Ball Endmill Feeds and Speeds

	A	B	C	D	E	F	G	H	I	J
1	Ball Endmill Application Data
2
3	WARNING: Haas Minimills have a maximum spindle speed of 6000 RPM. Depending on the application, some of these tools may exceed that. If so, program a fixed spindle speed of 6000 rpm.
4
5	Diagram of tool geometry (courtesy of Kennametal)						Diagram of tool stepover and incremental depth
6	Diagram of tool geometry (courtesy of Kennametal)						Profiling		Slotting
7
8
9
10
11
12
13
14
15
16
17
18	Note: when slotting (when the full diameter of the tool is engaged), reduce XY and Z feed PT by 20% for chip and heat evacuation.
19
20	Tool Geometry and Information							Application Notes
21	Shop ID	Diameter, D=D1 (in)	Total Length, L (in)	Length of Cut, Ap1 max (in)	Flutes	Catalog Number
22	These are preferred items that are kept in stock in the lab. Talk to staff to be issued one.
23	1/2" BM	0.5	2.5	1	4	4BN0500IR100A
24	1/4" BM	0.25	2.5	0.75	4	4BN0250IR100A
25	1/8" BM	0.125	1.5	0.5	4	4BN0125IR100A
26
27	Note: All these tools are general purpose ball-endmills, used for engraving and 3d profiling. They are made of K633M carbide.
28
29	Material Groups		Engagement			Cutting Speed (SFM)		Feed per tooth for diameters (in)
30			Side Milling		Slotting	Cutting Speed (SFM)		Feed per tooth for diameters (in)
31			ap	ae	ap	Min	Max	0.125	0.25	0.5
32	P	0	1-1.5xD	0.1xD	0.5xD	500	650	0.0015	0.0031	0.0057
33		1	1-1.5xD	0.1xD	0.5xD	500	650	0.0015	0.0031	0.0057
34		2	1-1.5xD	0.1xD	0.5xD	460	620	0.0015	0.0031	0.0057
35		3	1-1.5xD	0.1xD	0.5xD	390	525	0.0012	0.0026	0.0049
36		4	1-1.5xD	0.1xD	0.5xD	300	490	0.0011	0.0023	0.0043
37		5	1-1.5xD	0.1xD	0.5xD	200	330	0.001	0.0021	0.0039
38		6	1-1.5xD	0.1xD	0.5xD	165	250	0.0008	0.0017	0.0032
39	M	1	1-1.5xD	0.1xD	0.5xD	295	380	0.0012	0.0026	0.0049
40		2	1-1.5xD	0.1xD	0.5xD	200	260	0.001	0.0021	0.0039
41		3	1-1.5xD	0.1xD	0.5xD	200	230	0.0008	0.0017	0.0032
42	K	1	1-1.5xD	0.1xD	0.5xD	390	490	0.0015	0.0031	0.0057
43		2	1-1.5xD	0.1xD	0.5xD	360	460	0.0012	0.0026	0.0049
44		3	1-1.5xD	0.1xD	0.5xD	360	425	0.001	0.0021	0.0039
45	N	1	1-1.5xD	0.1xD	0.5xD	1640	6560	0.0021	0.0042	0.0085
46		2	1-1.5xD	0.1xD	0.5xD	1640	4920	0.0017	0.0034	0.0068
47		3	1-1.5xD	0.1xD	0.5xD	1640	4920	0.0015	0.003	0.0059
48		4	1-1.5xD	0.1xD	0.5xD	1310	2460	0.0015	0.003	0.0059
49		5	1-1.5xD	0.1xD	0.5xD	820	3280	0.0019	0.0038	0.0076
50		6	1-1.5xD	0.1xD	0.5xD	330	2460	0.0021	0.0042	0.0085
51		7	1-1.5xD	0.1xD	0.5xD	330	2460	0.0021	0.0042	0.0085
52	S	1	1-1.5xD	0.1xD	0.5xD	330	2460	0.0012	0.0026	0.0049
53		2	1-1.5xD	0.1xD	0.5xD	165	295	0.0012	0.0026	0.0049
54		3	1-1.5xD	0.1xD	0.5xD	80	130	0.0006	0.0014	0.0026
55		4	1-1.5xD	0.1xD	0.5xD	165	195	0.0008	0.0018	0.0036
56	H	1	1-1.5xD	0.1xD	0.5xD	260	460	0.0011	0.0023	0.0043
57		2	1-1.5xD	0.1xD	0.5xD	230	390	0.0008	0.0017	0.0032
58		3	1-1.5xD	0.1xD	0.5xD	195	295	0.0006	0.0014	0.0026
59		4	1-1.5xD	0.1xD	0.5xD	165	230	0.0004	0.0009	0.0017
60
61	Usage Instructions: Identify the tool that you need, based on tool diameter and length of cut. Create the tool (type: bullnose end mill) using the geometry listed here. In the operation, set the speed (SFM) to the listed surface speed here. (WARNING: see note at top regarding Haas Minimills.) Look up the feeds, speeds, and engagement based on your material. On the strategy page, set the incremental depth and stepover to the values listed here. Please be warned that the application data here is intended as a reasonable starting point. It may need to be adjusted depending on the specifics of your application. For example, feedrate may need to be limited in deep cuts where chips can't get out of the cut, or increased if there is very little radial stepover.
62
63	Definitions:
64	Catalog Number	This is the part number specified by the manufacturer, Kennametal. It can be looked up in the catalog for more information.
65	Diameter, D=D1	This is the diameter of the cutting flutes. All of these endmills have the same sized shank as the flutes, that is, D=D1.
66	Flute	Flutes or teeth are a tool's cutting edges. Feed rate is specified in how much each flute can cut off, or feed per tooth. When setting up tools, make sure that the flutse are not clamped in the collet, as it will not hold it properly, and may damage the tool.
67	Incremental Depth, ap	This is the maximum amount of the tool that should be engaged vertically. For common tools, the tool diameter is a fairly good stepover.
68	Length of Cut, Ap1	The length of cut is the total length of the cutting flutes on the tool. This is the maximum amount that the tool can plunge into a cut. Do not exceed it, this will cause the shank of the tool to rub on the part.
69	Radius, Rε	This is the corner radius on the ends of the flutes, which helps to prevent chipping. This will cause there to be a round in the bottom corner of cuts, which may need to be removed with a finish pass using a different tool.
70	Shank	The shank of a tool is the round, non-fluted part that the tool is held by. Take care not to engage it on the part, for example, by plunging too far in. When setting up tools, as much of the shank should be clamped as possible.
71	Stepover, ae	This is the maximum amount of the tool that should be engaged horizontally, in the XY plane. The exception to this is when cutting a slot the width of the cutter. In this case, the feedrate should be reduced.
72	Surface Speed, sfm	This is the maximum speed that the surface of the tool should contact the part at. The rotational speed can be calculated with the formula SFM = (RPM * π * Diameter) / 12
73	Total Length, L	This is the length of the tool, measured from the back of the shank to the end of the cutting flutes.
74	XY Feed Per Tooth	This is the amount that each tooth on the tool should cut each rotation while moving in XY (horizontally.) Feed speed can be calculated with the formula Feed = (RPM * PT * Flutes)
75	Z Feed Per Tooth	This is the amount that each tooth on the tool should cut each rotation while moving in Z (vertically.) It should be roughly 1/5 of the XY feedrate. Feed speed can be calculated with the formula Feed = (RPM * PT * Flutes)