Feeds and speeds - strategy

Feeds and speeds specifies the machine feeds and spindle speeds.

This displays the same options as the Cutting Conditions frame of the Feeds and Speeds dialog (Home tab > Setup panel > Feeds & Speeds).

This page contains the following:

Feeds and Speeds — Displays the Feeds and Speeds dialog where additional options such as the toolpath, tool, or material properties are available.

Load tool cutting data — Click to apply the values from the active tool's Cutting Data into this dialog.

Cutting Conditions — Enter the machine tool's cutting conditions.

Spindle Speed — Enter the rotation of the spindle, measured in revolutions per minute. If you edit this value then the Surface Speed value automatically updates to reflect your change.

The Spindle Speed is Surface Speed x 1000/3.14 x Tool diameter or, as a formula: n = Vc.1000/(.Dc). Editing either the Spindle Speed or Surface Speed automatically updates the other.

Cutting Feed Rate — Enter the cutting feed rate.

The Cutting Feed Rate is Number of teeth x Feed per tooth x Spindle Speed or, as a formula: Vf = Zn.fz.n. Editing either the Cutting Feed Rate or the Feed/Tooth automatically updates the other.

Plunging Feed Rate — Enter the speed of the tool when entering the material ready for its cutting moves. When 3-axis machining, these are vertical moves.

The Plunging Feed Rate is Cutting Feed Rate x Feed Rate Plunge Factor or, as a formula Vp = Fp.V. Define the Feed Rate Plunge Factor on the Tools > Feeds and Speeds page of the Options dialog available from the File tab > Options > Application Options.

Skim Feed Rate — Enter the skim feed rate for straight line moves from point A to point B. If everything is totally safe, the machine moves at rapid which usually appears as G0 in the output file. For skim moves, the machine performs a linear move (which G0 moves do not guarantee), normally G1 in the output file, at a high feed rate.

Coolant — Select the type of coolant.

• None — When selected, there is no coolant output.
• Standard — When selected, turns the coolant on.
• Flood — When selected, turns the coolant to flood.
• Mist — When selected, turns the coolant to mist.
• Tap — When selected, turns the coolant to tap.
• Air — When selected, turns the coolant to air blast.
• Through — When selected, turns the coolant to through spindle.
• Double — When selected, enables two coolant codes.

PowerMill turns the coolant off at the end of a toolpath.

You can apply coolant several different places. For more information see Coolant and how it updates/flows.

All of these fields are preceded by an icon (either or ).

• Calculated — When displayed, shows values calculated by PowerMill.
• Edited — When displayed, shows value entered by you (or another user). Click to change this value to the automatically calculated value.

Note: This value does not change when you activate a new tool.

Recommended — Displays the values specified in the Cutting Data tab of the Tool dialog.