HPHV Feeds and Speeds

	A	B	C	D	E	F	G	H	I	J	K	L
1	HPHV Ferrous 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
7
8
9
10
11
12
13
14
15
16
17	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.
18
19	Tool Geometry and Information								Application Notes
20	Shop ID	Diameter, D=D1 (in)	Total Length, L (in)	Length of Cut, Ap1 max (in)	Flutes	Radius, Rε (in)	Catalog Number
21	These are preferred items that are kept in stock in the lab. Talk to staff to be issued one.
22	1/2" EM (F, GP)	0.5	2.5	1.25	4	0.015	HPHV500S4125R015
23	3/8" EM (F, GP)	0.375	2.5	0.875	4	0.015	HPHV375S4088R015
24	1/4" EM (F, GP)	0.25	2.5	0.5	4	0.015	HPHV250S4050R015
25	3/16" EM (F, GP)	0.188	2.5	0.3125	4	0.015	HPHV188S4031LR015
26	1/8" EM (F, GP)	0.125	2.5	0.25	4	0.015	HPHV125S4025LR015
27
28	Note: HPHV tools are for all-purpose steel machining. They are made of KC633M carbide, with a helix angle of 38 degrees, with unequal flute spacing.
29
30
31	Material Group		Engagement			Cutting Speed (SFM)		Feed per tooth for diameters (in)
32			Side Milling		Slotting	Cutting Speed (SFM)		Feed per tooth for diameters (in)
33			ap	ae	ap	Min	Max	0.125	0.1875	0.25	0.375	0.5
34	P	1	1.25xD	0.25xD	1xD	490	660	0.0009	0.0014	0.0018	0.0027	0.0035
35		2	1.25xD	0.25xD	1xD	460	620	0.0009	0.0014	0.0018	0.0027	0.0035
36		3	1.25xD	0.25xD	1xD	390	520	0.0007	0.0011	0.0015	0.0023	0.0029
37		4	1.25xD	0.25xD	0.75xD	300	490	0.0007	0.001	0.0014	0.002	0.0026
38		5	1.25xD	0.25xD	1xD	200	330	0.0006	0.0009	0.0012	0.0018	0.0023
39		6	1.25xD	0.25xD	0.75xD	160	250	0.0005	0.0008	0.001	0.0015	0.0019
40	M	1	1.25xD	0.25xD	1xD	260	330	0.0007	0.0011	0.0015	0.0023	0.0029
41		2	1.25xD	0.25xD	1xD	200	260	0.0006	0.0009	0.0012	0.0018	0.0023
42		3	1.25xD	0.25xD	1xD	200	260	0.0005	0.0008	0.001	0.0015	0.0019
43	K	1	1.25xD	0.25xD	1xD	390	520	0.0009	0.0014	0.0018	0.0027	0.0035
44		2	1.25xD	0.25xD	1xD	360	460	0.0007	0.0011	0.0015	0.0023	0.0029
45		3	1.25xD	0.25xD	1xD	330	430	0.0006	0.0009	0.0012	0.0018	0.0023
46	S	1	1.0xD	0.15xD	0.3xD	160	300	0.0007	0.0011	0.0015	0.0023	0.0029
47		2	1.25xD	0.25xD	1xD	160	260	0.0006	0.0009	0.0012	0.0018	0.0023
48		3	1.0xD	0.15xD	0.3xD	70	130	0.0004	0.0006	0.0008	0.0012	0.0016
49		4	1.25xD	0.25xD	1xD	150	210	0.0005	0.0008	0.0011	0.0017	0.0022
50	H	1	1.25xD	0.25xD	0.75xD	260	460	0.0007	0.001	0.0014	0.002	0.0026
51
52
53	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.
54
55	Definitions:
56	Catalog Number	This is the part number specified by the manufacturer, Kennametal. It can be looked up in the catalog for more information.
57	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.
58	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.
59	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.
60	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.
61	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.
62	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.
63	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.
64	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 * Diamter) / 12
65	Total Length, L	This is the length of the tool, measured from the back of the shank to the end of the cutting flutes.
66	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)
67	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)