Use the Feeds and Speeds dialog to specify the machine feeds and spindle speeds of the machine tool. You can use the Feeds and Speeds dialog to make changes to the Surface Speed and Feed/Tooth values of an active, and calculated, toolpath without recalculating it.
Click Home tab > Setup panel > Feeds & Speeds to display the Feeds and Speeds dialog.
The Feeds and Speeds dialog contains the following settings:
Toolpath — Displays the name of the active toolpath whose feeds and speeds are described.
Stock material — Displays the stock material specified by the tool.
Tool — This is the same as the Name on the Tip tab of the Tool dialog.
Type — Select the type of toolpath cut with this tool. This selection loads the tool cutting data specified in the Cutting Data tab of the active tool. It also outputs a record to the cut file for the postprocessor, where you can use it for example, to select different smoothing tolerances on the CNC.
Operation — Select the cutting mode of the tool. This enables you to set the tool/material properties for different toolpath operations.
This is not a parameter, and so it does not set the actual toolpath operation. It loads the tool cutting data specified in the Cutting Data tab of the active tool.
Cutting data table — Displays the cutting data values specified in the active tool's Edit cutting data dialog.
— Click to open the Tool dialog for the active tool.
— Click to apply the values from the active tool's Cutting Data into this dialog.
Coolant — Select the type of coolant.
- None — There is no coolant output.
- Standard — Turns the coolant on.
- Flood — Turns the coolant to flood.
- Mist — Turns the coolant to mist.
- Tap — Turns the coolant to tap.
- Air — Turns the coolant to air blast.
- Through — Turns the coolant to through spindle.
-
Double — Enables two coolant codes.
PowerMill turns the coolant off at the end of a toolpath.
For more information see Coolant and how it updates/flows.
Overhang Compensation — Select to reduce the depth of cut when extensions are fitted. The distance a tool projects out of the tool holder can have a huge impact on tool life, especially for solid carbide cutters. Excessive overhang increases both tool deflection and vibration, both of which increase the rate of wear. Most tool manufacturers make specific recommendations similar to ap' = ap * (4Dc/len)2, where:
- ap' is the revised depth of cut
- ap is the depth of cut
- Dc is the cutting diameter
- len is the overhang
Typically, this correction is not made for indexable insert cutters since the length is predetermined by the holder construction. However, if you fit extensions, some kind of reduction should be made.
Tool/Material Properties — Enter the cutting conditions of the tool and material.
Surface Speed — Enter the speed of the tool during material removal. The surface speed represents the rate at which the cutting edges of the tool can be driven through the material. Any changes made to the Surface Speed value recalculates the Spindle Speed, Cutting Feed Rate, and Plunging Feed Rate. In calculations, this value is represented by the symbol vc.
Feed/Tooth — Enter the cutting feed per tooth. The feed per tooth is determined by the construction of the tool, and may be limited by the strength of the cutting edges or the capacity of the tool to remove swarf.. Any changes made to the Feed/Tooth value recalculates the Cutting Feed Rate and Plunging Feed Rate. In calculations, this value is represented by the symbol fz.
If only one flute is specified for the tool, then Feed/Tooth is the same as Feed/Rev.
Axial Depth of Cut — Enter the depth of cut measured along the tool axis. Typically, this value determines the maximum Stepdown for area clearance and constant Z machining. The flute length of a solid cutter or the inserts fitted limit the maximum value. In calculations, this value is represented by the symbol ap
Radial Depth of Cut — Enter the depth of cut measured normal to the tool axis. Typically, this value determines the Stepover for machining. In calculations, this value is represented by the symbol ae.
Working Diameter — When selected, PowerMill corrects for the effective tool diameter. These options enable you to make corrections for the working diameter of the tool. For example, when surface milling with anything other than a square-ended cutter with a small depth of cut, the full diameter of the cutter is never engaged in the material. If the spindle speed is calculated using the tool diameter, the surface speed of the part of the tool in the cut is less than it should be.
Depth of Cut — Enter the depth of cut. PowerMill uses this value in the surface speed calculations ap.
Surface Slope — Enter the inclination from the horizontal of the surface being machined. The inclination of the surface being machined has an influence on the effective tool diameter. PowerMill uses this value in the surface speed calculations.
Cutting Conditions — Enter the machine tool's cutting conditions.
Spindle Speed — Enter the rotation of the spindle, measured in revolutions per minute. The Spindle Speed is Surface Speed x 1000/3.14 x Tool diameter or, as a formula: n = Vc.1000/(
.Dc).
Editing the Spindle Speed or Surface Speed values automatically updates the other value to reflect your change.
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 the Cutting Feed Rate or the Feed/Tooth values automatically updates the other value to reflect your change..
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 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.
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.
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.
Apply — Click to apply the values in this dialog to the active toolpath. This button is unavailable unless the feed rates in the dialog are different from the active toolpath feed rates, so it is apparent when the feed rates need to be applied to the toolpath.
Close — Click to close the dialog without updating the feed rates.
For more information see using the feeds and speeds dialog.
To use the feed rates and coolant settings assigned to the tool, click File tab > Options > Application Options > Tools > Feeds and Speeds > Auto Load Feed Rate.