4140 prehard and hss cutters ?

I need to make a holder for a from cutter
for my cxa tool post so my question is
will the hss dove tail cutter do ok in
4140 prehard around 32rc ?

or should I machine it and then heat treat it?

and then for the profile cutter A2 or O1?
only cutting 6061 with it

HSS in prehard will work just fine. I would use A2 for a cutting tool.

Tom

Like he said- ought to cut fine! I'd take speeds down a little from cutting mild steel. It's pretty tough stuff and generates a lot of heat that your cutter won't like! I'd suggest using a spray mist as well.
For what it's worth, I made several tool post holders for several different lathes I my spare time at work. I used a bunch of different steel that I had laying around- old fork truck forks, hardened mystery metal about R40c or so and even some 4140 pre heat treat. Drilled and tapped fine. HSS hog mill fine, but I cheated and used a home made dovetail cutter with carbide inserts.
I used a cutter body turned out of 4140 ht. 7/8" shank and put it in a hex collet block with an angle shim (5 degrees) under it and just used a 3/8" end mill to make 3 "seats". Mill them down to the thickness of the insert. You'll have to get the vise swiveled to the correct angle (30 deg. for tnmg 322). Don't forget that the 5 degree clearance for the negative rake insert will slightly change your 30 degree to a little wider I didn't do the math, I just used Kentucky windage. If you used a positive rake insert and left the collet block flat in the vise it should come out correct, I'd think. The problem with the positive rake iserts that I have access to is that they need a clamp and that was just too mych to mess with. The tnmg inserts have a hole in them. I could use a 6-32 cap screw to hold them in !

Run REALLY slow with a dovetail cutter. They have so little material on the tips that they can't shed heat and burn easily. Takes a little more time, but saves your cutter. I'd run 40-50ft/min at max, even using coolant. Mist, flood or even squirt bottle of cutting oil, anything helps.

I find that 4140 PH does tend to wear HSS tools down. Dovetail cutters, depending on type, may be more easily worn down. I was referring to lathe cutters. I thought the HSS would give a good finish because I did not want to grind the part, but I had to go back to carbide inserts to get any work done. I was making some longish custom mill arbors, so there were a lot of long passes.The HSS was dull before the finish pass was done.

I have use HSS to thread 4140 in a pinch but it is rough going even at slow speeds: The HSS gets worn down really fast and it is difficult to get a good surface finish (because of the low speed you need to go at).

A lot of our fixtures fit onto a 3R rail and utilize a dovetail. We use a hss cutter in 17-4 around 32Rc and have excellent results. Typically I run around 200 rpm and 1 ipm radial cuts are around .03. These days I cheat and wire them lol.

New HSS dovetail cutters are often ground so that the tips of each flute are the intersection of the two cutting surfaces---an extremely fine tipped point. Those points are easily overheated or broken off---in fact it is hard not to do so. I would suggest stoning off just a bit of each tip so that there is a small cutting flat at the intersection of the cutting surfaces. This is equivalent to putting a nose radius on a lathe cutting tool. Dovetails never fit together at the intersection of their surfaces as two perfectly nested triangles.

Dubbed off cutters last a lot longer.

Denis

I'll throw in a couple more thoughts on this process. I would saw out as much of the waste as possible on this part either using a slitting saw or a vertical bandsaw which ever you may have available. Also at the intersection of the two dovetail surfaces I would probably go ahead and drill through at that intersection with a 3/16 or so drill so that the cutter tips don't have to deal with cutting but rather the side surfaces of your cutter will be doing the material removal.

If you saw out the waste and drilll be intersection, this whole process will go much more quickly and easily and your delicate and expen$ive dovetail cutter will be required only to do finishing passes.

Denis

Dorian makes dovetail cutters with inserts. They cut about as good as any dovetail cutter (which is poorly), but at least you've got the hardness of the carbide going for you, you can run them faster than paint dries, and you can index the inserts.

Is this for home shop use?

I need to make some Hardinge ones for my HLVH (have been looking for reasonbly priced used one for years), not for home shop use, info is applicable and useful.

SBAER said:

I need to make some Hardinge ones for my HLVH (have been looking for reasonbly priced used one for years), not for home shop use, info is applicable and useful.

Click to expand...

Whew! Good thing it is not for home shop as machining 4140 would be altogether different in that case. Gotta keep in mind the crucial questions here.

Denis

Yeah, I know, I will be publicly flogged for this bit of hypocrisy, but this is where shapers can shine. I have several CXA tool holders made on the shaper, made when I needed them on the quick/need. They are just as good as my Aloris toolholders. If memory serves, one or two are made from 4140. If HT 4140, just slow down the speed a little. No big deal.

JH

I know it's no big deal cutting it with carbide do that all the time.
1018 would probably work ok.
but I only have a hss cutter on hand and well don't really want to buy a carbide one

yes did think about grinding a fly cutter but that would be too much work.
ah if only I had a shaper there are still times when it's the right tool for a job.

then again a cnc lathe would eliminate the need for a form tool.

then there is the thought of just making a holder to fit in a cxa-1 holder

but you work with what you have and cutting the right profile on a piece of A2 with my
VMC makes the lathe job much easier.

Drilling and saw cutting is definitely a good idea, but even with both of those the tips of a dovetail cutter will still be cutting on their way into (climb milling) or out of (conventional milling) the hole made by the drill. They will be creating the flat bottom surface of the dovetail. With the saw cut, the amount of material being removed on that flat bottom of the dovetail will be a lot less and the heat will be able to escape the area where the tip is cutting a lot easier. So the tip will stay cooler during the cut and that should help a lot.

The drilled hole will remove any worries about the male dovetail bottoming out in a rounded bottom angle of the female dovetail. It also reduces the stress riser at that point.

dgfoster said:

I'll throw in a couple more thoughts on this process. I would saw out as much of the waste as possible on this part either using a slitting saw or a vertical bandsaw which ever you may have available. Also at the intersection of the two dovetail surfaces I would probably go ahead and drill through at that intersection with a 3/16 or so drill so that the cutter tips don't have to deal with cutting but rather the side surfaces of your cutter will be doing the material removal.

If you saw out the waste and drilll be intersection, this whole process will go much more quickly and easily and your delicate and expen$ive dovetail cutter will be required only to do finishing passes.

Denis

Click to expand...

EPAIII said:

Drilling and saw cutting is definitely a good idea, but even with both of those the tips of a dovetail cutter will still be cutting on their way into (climb milling) or out of (conventional milling) the hole made by the drill. They will be creating the flat bottom surface of the dovetail. With the saw cut, the amount of material being removed on that flat bottom of the dovetail will be a lot less and the heat will be able to escape the area where the tip is cutting a lot easier. So the tip will stay cooler during the cut and that should help a lot.

The drilled hole will remove any worries about the male dovetail bottoming out in a rounded bottom angle of the female dovetail. It also reduces the stress riser at that point.

Click to expand...

Well, you can actually do it so that the tips never have to cut. For simplicity of description, suppose you drill your hole centered right at the intersection of the bottom and the sides of the dove. Then straight mill, chain drill, or saw out the "mid portion" of the dove---the part you could reach with a conventional straight end mill. Then saw out the remaining two triangular portions coming safely close to the scribed lines of the dove. Now you can alternately cut with just the bottom or the side of the dovetail cutter with the tips always taking a free ride in the drilled hole. You don't ever have to have the bottom and the side of the cutter both cutting at the same time. And the tips never have to cut.

Denis

I’ve been cutting quite a bit of 4140 prehard and 17-4 recently on the lathe and have had great results at 700rpm (feed set slow). I’ve been using my cheap Chinese hss coated inserts at $4.99/10pk. I was getting my best with cut compressed air cooling while dry cutting. Anytime I used cutting oil it would get hot and discolor and make more smoke than help in cutting. Coolant isn’t connected yet because this lathe is new so I can’t advise. Cuts like a dream dry and I have a new rotary broach holder, r8 arbors, straight shanks, revolving tool holder, etc... I even machined the 17-4 after heat treating to clean up discoloration. Granted it was obviously more difficult yet everything came to a shiny finish when I was done. I haven’t had to use my cbn inserts yet so I will save those expensive inserts for when things get finicky. One thing I did notice you have to have it chucked in firmly and a stout machine and don’t forget to take deep cuts when you can. Light cuts the inserts will tend to back off as it travels. Anything less than a 12” lathe will likely need everything you can throw at it. I’ve got a 13x37 with d1-4 spindle so it’s as rigid as I need for these materials. I had the most difficulty drilling, tapping (a tap broke), and boring holes. Next time I will be sure to drill my holes before hardening. I was a little excited and preemptive before I realized what I had done and my straight shank broach adapter was a solid 55hrc after heat treating :-(. I will say that those Ebay cheap inserts have been hit and miss for me. I’ve had a couple Chinese suppliers where I’d use a 10pk to cut one part and this recent purchase I only went through 2 inserts cutting up 12” of 4140ph and 17-4ph. Definitely going to buy more inserts from them and hope the same results.

72bwhite said:

I need to make a holder for a from cutter
for my cxa tool post so my question is
will the hss dove tail cutter do ok in
4140 prehard around 32rc ?

or should I machine it and then heat treat it?

and then for the profile cutter A2 or O1?
only cutting 6061 with it

Click to expand...

.
you got more than one dovetail cutter ?? as someone who has made many tens of thousands of parts my experience is you do things differently based on spare tooling amounts and if it is ok or not ok to scrape the part and have to remake it

look at the original date.

made the tool and the part over a year ago.
just cut the form tool out of a piece of A2 and clamped it in a
CXA 1 holder.