We talked about turning threads using chromium alloy. We end up with above ideas:
1) Flipping verticaly a tool to force forces to the bottom [x]
2) Use very shallow cutting [v]
3) Use molybdium disulfide [v]
4) Use live center [vx]
[x] - impossible for me because of lack of headroom in mounting [vx] - irrelevant
We haven't talked about cutting geometry but said about compound feed. As I understand English this is a cutting along generator (?). My tries fell down - one side of generator had much smaller angle.
New things to considerate. I've measured hardness and it's about 9HRC (Rockwell C) - ten times the duralumin. Cutter with carbide makes very rugged surface. High speed steel is much better. Why softer steel is better?
Nowadays cuters uses profiled carbide with coatings (see Sandvik Coromant F profile). They are too expensive for hobby work. ISCAR holders - 200$ + plate (10$). This is interesting. Do You say that the CNC lathes have much smaller vibration and the cutting speed is higher than 100 turns/min for 1 mm ISO metric threads? I don't know how to get good thread from carbide.
I think I could master HSS cutting here but there's problem with cutter geometry. I don't see one angle - angle of rise in thread (maybe wrong translation). This angle is important for surface quality. They depend on thread diameter - typically 1.5°. Maybe I overestimate its importance. Correct me if I am wrong.
Why is a live center irrelevant? The workpiece will flex. If the unsupported length is much more than about twice the diameter, it
*will* need support.
It sounds as though you adjusted the compound, but did not also adjust the threading tool so it was at the proper angle to the axis of the lathe. There is a special rule, called a "fishtail rule", which has notches to help you get that alignment correct. (As well as to help you to grind a threading tool to the proper angle.)
The rule looks something like this (within the limits of ASCII graphics): _________________ / V / / / < < \ \ \________/\______\
All of the angles at the ends and the sides should be 60 degrees for either US threads or Metric ones, but 55 degrees for British Whitworth threads). The corners of the fishtail tips should, instead, be 30 degrees, and the obtuse angles at the sides of the arrowhead end should be 150 degrees.
You place one side of the rule against the cylindrical workpiece, and adjust the toolpost so the tip of the threading tool fits properly into one of the side notches (pick the one which is the better fit for your size of threading tool). An alternative is to place the two tips of the "fishtail" (to the right in my drawing above) against the face of the chuck, and as above, adjust the threading tool and toolpost so the tip matches one of the side notches.
The sign of correct setting is that there should not be more light showing through one side than the other. (Put a piece of white paper below it to reflect more light up to the underside.)
HSS is not really *that* soft. Its benefit is that it can be sharpened much better than *most* commercial carbide inserts -- especially coated ones, which tend to dull the edges slightly.
That sounds much more expensive than what I have paid buying from MSC -- but you probably have to deal with import duties, among other problems.
Most CNC lathes are *very* rigid, and they can cut threads much more rapidly, simply because they do not have to depend on the operator's reaction time to stop the thread at the end. That is all automatic with CNC threading. (My particular small CNC lathe -- an Emco Maier Compact-5/CNC -- is not that rigid, and the controller is too slow to allow threading at much more than 200 RPM -- and sometimes slower for particularly coarse threads. But it is not typical. Those were mostly sold for use in training classes so people could learn CNC without risking damage to a big and very expensive lathe. However, for hobby work, it is quite satisfactory within its size range -- a maximum workpiece diameter of about 5" (125 mm) at the chuck, and probably about
80mm to pass over the cross slide.
My experience is (mostly) with coated carbide inserts, in the
12x24" Clausing (300mm maximum diameter above the bed and 600mm between centers.)
And I normally thread brass, aluminum, or 12L14 steel -- a
*very* free-cutting steel. The steel which you are cutting might give me problems too.
For most threads, with HSS tools, it is accommodated by the clearance angles on both sides of the tool -- the angle of the sides from the top to bottom. Typically, there is more clearance on the left hand side than on the right hand side, which is fine for normal right-hand threading, but not for left-hand threading.
The insert tooling which I use has the carbide anvils (hard plates which support the carbide inserts) available with different angles from one side to the other, so they will tip the insert to adapt to the helix angle of the thread. This seems to be more important with Acme threading inserts than with normal V-threading inserts, but for left-hand threads, you *will* need an extreme one.
Note that the normal design of the insert tooling is such that if you have the shank of the insert holder parallel to the face of the chuck, your angle will be correct, so you won't need to use the fish-tail rule. Just set the toolpost properly *after* you set the compound angle, as otherwise, setting the compound angle will disturb the setting of the tool's angle.
Thanks you still watching. I didn't use a live center because before doing the thread I used a test area as near the headstock as possible.
I always use a 'fishtail rule'. You know, yesterday I turned several threads. In chromium alloy and in brass. After reaching the 0.7 mm of the thread height it was destroyed! I missing something. I also found some different thread heights. In my handbook it is ~0.8 and in SECO guide it is 0.65 for 1mm pitch.
HSS is about 65 HRC (at the end of the scale). Carbide makes awful sound I always worry with it. One note - I used carbide which is soldered to the HSS. This is a P30 carbide. I don't have any problems with sharpening.
Thread turned with HSS after polishing using a paper looks reasonable. Unfortunately I had my second accident. The first was my hand struggled by HSS. An unexplained behavior of my lathe - after adjusting cross slide direction from roller to me the slide went reverse. Luckily the feed was 0.08 but my lathe got for its bearings :(
The cheapest holder + plate in Poland - 78$ made by Pafana (Seco license):
Looked at the Compact-5/CNC - why such a big control unit in microcomputer era ? Maybe a requency converter for RPMs insetad of transmission?
I will look at the 12L14 but it sound like what is strange that it doesn't have an equivalent in old polish sort. The sulfur and lead is the reason of very good machining properties.
Helix angle you wrote is a lead angle ? How important ?
With Kind Regards, ______________________________________________________________________
Jack Zagaja - photographer, designer, programmer free photoshop plugins, photographic assistance opinions and much more ... email@example.com
Hmm ... this is feeding with the compound? It may be that your compound is marked differently. Some are.
The angle needing to be set is 29-1/2 degrees (or 29 degrees) to the direction of the cross-feed. Some machines have scales on the compound which instead measure the angle to the carriage travel along the bed, so on those, the angle should be 60.5 or 61 degrees instead. At least degrees are the same, Metric or Imperial measurement. :-)
The proper angle is just barely grazing the side of the thread as you feed in -- cutting a tiny amount off the right-hand side of the thread, while cutting mostly off the left-hand side.
If you are using the kind of index which has the measurement from parallel to the bed ways, you will destroy the right-hand side of the threads.
I would draw that with ASCII graphics, except that I only have one angle of '/' and one of '', so I can't really show what I mean.
The end of the scale for steels, perhaps (with Cobalt steel being a bit harder and a bit better at handling high temperatures), but solid carbide is noticeably harder.
Usually called "brazed carbide". Not what I use. By "carbide inserts", I mean the ones which are secured to the shank by screws and clamps, and which can be replaced without having to re-zero the dials on the lathe.
The noise may be chatter -- and that could come from flex in the steel shank to which the carbide is brazed. A larger shank cross-section helps significantly with this.
My insert-type threading tools have a 5/8" square shank (about
16mm), and are noticeably better than the 1/2" ones (12.70 mm)
For my best boring bar, the bar itself is solid carbide, with an insert mounting in the end. This has *much* less flex than steel of equivalent size -- even with a significant length extended, and allows me to start boring in a drilled hole of only 1/2". (It is too expensive for me to buy normally, but I was lucky to get one in an eBay auction, so I am quite happy.)
Sharpening, of course, makes you *need* to re-zero the dials, even with a very good quick-change toolpost.
And for sharpening carbides, you should be wearing a dust filtering mask, as the grindings from carbide tools can be dangerous to your lungs, long-term.
I'm a little puzzled by your description of what happened. I hope that you were not hurt.
The spindle motor is a big permanent magned DC motor, and the speed is controlled by applying differing voltages.
The actual controller circuit board in the Compact 5 is about 8" wide by perhaps 16-18" long. All of the controller is on that single board (except for a daughterboard to allow larger EPROMs for the later version of the firmware.
However -- also in that housing are:
1) Large transformer to provide the various voltages -- including that to run the spindle motor.
2) Large contactor (relay) to control power to everything, so the big red "panic" switch can shut it *all* down at once.
3) Key-operated power switch to allow protecting the system from little hands.
4) The big red "panich" switch.
5) Meter to monitor current drawn by the motor.
6) Small tape drive, to allow saving programs onto tiny Phillips dictation tapes.
7) Additional board to allow control of the tool-changing turret, and to allow starting and stopping the spindle motor under CNC control.
8) Piggy-back board which contains:
a) Video driver to allow editing a program on a CRT screen.
b) RF modulator, to allow this to be displayed on a standard TV receiver
c) serial interface, to allow saving to punched tape and loading from that. (With a bit of programming, you can save to and load from a PC as well, and with a bit more programming, you can build the machine programs in the PC and download them to the CNC machine.
9) A board along the bottom which plugs into the CPU board and which contains the stepper motor drivers.
10) There are probably some other things in there which I have forgotten.
But -- it also serves as the back splash guard for the machine, and gets the controls well above the area of danger while the machine is operating.
Note that the actual CPU in that machine is far from exciting, It is the 6502 -- 8-bit data bus, and 16-bit address bus, and to my mind inferior to the 6800. (The 6502 was used in both the Commodore "PET", and the Apple-II, among other machines. As a result, it is a lot more limited than normal.
They are, indeed.
The analysis of 12L14 from a 1972 Steel and Aluminum book from Jorgensen (a vendor of metals) is:
Carbon 0.15% Maximum Manganese 0.85/1.15% Phosphorous 0.04/0.09% Maximum Sulfur 0.26/0.35 Lead 0.15/0.35%
The recommended cutting speed for 12L14 is 300 SFM (Surface Feet / Minute), which corresponds to about 91.4 Meters/minute. (About 360 RPM for an 80mm diameter workpiece.
Note that 12L14 is not particularly strong compared to many of the steels, but it is the nicest steel to machine in existence. The strength specs are:
Tensile Strength (PSI) 78000 (sorry, I can't convert these to metric quickly) Yield point (PSI) 70000 Elongation in 2" 15% Brinell hardness 163
They are not weldable, and are not considered particularly good for case hardening. But --
For fairly fine threads (as is common for optical parts), not very. The relief angle of the sides of the cutter accommodate it. However, if you have an unusually coarse thread, the tool will have to be ground to accommodate it.
Good Luck, DoN.
P.S. Out of curiosity -- have you looked at the free unix image processing program, called "The GIMP"? Have you considered working up plugins for that?
I used the compound but forgot to use a proper angle. I used constant
0.05 mm compound and 0.15 per transition infeed. My fault. Without compound I've found that height above 0.7 cuts down the thread. I don't know why. I will certainly spend more time in practice since in advance this didn't happen.
I also red old messages about threads so no need to repeat.
Try to use some drawing suites. Send me your graphics. My mail address need a bit of editing (anti-spam).
I didn't know that. I was informed that the clinker used to even out a grinder is dangerous not the carbide itself.
No no but the scar is visible. I've just touched a cutter. That was my first hours with lathe and I think it is needed to take care in future. A student working on university lathe is illegal so it's my friend favour.
I am not a regular programmer. Truly no talent here however wrote a small plug-in for DTP studio. It can manipulate on negatives and slide RAW scans and several scanners. Because of small knowledge in programming I and my friend had encouraged GIMP developers for several changes in API. For example linear histogram, highlights-mids-shadows probes, changes in their algorithms etc. So what you see in ver. 1.3 and 2.0 in Levels and Curves is our work :) Hopefully GIMP will read Photoshop AMP curves settings and use colour-management.
Hmm ... your infeed was via the cross-feed, not the compound, you say? This suggests that the cutter was lacking one or more or the relief angles -- or that the cutting point is above the centerline of the lathe spindle, so the relief is rubbing on the thread.
Or -- perhaps the threading cutter is not full width or depth? The 'V' of the point should be the full width and depth of the thread. (And in the case of some threading inserts, it even forms both the crest and root shapes as well, so it is appropriate for only one thread pitch.
O.K. I've drawn the infeed angle using xfig, and converted it to .PDF format, since I don't know whether you have xfig available. It shows the basic thread form (lacking the features of root and crown shaping) and the infeed angle. Note that the angle of infeed is such that it cuts mostly off the left flank of the thread, and only skims lightly off the right flank.
The size is only 1304 bytes (before encoding for transmission).
I'll try e-mailing it to you (actually before I send this message to the newsgroup, so I have your e-mail visible.)
Be warned that there is a good chance that you will *not* be able to e-mail me, as I have many Polish sites blocked as sources of spam. (Most likely, they are simply not careful enough to keep customer's machines from getting infected and being used to relay spam.
A quick check suggests that your ISP is not blocked at the moment.
Each carbide tool from MSC comes (at least in the USA) with a required document called a MSDS (Material Safety Data Sheet), and it warns about hazards of inhaling the dust from grinding the tools (Actually, carbides are carbides embedded in a Tungsten (Wolfram) matrix, and that may be the actual source of problems.
Yes -- is is possible to cut yourself on the lathe tools if you don't take enough care -- and of course there are much greater hazards, though those are usually more obvious.