to a trochoidal path when entering sharp internal corners, avoiding the overload situation.
PartMaker uses the feed rate to calculate the Minimum radius and Minimum point spacing values for a Vortex toolpath. Therefore, you should click Recalculate parameters if you change the feed rate so that PartMaker recalculates the Minimum radius and Minimum point spacing values based on the new feed rate.
Minimum radius (r) — This is the minimum radius used in the internal trochoids. PartMaker calculates a minimum radius value that is suitable for a typical machine tool at the feed rate specified in the Cutting feed rate field. As the feed rate increases, the minimum radius increases.
Minimum point spacing — This is the minimum point spacing at which the machine tool can move at the specified feed rate. If the machine tool has too many points to process, it cannot sustain the specified feed rate.
Lift on air moves — Select this option to raise 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.
- Distance (z) — Enter the lift height (the height above the cutting level).
Increase feed rate for non-cutting moves — Select to enable PartMaker to speed up non-cutting moves.
Non-cutting feed rate — By default, PartMaker 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 minimum radius; or
- increasing minimum point spacing.
Retract on non-cutting moves — Specify whether PartMaker replaces non-cutting moves, which exceed a certain length, with more time-efficient lift moves.
- Never — PartMaker keeps all non-cutting moves.
- Longer than — Enter the maximum length of non-cutting moves.