PDA

View Full Version : Trouble making dovetails - darn bits keep wearing out!



Paul R
11-22-2009, 08:14 PM
Hi Folks,
I've been making an MLA quick change toolpost for my Logan 10-inch lathe for the last few weekends. This weekend, I was trying to make some toolholders out of 1018 cold rolled steel. This involves cutting a dovetailed "socket" in the tool holder to fit over the dovetail "tail" on the main body of the tool post. I rouged out as much as I could with a straight bit, and then used the dovetail cutter just to finish the dovetail part. The trouble is, the corners of the dovetail bits wear out really fast - I could only make 2 tool holders with the dovetail bit before the corners were too worn and the cutter quit working well. What going wrong here? Here's the dimensions and cutting conditions:

Dovetail cutter: Whitney 3/4-inch x 60 deg M-42 cutter
Workpiece: 1018 cold rolled steel
Dovetail is 1/4-inch deep
Cutting rpm is ~500-700 rpm
Cutting depth of cut is ~5 to 10 thousandths per pass
Using water based cutting fluid

Is it normal for these bits to wear out so fast? They're kind of pricey, so I would be surprised if that's all you could get out of them. Should I use another metallurgy for the bit? Different cutting speed/feed? Any suggestions?

Thanks for your advice!

Paul

wierdscience
11-22-2009, 08:33 PM
Are you making sure to clear all the swarf out of the way as the cutter is working?Re-cutting chips dulls mills fast.

mechanicalmagic
11-22-2009, 08:57 PM
No, it's not normal for a cutter to wear out on two parts.
I see a few things that send up a ted flag.

First; at .005-.010" per pass, you made something like 20 passes on each part. WAY too many passes, I'd probably use two rough passes, and two finish passes of .005". Conventional milling, until the last pass.

Second; you don't mention the feed per tooth. If you feed rate is too light, the material will work harden. Measure the feed rate and keep it above .001" per tooth.

Third; it sounds like the tips are first to go. The tip is moving the fastest, slow it down. (A faster tool tip will also burn first, if the material has been work hardened.)

TGTool
11-22-2009, 09:06 PM
I'd agree with Mechanicalmagic's analysis and suggestions. I've got one dovetail cutter I've so far used on the MLA T-slot crosslide (8" or so long in cast iron) and perhaps 10 AXA quick change toolpost holders in cold rolled mild steel and it shows no signs of fatigue. It may seem surprising how much material you can reap off in one pass even with the fragile looking tips. I keep a squirt bottle of water based coolant handy to keep things cool and a little lubricated and move chips out so I'm not wasting energy and the tool in much re-cutting.

dp
11-22-2009, 09:13 PM
I've read a couple different methods of doing this. One is to cut from the top down in steps, the other to start at the bottom and move out. The latter being the way to rub the tips off, it seems to me.

And it should be obvious that the center section is cut out with an end mill, first.

Now having said that, I really don't know which is the better method but I'd think that keeping off the tips would be a good idea. It's why all the dovetails I've cut so far have been done on my shaper.

Mcgyver
11-22-2009, 09:19 PM
In a perfect world, parts would lend themselves to drilling a clearance hole at the apex - so the corner of the cutter never touched anything. there us no need, and in fact it is correct, to have the dovetail under cut like this so the two planes don't in fact meet.

As was said, two passes, one to remove material and one to finish. you're on the high end for speed, 80-100sfm is good for mild steel - that's 400-500 rpm. going slower still will not hurt and might prolong cutter life....cutter life is extended by going slow with a decent chip vs fast and making dust. lots of coolant, ideally flood....but i think mm nailed 80% of the problem with the multiple passes

smalltime
11-22-2009, 09:20 PM
Way too fast in the rpm dept. try around 200.
Try to use two ruffs and one finish of .010 per side.

Paul R
11-22-2009, 09:24 PM
Sounds like I have a LOT to learn!

The dovetail milling was done on a friend's benchtop mill, and it has manual feed on it, so I'm not sure exactly what the feed rate is. Basically we were turning the feed crank at a rate that would move the cutting bit across the 1-inch wide workpiece in about 10 seconds. It seemed like if we fed faster than that, the bit would chatter/squeal.

The cutting bit has 6 flutes on it, so I suspect we were going WAY less than 0.001 inches per tooth.

It sounds like we may need to slow down the rpm of the bit so that the feed/tooth would go up. What rpm would you suggest starting at? {Oops - this was answered as I was writing my response - maybe 200 to 500 rpm...}

Regarding the work hardening, is that temperature dependent? In other words, will it still happen if the workpiece is flooded with coolant?

Thanks,

Paul

J Tiers
11-22-2009, 09:53 PM
500 RPM is about 98 fpm, OK for 1018, generally. The 700 is a bit fast, 140 FPM.

if you DULL the cutter, probably your RPM are high or feed is slow(and/or material is hard). if you CHIP the cutter, your feed is high (or material is hard). Obviously with 1018, the material isn't hard.

6" per minute, and 500 rpm x 6 teeth= 3000 teeth per minute. 6" per minute / 3000 teeth per minute = 0.002 inches per tooth. Acceptable chipload, probably.

if chipload is OK, speed must be too high. slow down, and adjust feed.

Carld
11-22-2009, 10:18 PM
At .005-.010" per pass all your doing is wearing out the tip of the dove tail cutter. Try 200 rpm and a two or three pass cut.

On the other hand a bench top mill may not take that load. I would take as heavy a cut as the machine will allow.

Fasttrack
11-22-2009, 10:29 PM
In a perfect world, parts would lend themselves to drilling a clearance hole at the apex - so the corner of the cutter never touched anything. there us no need, and in fact it is correct, to have the dovetail under cut like this so the two planes don't in fact meet.

As was said, two passes, one to remove material and one to finish. you're on the high end for speed, 80-100sfm is good for mild steel - that's 400-500 rpm. going slower still will not hurt and might prolong cutter life....cutter life is extended by going slow with a decent chip vs fast and making dust. lots of coolant, ideally flood....but i think mm nailed 80% of the problem with the multiple passes

To save buying a new cutter, why not do as McGyver mentioned and drill a hole in the "corner" ?

It will be stronger and allow for ample clearence during construction and assembly. Just layout the dovetail profile with the tool holder standing "up right" and center punch at the apex where the lines intersect. Then run an 1/8" drill bit (or so) all the way down. A little bit of care should be used (i.e. peck drilling) to avoid a ridiculous amount of drift. A little bit of drift isn't going to matter, so even that isn't a big deal. I'm assuming these holders are only a few inches tall, so you should just be able to get an 1/8 bit all the way through.

<edit> Something like this (this is the "artistic" representation of a tool holder ;) ):

http://i108.photobucket.com/albums/n22/fasttrack237/untitled.jpg

mechanicalmagic
11-22-2009, 10:35 PM
Regarding the work hardening, is that temperature dependent? In other words, will it still happen if the workpiece is flooded with coolant?


Work hardening has ~nothing to do with speed or coolant. Only rubbing the cutter on the material. Some Stainless Steels are known for this trait. Cut or don't.

Paul R
11-22-2009, 10:37 PM
Is M-42 a good material to use for a cutting bit when cutting the 1018 steel? Should I have used carbide or something else?

Fasttrack
11-22-2009, 10:46 PM
Is M-42 a good material to use for a cutting bit when cutting the 1018 steel? Should I have used carbide or something else?

Cobalt is a good choice. It has higher hardness at elevated temperatures than ordinary tool steel. No need for carbide. Since a picture is worth a 1000 words, I attached a picture in my post above. I would really consider doing something like that and just using the cutter you have, unless it is really trashed (or unless someone else here sees an obvious reason not to do it this way...)

dp
11-22-2009, 11:15 PM
Here's a homemade cutter using an insert: http://www.gadgetbuilder.com/ToolHolders.html

I had less luck with mine:
http://metalworkingathome.com/?page_id=35

DR
11-23-2009, 02:36 PM
.................................................. .......

The dovetail milling was done on a friend's benchtop mill, ............................................




That's one of the problems, dovetail cutters need a rigid machine. These type cutters usually have neutral rake which makes them not very free cutting. But, that type grind makes them relatively easy to sharpen.

I have a largish dovetail cutter that was CNC custom ground with a helix and rake. It cuts like butter compared to normal factory grinds.

lazlo
11-23-2009, 02:46 PM
These type cutters usually have neutral rake which makes them not very free cutting.

The home-made FrugalMachinist type doorknob cutters have neutral rake, but the commercial indexable dovetail cutters all have double-positive axial/radial rake.

By the way, another advantage of the cut-out, like McGyver is describing, is that it's much easier to scrape :)

Frank Ford
11-23-2009, 02:57 PM
I got one of those insert dovetail cutters:

http://www1.mscdirect.com/ProductImages/0003187L-81.jpg

It has those flat inserts that basically club the metal into submission. After cutting a few tool holders from 1018 steel, I finally took the inserts off and with some judicious filing, adapted the tool to accept the same triangular inserts my lathe tools take - with the built-in chipbreaker. Now it cuts really well. I just made six special boring bar holders last week.

By the way, I've come up with a way to get them to fit really well to my wedge-style lathe tool post. I cut the dovetail recess just a bit deeper and not quite wide enough to fit on the toolpost dovetail - narrow by just a few thousandths. Then to adjust the fit to perfection, I mill off .001 at a time from the flats that contact the tool post when it's tightened. I guess that's just another example of how I still think like a woodworker, fitting guitar neck dovetails. . .

tattoomike68
11-23-2009, 03:53 PM
Way too fast in the rpm dept. try around 200.
Try to use two ruffs and one finish of .010 per side.

Thats the way I made a bunch of holders at work, I made a long cut in a bar about a foot long then sawed them off. I ran the 1.250" dovetail cutter about 275 rpm.

That cutter is now 10 years old and still cuts fine. we even cut sickle teath shapes in T1 to make grape pruning machine cutter bars with it, without hurting it.

Frank Ford
11-23-2009, 07:27 PM
Another trick I use for making tool holders is this little diagram I have posted on the back of one of my tool holder drawers:

http://www.frets.com/HomeShopTech/ShopTips/225.jpg


So, now I take a piece of 1018, rough out the center of the cut, and make a total of two passes with the dovetail cutter - one on each side - full depth. Using the guide as to how deep I cut and how far left and right I need to move the cutter, I just use the DRO and I don't have to measure anything at all when I want to make holders. I find myself making special holders for special tools. Last week, it was a set of dedicated boring bar holders - one each for the 1/4, 5/6, 3/8, 1/2, 5/8 and 3/4 Mari Tool insert boring bars I've acquired.

Alguy
11-24-2009, 12:10 AM
I have a weldon brand dovetail cutter i have cut 4 tool holders in steel and 2 in alum. It seems to cut as it did when new . i cut at 450 rpm (slowest speed on my machine) usually making 3 or 4 cuts per side. i also cut dry. perhaps you speed was bit high.

whitis
11-24-2009, 01:25 AM
It seemed like if we fed faster than that, the bit would chatter/squeal.


Generally speaking, you increase feed when you have chatter, not decrease it. "Increase feed, decrease speed".

You already know you were feeding too slow. But knowing you reacted backwards can help in the future.

Peter N
11-24-2009, 03:08 AM
This was cut in 2 passes plus a 0.005" finishing cut out of EN8 (1045) steel.
It's approximately 3/8" high and 1/4" deep. Coolant applied via squirt bottle.

http://www.btinternet.com/~p.neill/Dovetail_Small.jpeg

Peter