The majority of model engineers using the lathe for milling will accept the tooth angles found on the cutter “as bought”, and as most which are stocked by tool dealers will be “general purpose” cutters there is little need to worry about them – though some care may have to be exercised when dealing with “surplus” tools, some of which may be specials, However, some knowledge of the necessary rakes and clearances is of value, both in diagnosing faults if anything goes wrong and when making cutters. Those who own a cutter-grinder will usually find setting details for the various types of tooth in the handbook.
Fig. 1 shows the nomenclature used – the rakes etc have been somewhat exaggerated for clarity. It will be realized that a straight flute cutter with side teeth (such as an endmill or a side-and-face cutter) can have no axial rake, but a helical flute cutter cannot avoid rake. In cases where the helix angle is such that the rake is excessive it is necessary to stone the edge of each tooth to reduce it – just as we do to a drill when taking heavy cuts in brass. Those who read the engineering press, or who fall into conversation with production engineers, may be forgiven if they wonder about the merits of “negative rake” (Fig. 2).As such it has little virtue; its merit is that the cutting angle, shown in Fig. 42, is increased and the tooth point is stronger. It is almost imperative when cutting hard materials with tungsten carbide tools, as the tool material is very brittle, but not elsewhere. The power consumption goes up markedly, so that there is no point in even trying negative rake on a milling cutter used in the lathe!
The clearance angle is important. It will be appreciated that the action of a milling toot h is similar to that of a boring tool, except that the cut is entirely on the cylindrical face and not on the side. This means that the smaller the cutter the more important the peripheral clearance becomes.True,small cutters have smaller lands on the teeth, but equally, the amount of wear needed to eliminate the clearance is small also. When making flycutters and especially f lat form cutters it is very important to keep this in mind.
The “blunting” of endmills and side and-face cutters is always characterized by complete loss of clearance on the corner of the tooth, causing rubbing and overheating at this vulnerable point. Reference has already been made to the desirability of stoning a small chamfer, or even a radius.at this corner when the tool is used for facing duties. The chamfer or radius will automatically acquire a cutting rake, but the need for clearance must not be forgotten.
At first sight it might be assumed that the teeth on the end of an endmill will not cut at all, if all the metal removal is done by the teeth on the cylinder, and the same would appear to apply to slot drills except when plunging, and to side-and-face cutters. This is true to some extent. but these end or facing teeth do have the job of removing the machining marks which would otherwise appear. If blunt they will trap tiny pieces of swarf and do more harm than good,the swarf cutting circular tears on the machined face. This being so the end teeth are often retouched with an oilstone; when this is done care must be taken to preserve the correct clearance – or at least. as near as possible.
Recommended angles can be found in the table opposite. There is quite a range for each material; the “middle of the range” will serve for most purposes. In genera l power w ill be saved if the larger rakes are used on materials which would produce a curly chip when machining. but for “grabby” metals like brass the less rake the better as the milling process tends to “drag up” the clearance in slide feed screw nuts. For really tough material the minimum of both rake and clearance should be used. Slitting saws have zero rake as a rule.
The axial rake is. of course. preset by the helix angle on helical tooth cutters – it can be reduced by stoning or grinding, but cannot be increased. On the other hand, axial rake on straight-flute cutters is fixed at zero.
|Material||Radial Rake degrees||Axial Rake degrees||Clearance degrees (see note)|
|Cast Iron (Grey)||5-10||5-10||4-7|
|Cast Iron (Hard)||3-5||3-5||4-7|
|F.C. Mild Steel||8-12||8-12||3-5|
|B.D. Mild Steel||6-12||6-12||3-5|
1. For general purposes, clearance angles should range from 4-5° for cutters 21-in.dia to 13° for 1/8 india.
2.The tabled clearances should be applied only to a “land” about 1/64-1/32 in. wide; behind this a further clearance of about 5° more should be ground.
To conclude this section. an important point must be emphasised. Owing to the peculiar action of the cutter the rate of feed will reduce the effective clearance angle when facing, or when cutting slots with a slot-drill. If the “land” is wide and the clearance angle small actual Interference can result. THIS IS THE MOST COMMON CAUSE OF BREAKAGE OF SMALL ENDMILLS AND SLOT DRILLS, and cutters which appear to be blunt may well be suffering from overdriving.
CUTTING SPEEDS AND FEEDS. Two factors are Involved. First, the power available to “shift metal”, and, second, the acceptable rate of wear of cutting edge. In both cases the data published in “Production Engineering” tables and “Engineering Yearbooks” can be misleading to the model engineer. On the first point, any milling machine with 3 HP available would be regarded as “tiny” in a production workshop. We have, as a rule,about half a horsepower available and a lot of that is lost in the belt drive. Our machine is far less rigid, too. The best we can hope for is the removal of perhaps one quarter to one third of a cubic inch of steel or cast iron per minute on a 31-inch lathe. The amount we can remove when TURNING is not relevant – milling is a different kettle of fish.
On the second point, cutting speeds in industry are geared to an economic overall cost of production. It pays to drive cutters hard and to regrind often. Few model engineers have cutter-grinders, and we must treat our tools accordingly, AND bear in mind that we are using a lathe and not a milling machine. A blunt turning tool can soon be remedied, but an endmill cannot.
CUTTING SPEED. For HSS endmills the following cutting speeds can be used as a basis, but see also the note at the end of “Feed Rate” Section.
- Cast Steel, Malleable Iron, Monel, Stainless steel …… 35ft/min.
- Cast Iron, Bronze,Drawn MS. Gunmetal ……………….. 60ft/min.
- Cast Iron, Bronze,Drawn MS. Gunmetal ……………….. 60ft/min.
- Cast Iron, Bronze,Drawn MS. Gunmetal ……………….. 60ft/min.
Slot-drills can be run perhaps 10% faster. Side-and-face cutters can be run at the above speeds if the mandrel or arbor is stiff enough to avoid chatter. Single point flycutters can be treated as boring tools. but again the stiffness of the tool (and work) must be taken into account. Subject to what follows the rule should be to reduce speed if in any doubt.
Finishing cuts. For small cutters. 1/Bin. diameter and below, the above speeds when translated into RPM may well be beyond the capacity of the machine – you must then run as fast as possible. Cutting speed may be found by writing
FEED RATE. Milling practice is to use a figure known as “Tooth load”. This is the feed per revolution per tooth, so that the feed in ins/min is the product of speed in RPM, number of teeth, and tooth load. Tooth load varies very little from one material to another. but it does go down rapidly as the cutters get smaller. (We are not. of course,concerned with “Industrial” cutters,which can be 6 inches to a foot or more in diameter !) The chart. Fig. 3 . plots a “Tooth load Factor” against cutter diameter for those between 1/16 inch and 1 inch diameter. This is for HSS endmills working at the depth of cut shown in this figure (Fig. 15 Design (maximum) cutting conditions for an endmill) For slot-drills – again working full depth – the factor may be increased by 50% (but remember that they have only two teeth). When used on a very light cut. as for surfacing,the rates may be doubled, provided that this gives an acceptable finish.
The factor “F” is practically constan t for all materials in the sizes we normally use – the actual feed rate will depend on the number of flutes and the RPM,as well as “F”.
Feed Rate = “F” x Cutter Dia(lns) x RPM x No. of Flutes = (inches/minute)
The feed rate thus depends on the CUTTING SPEED, and this varies according to material being cut, as mentioned above. It is always tempting to reduce the feed rate if the cutter exhibits distress. but though a slight reduction does no harm this is, in general, a mistake. The depth of cut should be reduced and the feed rate maintained. With very small cutters the “tooth load” is very small indeed and you w ill recall from Fig. 1 here that tho out seen by the tooth starts at a very low figure. Very slow feed rates cause the tooth to rub at the beginning of the cut, and t his causes poor finish.
The comments so far refer to the “normal” situation of the model engineer, who has no facilities for proper cutter grinding ,and who is more concerned with tool life than with rate of metal removal. However,if you have a “Quorn” or similar, and care to spend time resharpening every now and then,you can work faster. I show in Appendix I the recommended INDUSTRIAL speeds and feeds, and subject to the rigidity of your setup you can approach these. You will note. however, that the TOOTH LOAD is nearly as above – the difference is in the increased cutting speed.
DEPTHS OF CUT..The rule here is simple: the depth of cut should be as large as the available power will permit up to the limit prescribed for the type of cutter. (And. of course, the amount of metal you wish to remove! To refresh your memory I show in Fig. 4 the design cutting depths for endmills, slot drills, and “Rippa” cutters. These may look formidable to those not accustomed to milling, but it will be realized that the thickness of the chip is unaffected by the depth “D” – it depends only on the feed rate. A full depth cut produces a long, but thin, chip. For the average 3 inch lathe in good condition a rough estimate of the size of cut can be made by multiplying feed rate in inches per minute by the depth and width, “D” and “W”; if the proposed cut works out at much above one third of a cubic inch per minute for cast iron or steel you will probably overload the machine. For aluminium alloys and soft brass higher rates may be possible, but the depths and widths of Fig. 4 should still not be exceeded.
Model engineers frequently use endmills as facing cutters. This is fair enough for finishing cuts, but end-mills are not happy when taking a deep cut of width approaching the cutter diameter. and downright miserable if asked to cut a slot. The “Rippa”will work full width. as will the slot drill. If much metal has to be removed it is best either to rough out with a series of cuts as at 4a and then take a facing cut. or to use one of the other types of cutter and change over for finishing. Shell endmills ARE endmills, and designed for use as Fig. 4a, but again with light cuts can be used almost full width for finishing. The maximum depth of cut for side-and-face cutters or slitting saws Is academic so far as work in the lathe is concerned, as there is not enough power to use them to the full.
For flycutters the situation is rather different. They can be treated as ordinary boring tools,but as soon as the depth of cut becomes large the shock load at the beginning or end of contact causes problems. The feed rate can be increased to perhaps 0.005 inch per revolution for most materials. The rule here must be to work at a depth of cut which the machine and work seem to be prepared to accept. Do NOT forget the workholder; the shock load can easily displace a machine vice – it happens even on full-size milling machines occasionally!
To sum up. The cutting speed is the main factor determining tool life. The figures suggested above are not critical. but when in doubt, use a lower speed. Feed rate is governed by the tooth load. Too high a tooth load will result in poor finish and may cause “interference ” on the primary clearance. Too low a feed rate will cause rubbing, especially if the cutter is a bit worn. Again,the rates derived from Fig. 3 are not critical. The depth and width of cut which can be used depends more on the rigidity of the machine and the power available than on anything else, and should be as high as can be managed (though preferably not beyond those shown in Fig 4) with comfort. Very light cuts should be avoided, especially if the cutter is not dead sharp. In general, if the machine seems to be cutting happily there is no need to worry too much about exact feeds, speeds, and depth of cut!
CUTTER HOLDING. The classic milling arbor, carried between centres, is of limited use when milling in the lathe. First. the clearance between arbor and cross slide is small and as seen in Fig. 5 will not permit any reasonable size of machine vice to be used. Secondly , the need for clearance between tailstock and saddle means that the arbor will be relatively long and slender. The third difficulty is that due to the direction of rotation of the cutter the work ought to be fed from the back of the lathe to the front. The cutting forces then tend to be upwards, but the saddle is designed to take downward thrust.
Nevertheless. there are situations where such a mandrel is useful, and Fig. 6 shows the arrangement. The cutter (usually of half-inch bore) is held against the shoulder by recessed spacers, and it is important that these be a good fit on the mandrel and be faced square to the bore. A narrow double-ended spacer can be made if it is desired to carry two.cutters for straddle milling operations, but in my experience the arbor is used mainly for slitting-saws and, occasionally, for gear cutters. The usual set-up is with the arbor between centres, but if the driving end is held in a 3- or preferably a 4-jaw chuck this does stiffen up the assembly.The end of the arbor is turned down with a shoulder so that this can be located positively against the chuck jaws. It is not usual to provide a key for the cutter, even though the latter may have a keyway. The depths of cut which the slender arbor permits are unlikely to cause cutter slip, and in a way this can be a safety device if excess load occurs accidentally.
ENDMILLS are usually held in the lathe chuck. The slight runout will not matter unless co-ordinate setting is being used, in which case the cutter should be ·mounted in the 4-jaw independent chuck and set true. The greater problem with the chuck is wear on the jaws. This means that the cutter shank is unsupported at the outer end, the end which matters. A strip of paper round the shank at the front edge of the jaws will help a great deal – use paper rather than shimstock. However, there is another consideration which makes the use of the independent chuck desirable. The grip must be really tight, if anything other than a slight finishing c’ut is involved. The vibration can cause the cutter slowly to move in or out of the chuck jaws and if an attempt is made to counteract this with a self-centring chuck the scroll may be overstrained. SLOT DRILLS should always be carried in the 4-jaw chuck and set true if an accurate slot is to be cut. (The usual tolerance on cutters below inch dia is -0.0005 to -0.0013 inch, but an endmill will lie between -0.0005 to +0.0025 inch).
Bar-holding collets do offer an accurate means of securing cutters, but though they may hold the cutter securely in the rotationary mode there is more risk of the cutter moving axially. The collet is hard, as is the cutter shank if it is HSS, and this combination is very slippery.A depth stop within the collet will prevent movement inwards. but there is no means of prevent ting the cutter from “walking outwards”. Small cutters mounted on 8mm “collet arbors” (Fig. 7) may,of course,be held in an adaptor held in the taper of a larger lathe if a suitable drawbar is used.
SHELL END MILLS require a special stub-arbor. and Fig. 8 shows a design which can be used eit her in the “Autolock ” chuck mentioned later or in a normal lathe chuck. It will be noted that there is prov1s1on for a drawbar in the latter case.The diameter of the shank is made to suit the largest collet of the smaller “S” type Autolock, but can be larger if for use only in the lathe chuck;the stiffer the assembly the better. The drive to the cutter is taken through the small peg (though friction would probably be adequate) and the adaptor is drawn back until the shoulder butts on the chuck jaws before finally tightening the chuck.
A similar adaptor can be used for gear cutters, side-and-face cutters etc, but the distance between chuck face and cutter may have to be extended to bring the cutter to a reasonable position relative to the cross-slide. This extension should be of the maximum diameter possible; it would be unwise to extend the arbor for more than an inch or so as the overhang would then be excessive.
The majority of the endmills and slot drills sold today have screwed shanks to fit one or other of the proper milling chucks. Fig. 9 shows the Autolock. This is carried on a taper which fits direct into the milling machine or lathe mandrel. (No. 2 M.T. is usual for lathe work). The taper shank is screwed for a drawbar and this must be used. The body carries a collar with a left-hand thread. Fig. 9a. This is the damping ring and is intended to be tightened against the mandrel nose once the drawbar is tight. It stiffens the assembly, and is not needed on larger machines with bigger tapers. It is NOT a device for freeing the chuck from the taper, though it can be used as such.
Referring to Fig. 9 the body, A, carries a locking sleeve, B, which, in turn,carries the collet, C. The sleeve with the collet is inserted into the body and screwed up until the shoulder butts. It is then tightltned with the special spanner. The cutter, E, is inserted and screwed up hand tight, when the centre in Its shank will abut onto the centre at D. In action, if the cutter is not quite tight enough the first touch with the work will take it up further, at the same time automatically tightening the collet on the shank. The cutter cannot move up or down thereafter – indeed, if the cutter is taken out and replaced the projection will be found to be within the odd thou or so of the original position.
Each chuclk has four collets in the set and the “small” chuck will accept from 1/16 inch up to 25/32 inch dia cutters or the metric equivalents. (Metric holder collets are needed for metric cutters). A large size IS available, but not w ith a No. 2 M.T.shank ; this carries cutters from 13/ 16 up to 2 inch diameter. A similar type the “Dedlock ” chuck – is available for carrying shell endmills and short overhung slabbing cutters,but this is too large to fit most lathes.
Both types of chuck are relatively costly,though not as expensive as a precision 3-jaw chuck, the alternative commercial product. They may be considered not really worth while unless a great deal of milling is done. However, for the serious practitioner this type of holder (there are others on the market on the same principle) is by far the best. And as many milling machines used by model engineers also have No. 2 M.T. sockets the chuck can be used there also, should the Christmas stocking be found properly filled some time!
Those who have made themselves a master-and-slave chuck system can, of course. make up “slaves” to occept both plain shank and threaded cutters. Fig. 10 shows one such , carrying a FC3 “throwaway” type endmill, though the same slave can accept any 1/4 inch shank cutter. It is only necessary to make a slave, bored when held in the master. to suit the shank diameters of the cutters you have. Fortunately these are more or less standard diameters these days, but a “special” takes very little time to make. I find that I can hold most cutters simply with a set- or grub-screw, but you can easily grind a flat if you like. For endmills and slot-drills up to t-inch diameter the master-slave system is as accurate a cutter-holder as anything available and,of course. has the added merit that it serves for many other purposes as well. It can hold the centring point in one slave, to be replaced by the cutter slave when ready.
The really important point to watch in holding any type of cutter is axial security along the axis of rotation of the On some materials (especially soft brass) the inevitable rake on a spiral-flute cutter can cause it to “walk into cut”, and the vibration found on most milling work can encourage movement. This vibration will rapidly loosen any Morse taper if no drawbar is used. It is a bit disconcerting to find the cut getting deeper and deeper along the feed-line I (yes, it has happened to me,too I) Cutter slip in the rotational sense may not be so serious; to be avoided,of course – it is not the best type of “safety valve ” against overloading, as some would have us believe. The second important factor , more important for slot drills than for endmills, is cutter runout. For normal facing work a GOOD 3-jaw chuck is sufficiently accurate, but for serious slotting it is wise to correct any error if you can.