Milling Dovetails

[Chuck in E. TN]

I am in the middle of making Harold Halls Deluxe Grinding Table. I need to mill dovetails in several parts.  The dovetails are 60° and 8 mm (.314 in) to 8.5 mm (.335 in) high, length up to 50 mm. As I’m getting ready to order my first dovetail cutter, what size is recommended?
I will be ordering the cutter from LMS and sizes available are 3/8”, ½” and Ύ in. The cost difference isn’t that much, but I don’t want to order all three now.
Any other comments on milling dovetails welcome, as I’ve not done them before. Speeds and feeds? DOC? Multiple passes? Material is mild steel. Mill is an HF X2.
Go easy on this noob, eh? Thanks in advance.

Chuck in E. TN

[Lew_Merrick_PE]

Chuck,

Get the largest diameter that will clear your dovetail.  I am not sure what an "HF X2" mill is, but I assume it is some type of mini-mill.  Clear as much material out of the way as you can with regular end mills before using your dovetail cutter.  If at all possible, get two cutters.  Identify one for roughing out the dovetails and keep the second as a finishing cutter that will stay sharper longer because of the limited number of lighter cuts.  I don't think I have ever successfully taken a dovetail cut more than (about) 1/8 inch of material removal -- and that was on a rigid column mill, not a light mill.  I usually limit such cuts on my "mill/drill" (that started out life in 1976 as a JET-16 unit before it was dropped off a loading dock) to about .050 inch when roughing.  Finishing cuts are usually in the less than .015 range.

The recommended cutting speed for LC steel (1015-1020 assumed) is 80-150 surface feet per minute.  As I am assuming that you are running a light mill with lots of flex (as compared to, say, a Gorton 9J vertical mill), run towards the bottom end of the speed range and subtract (about) 20%.  80 SFM is 960 surface inches per minute.  Divided by pi gives you 305.6.  Divide that by the largest diameter (in inches) of you cutter to get your RPM.  You should be able to use as high a feedrate as your mill will handle without vibrating the cutter too badly.  Were this being done on a truly rigid mill, I would set the cutter speed at about .008/flute (i.e. .008/flute * Number_of_Flutes * RMP = inches per minute feedrate).

Does that help?

[DaveH]

Chuck,

See if I can add a little, to what Lew as said.

With respect to Lew, forget the manufactures data regards feeds and speeds they are not for you and me with home workshop type mills. Semi and industrial machines fine.

Make sure the work piece is held in a rigid manner.
Only cut one side of the dove tail at a time.
Use the largest cutter possible.
Only cut in conventional milling. (Not climb milling)
Make sure the two unused axis are locked.
Take it slow and steady.
First cut the slot out with a normal end/slot mill.

Now for the dove tail.
Start with a spindle speed 500/700 rmp – first cut tiny .005”, a slow and steady speed careful when the cut first starts – making sure it is just cutting – not too fast – listen and feel the machine. At the end of the cut, remove all chips then return the cutter to the start. Two ways here either leave it running, or stop the spindle and return, if you stop the spindle you can then turn the cutter by hand so it does not touch the work piece.
It is not a good idea to cut on the way back.

Now remember each time the cutter it set into the work piece the load on the cutter increases, there is more cutter surface in contact with the work piece. So as you cut more of the dove tail you may have to reduce your feed. Try to keep clearing the chips away.

If you are happy and the machine was happy you could in crease the speed, and feed rate, keeping the same .005” cut. Everything good no bad vibrations increase the cut say to .010” or even .025”. Listen and feel the machine, it will start to complain, take notice or your cutter may break.
Finish cuts of .002” or even .001” if you have to are OK, just increase the feed a little.

Chuck, it is a bit of a slow process, take your time, feed especially slow when the cutter just starts to cut, then speed up.

Try to keep the chips away.

I hope this helps a little, it’s one of these things that is much easier to show than explain.
 
DaveH

[Jonny]

The dovetails are 60° and 8 mm (.314 in) to 8.5 mm (.335 in) high, length up to 50 mm.
3/8”, ½” and Ύ in.

Just measured a 3/8" as best i can, the max depth you will achieve is 4.5mm.
An 1/2" decent quality one i have here can only achieve 4mm depth!
All the same a 3/4" on an X2 will be asking for trouble, underpowered and serious flex. Soon find out when cutter lasts a couple of minutes.

Sound advice from Dave i always ignore recommended speeds and 'get a feel for it', dont force it.
You can get a far better finish by climb milling, i do it all the time especially on precision dovetails.
Plenty of coolant as well.

[DaveH]

Jonny,

You can get a far better finish by climb milling, i do it all the time especially on precision dovetails.
Plenty of coolant as well.

Ah... but do you climb mill on a X2, and if he doesn't have flood coolant?

DaveH

[Chuck in E. TN]

I have climb milled on my X2, with varied sucess. Usually, with tiny DOC, I get better finish.
I do not have a collant system, but for the dovetails, I will have a pump oil can at hand and apply liberal cutting oil.

Chuck in E. TN

[Bogstandard]

Take Dave's advice about climb milling. I have a mini Bridgeport, and I avoid it like the plague, it causes more breakages and trouble than anything else if you don't have anti backlash lead screws.

If you take it steady with your cuts, not only will you end up with a great surface finish, your cutter will survive until another day as well.

If you go to the bottom part of the first post, I show in detail how I do my dovetails, and then a bit further down on the first page, the next post I do showing pictures, I show how I brought them to exact size.

http://madmodder.net/index.php?topic=2323.0

Use a bit of cutting oil in a squeezy bottle for when the going gets tough, don't use a lot, just enough to keep the cutting smooth.

[Chuck in E. TN]

Thanks for chiming in, John. I always learn from your input. I lived in the UK for 8 years, and man, I wish it was down the street from you. I have learned a lot from you over the years, in spite of meself!

Chuck in E. TN

[mgj]

I'd second or third the bit on feeds and speeds. I was supplied a dovetail cutter which seemed very spindly at the thin tips, and to have gone wombling in with that cutter at normal rates might have been unwise - don't know for sure because I never tried it.

For those who are determined to climb mill without the right backlash eliminators, you can nip up the table locks, just to prevent the table from being drawn in. OTOH to my way of thinking, on a lighter mill it might be better just to go slow and then lap the dovetails after cutting the normal way? (if necessary - which it may be because the final cut is quite long)

[johnf345]

no-one seems to have mentioned that for a good dovetail all of the four touching surfaces must be "parallel".
Cut each side to nearly complete then do a last pass with the cutter at the same setting. On the female part
it is the side - slopy bit - and the top surfaces that touch. Cut both of the top surfaces with the
cutter at the same height.
On the male part the flat surfaces that touch can be cut at the same time with the same tool as
the slopy bits.

But there are other ways the touching surfaces can be defined but whichever they are cut them so they are all parallel.

[dvbydt]

What everyone else said but I would hog out the V with a single point cutter like a flycutter of a bigger diameter than the dovetail cutter. That way you have a chance to get the geometry of the cutting tip better supported so it won't chip. Slow - yes because you want to use it like a screwcutting tool that is being plunged straight in, but it's not expensive like a dovetail. Just leave enough for a clean up cut.

Ian

[AdeV]

I second everything DaveH says. I've cut a few dovetails now (QCTP holders mostly); because I have a full-sized Bridgeport I can go quite deep with the early passes, when only the ends of the teeth are engaged, but the final passes are in the 2-3 thou range. I DO climb-cut my final cuts, but I only take 0.001" off at most, and I take it very slowly with plenty of cutting oil. I use neat oil, and the flood system, which makes a bit of a mess but at least keeps the chips out of the way. Before I had enough oil in the sump to use the flood pump, I'd use the hand pump to squirt oil in "frequently".

I usually cut dovetails to width using pre-calculated distances & the DRO to tell me when I've done enough; but having a test piece is a better method, there's nothing worse than taking the piece of the mill and finding you need to take another couple of thou off it...

[andyf]

...... there's nothing worse than taking the piece of the mill and finding you need to take another couple of thou off it...

Oh yes, there is! Making such a mess of measuring that you need to put 2mm back on, as I did with a QCTP toolholder. 

Happily, the piece of 2mm steel strip which I stuck on with JB Weld is still in place after two years.

Andy