Pocket Rough Milling Options
Rough milling provides the following options:
• Requested Percent Milled: percent of the total pocket volume milled by the current occurrence of the roughing operation. Roughing on a given pocket has either one or two ccurrences, depending on whether one or two tool diameters were selected for the pocket. When two diameters are chosen, there are two occurrences of roughing. In this case, part of the pocket’s total volume is removed by the first occurrence, and the rest is removed by the second occurrence.
By default, the volume removed by the first operation occurrence is determined by linear interpolation—see
Chipmaking Time for Pocket Rough Milling. The volume removed by the second occurrence, by default, is the difference between the total pocket volume and the volume removed by the first occurrence.
You can override the default with this setup option.
• Material Removal Rate: rate at which material is removed during chipmaking. By default this is based on feed, speed, engagment width, and cut depth (see
Chipmaking Time for Pocket Rough Milling). Use this option to override the default.
• Tool Diameter: diameter of the selected tool. Larger diameters can decrease engagement time—see
Chipmaking Time for Pocket Rough Milling--and have a more favorable length-to-diameter ratio. Smaller diameters have better corner accessibility.
Diameter selection picks either one or two diameters for roughing a given pocket. If two diameters are chosen, two occurences of the Rough Milling operation are associated with the pocket. The first occurrence uses the larger diameter to remove most of the pocket’s volume, and the second occurrence uses the smaller diameter to remove the remaining volume.
By default, larger diameter is chosen to allow access to most of the part’s volume, and the smaller diameter is chosen to allow the tool to fit into the pocket’s corners. See
Diameter Selection for Pocket Roughing for detailed information.
With this setup option, users can override default diameter selection for a particular occurrence of the Rough Milling operation.
• Tool Cutting Speed: how fast the tool turns in unit distance per unit time; that is, the speed at which a point on the outer edge of the tool moves along the circular path around the center of the tool. This value is used (along with feed, tool diameter, cut depth, and cut width) to determine volume removal rate. See
Tool Axis Speed and
Chipmaking Time for Pocket Rough Milling for more information on how speed contributes to cutting time.
Select one of the following options:
o Use Recommended Tool Cutting Speed: aPriori determines this value by interpolation from data tables based on tool series, tool type, tool diameter, and material cut code--see
Tool Selection. This value is adjusted to compensate for various factors, including machine spindle speed limitations and stock hardness. The value is also adjusted by multiplying by the cost model variable
millSpeedAdjustment. The adjusted value is used to help determine volume removal rate.
o Override Tool Cutting Speed: enter a speed in meters per minute. This value is adjusted to compensate for various factors, including machine spindle speed limitations and stock hardness. The value is also adjusted by multiplying by the cost model variable
millSpeedAdjustment, and a factor associated with the setup option
Rough Milling Aggression Adjustment Dial (see
User Inputs for Machining). The adjusted value is used to help determine volume removal rate.
• Requested Feed per Tooth: distance the tool travels along the surface of the part per tooth of the tool during one rotation. The number of tool teeth times this value is the distance the tool travels along the surface of the part per rotation of the tool. This value is used (along with speed, tool diameter cut width, and cut depth) to determine volume removal rate. See
Tool Axis Speed and
Chipmaking Time for Pocket Rough Milling for more information on how feed contributes to cutting time.
Select one of the following options:
o Use Computed Feed per Tooth: aPriori determines this value by interpolation from data tables based on tool series, tool diameter, and material cut code—see
Tool Selection. aPriori multiplies this value by the number of teeth to derive tool feed. This value is adjusted to compensate for various factors, including tool reach and required tolerance. Tool feed is also adjusted by multiplying by the cost model variable
millFeedAdjustment. The adjusted value is used to help determine volume removal rate.
o User Override: enter a value in millimeters. aPriori multiplies this value by the number of teeth to derive tool feed. This value is adjusted to compensate for various factors, including tool reach and required tolerance. Tool feed is also adjusted by multiplying by the cost model variable millFeedAdjustment. The adjusted value is used to help determine volume removal rate.
• Number of Teeth: number of tool teeth. This value together with feed per tooth determines feed (which affects volume removal rate)—see
Tool Axis Speed and
Chipmaking Time for Pocket Rough Milling.
Select one of the following options:
o Number of teeth: aPriori determines this value by interpolation from data tables based on tool series, tool diameter, and material cut code—see
Tool Selection. aPriori multiplies this value by the feed per tooth to derive tool feed. This value is adjusted to compensate for various factors, including tool reach and required tolerance. Tool feed is also adjusted by multiplying by the cost model variable
millFeedAdjustment. The adjusted value is used to help determine volume removal rate.
o User Override: enter a value greater than or equal to 2.
If you supply a user override for both Number of Teeth and Requested Feed per Tooth, aPriori multiplies the two values together to derive tool feed.
If you supply a user override for Number of Teeth, and you do not specify a user override for Requested Feed per Tooth, aPriori sets the unadjusted value for feed as follows:
Feed = Interpolated Feed * (Specified Number of Teeth / Interpolated Number of Teeth)
(Interpolated feed and interpolated number of teeth are derived from data tables during tool selection—see
Tool Selection.)
In either case, the value is adjusted to compensate for various factors, including tool reach and required tolerance. Tool feed is also adjusted by multiplying by the cost model variable millFeedAdjustment. The adjusted value is used to help determine volume removal rate.
• Radial Cut Depth: engagement length, either in millimeters or as a percentage of the tool diameter. This is the length along the tool radius of the area of contact between the part and the tool during chipmaking. Radial cut depth helps determine contact area and cut time. See
Chipmaking Time for Surface Rough Milling.
By default, radial cut depth is half the tool diameter.
Users can override the default with this setup option, by doing one of the following:
o Specify the radial cut depth in millimeters.
o Specify the radial cut depth as a percentage of the tool diameter.
• Axial Cut Depth: cut depth as a percentage of the tool diameter. This is the length along the tool axis of the area of contact between the part and the tool during chipmaking. Axial cut depth helps determine contact area and cut time. See
Chipmaking Time for Surface Rough Milling.
By default, axial cut depth is half the tool diameter. This value is adjusted based on machine power, and limited by the tool’s maximum cutting depth and by pocket depth.
Users can override the default with this setup option, by doing one of the following:
o Specify the axial cut depth in millimeters.
o Specify the axial cut depth as a percentage of the tool diameter.
• Tool Type: either Flat End Mill or Ball End Mill. By default, ball end mills are chosen for the smaller (or only) tool when the pocket has one or more of the following:
o Matching wall and bottom fillet diameters
o Non-planar floor
o Walls that form an acute angle with the floor
Users can override the default with this setup option.