side cutting slitting saw use, feed speed?

[LarryMck]

I need to cut a slot centered in 3/8 x 1" wide 304 stainless. The slot needs to be 5/8 inch deep 5/64 wide and runs through the 1" width. I have very little experience using slitting saws. I do not have cutting oil on my mill but I do have it on my lathe. The slitting saw I have is 4" diameter.

If I use my lathe I will need to make a jig to attach to my cross feed and an arbor for the slitting saw.

I have an R8 arbor for my Bridgeport that will work but no cutting oil. I have a about 12 pieces to make that require the use of the slitting saw.

Can I make the cut in one pass or do I need to do it in multiple passes to get the the 5/8 depth.

Should I use the power feed or feed it by hand?

Off course the two things I am trying to avoid in getting the stainless hot and work hardening it and damaging the slitting saw that I just purchased.

Thanks

Larry

[Harold_V]

I need to cut a slot centered in 3/8 x 1" wide 304 stainless. The slot needs to be 5/8 inch deep 5/64 wide and runs through the 1" width. I have very little experience using slitting saws. I do not have cutting oil on my mill but I do have it on my lathe. The slitting saw I have is 4" diameter.

You may not have the ability to pump oil on your mill, but nothing prevents you from brush applying cutting oil. Keep the blade wet (sulfur based cutting oil) and ensure that you do not exceed 70 RPM. A little slower would be wise, assuming you don't use flood coolant. 304 stainless is not tolerant of over-speeding when using HSS.

Can I make the cut in one pass or do I need to do it in multiple passes to get the the 5/8 depth.

If your setup is rigid enough, you should be able to make the cut in one pass. I'm assuming you have a side cutting slitting saw, not a screw slotting saw. Chip clearance of the teeth can become an issue with the latter.

Should I use the power feed or feed it by hand?

Power feed is far more reliable than hand feeding, and can prevent work hardening, assuming you select a respectable feed. You'll have to consider the number of teeth and the RPM at which you operate the cutter, which will allow you to select a feed that is acceptable. I'd suggest you don't go below .002" per tooth, and that may be all you should consider if your setup isn't quite rigid. Make damned sure you aren't climb milling.

Off course the two things I am trying to avoid in getting the stainless hot and work hardening it and damaging the slitting saw that I just purchased.

You can expect the stainless to get hot--but hot is a relative term. If you exceed the maximum speed, you'll create unacceptable heat at the tip of the cutter, which will result in rapid edge failure. Watch the chips coming off. They should not change color, not in the least. If they do, you're running too fast, and the damage may already be done. With stainless, which is very unlike aluminum, you're better served starting out a little on the slow side, assuming you have any doubts.

If you find that .002" feed is acceptable, you may be able to increase a little. Don't get caught up using too little feed, as that can lead to work hardening. The cutter must make a chip with each tooth, and do so repeatedly. If it does not, you most certainly will experience some work hardening.

Harold

[seal killer]

Harold--

I have little experience slitting. I have many saws with no side clearance and one from Niagara with side clearance. I have slit aluminum and 1018, but I am FAR more timid with the saw than you recommended to LarryMck. I usually take no more than 0.030" per pass. My mill is rigid. Should I experiment with a greater DOC? (I never climb mill with a slitting saw.)

--Bill

[ctwo]

Harold--

I have little experience slitting. I have many saws with no side clearance and one from Niagara with side clearance. I have slit aluminum and 1018, but I am FAR more timid with the saw than you recommended to LarryMck. I usually take no more than 0.030" per pass. My mill is rigid. Should I experiment with a greater DOC? (I never climb mill with a slitting saw.)

--Bill

seal killer, Harold provided excellent advise on individual tooth chip load. The short answer I would guess is, it depends. It seems DoC is not the main consideration, but a single factor of many to consider. Before I read his post, I likely would have just gone over-conservative and taken shallow cuts, and that would likely result in most of the teeth just rubbing on the work at any given time.

Now, I'm off to figure out a formula to add to my excel spreadsheet that can take saw diameter, number of teeth, surface cutting speed, and then pop out a feed rate and RPM. Somehow I think DoC is in there too. Hmmm...

[Harold_V]

Harold--

I have little experience slitting. I have many saws with no side clearance and one from Niagara with side clearance. I have slit aluminum and 1018, but I am FAR more timid with the saw than you recommended to LarryMck. I usually take no more than 0.030" per pass. My mill is rigid. Should I experiment with a greater DOC? (I never climb mill with a slitting saw.)

--Bill

In my opinion, yes, you should. A .030' depth of cut is very wasteful of time, assuming that is a consideration. It also adds a huge amount of mileage to a cutter unnecessarily, drastically shortening its useful life. Key, here, is tooth design. If you're using a screw slotting saw, which have a large number of shallow teeth, depth of cut will be restricted, as the gullet may fill before the tooth leaves the cut. Also, depending on the width of the saw, and the nature of the material being machined, deep cuts may wander. They do so, regardless of depth, but as the cut deepens the blade can bind. Each case would be its own, as what works with one combination may or may not work with another.

In regards to a wandering blade, I had occasion to cut a .010" wide slot about ¼" deep in little circles of copper, quite thin. Each disc had two slots, located in line with one another, cut from the outer edge towards center. These discs of copper were grit blasting masks for use in building gyroscopes for guidance systems. Blade wander was a huge problem, so multiple passes were taken, each only .050" in depth, with the blade reversed for each pass. That kept the slot straight. As a large number of the thin discs were mounted in a holder, the time spent reversing the blade was amortized over many pieces. Resorting to this process reduced the price of the item from $10 each to just $2.00 each for the customer.

If you take note, thin blades, screw slotting types, have relief, but it's achieved by hollow grinding.

Harold

[LarryMck]

First of all thanks for all the help. While i have learned so much from all the post on this forum I am amazed at how much I don't know. But I am getting smarter about asking a question or looking at old post for an answer. Burning up a $50.00 tool will make you want to get an education quick.

Now for a couple more questions:
My slowest spindle speed is 80 RPM so i would calculate my feed speed as follows:
.002 per tooth X 36 teeth x 80 = 5.76 inches per min.
I will have to set my power feed with a stop watch since I have an old DRO that does not display this.
Note my saw is 4" diameter.

I took a couple pictures of my potential set up. I was going to mill the aluminum base so it will have 2 square edges to seat the parts against.

I also included a picture of the drawing. I thought the first step would be to cut the slit in the part.

[NP317]

That piece of corrugated cardboard will allow motion of the parts being cut.
I suggest clamping them straight metal-to-metal.
Rigidity is your friend when machining, especially for the slotting operation you are going to perform.
~RN

[Harold_V]

What NP317 said. Don't even think of taking a cut like you need with cardboard in the setup. In fact, don't rely on a bar to hold each piece, as if there's any variation in thickness of the parts, or the bar isn't flat, you'll have movement of one or more of the parts. You'll kiss good bye your cutter in a heart beat. If the fixture allows for it, place multiple step clamps on top of the bar, as close to one another as you can. One on top of each piece would be best.

Don't run that saw at 80 rpm in 304. It won't hold up, and may fail quickly.

One is generally not free to make changes to a part. However, if you can substitute 303 S for 304, you can probably get away with the 80 rpm. If this project is for others, don't substitute without their permission, as 303 does not have the same chemical resistance as 304, and that may be a factor in how the material was chosen.

If you must stick with 304, you'd be well served to purchase a smaller diameter blade, assuming it will provide the necessary clearance. You'll be able to use the 4" one for aluminum or other less difficult to machine materials, so all is not lost.

Harold

[GlennW]

I thought the first step would be to cut the slit in the part.]

I would mill the end of the stock flat and square, and the pieces to the proper length first. That way you can accurately cut the slot to the proper depth.

[LarryMck]

I thought the cardboard or some thick paper was a good idea because of the variation stainless steel flat bar that I am using for the parts. I guess that was a bad idea.

I will rethink my set up jig. I may just machine one part at a time. My Bridgeport slowest RPM is 80.
I do have a Van Norman No 12 mill that I don't have up and running yet. It was a rescue machine from the scrap iron. Got it at an auction. The only person bidding on it was the local scrap guy. I just could not let him take it. I have started cleaning it up to prep it for paint. I just don't have a lot of tooling for it and it is not all that easy to find. I do think I have an arbor for the slitting saw.

Maybe it is time for a test run.

[Harold_V]

I thought the cardboard or some thick paper was a good idea because of the variation stainless steel flat bar that I am using for the parts. I guess that was a bad idea.

Given the fact that material tends to vary in thickness, I can understand how you'd make that decision. Problem is, thin pieces will not receive the required clamping pressure, so they'll shift in the cut. That usually spells doom for the cutter, as it will be pulled in to the cut, making it impossible for the cutter to remove the amount of material presented. That will stop the cutter dead, resulting in a broken cutter. Even if there's a key that can shear, the continued table feed will ensure breakage.

If you take the cut to full depth in one pass, I'm sure you can see that the cut begins at the tip of the part. The motion of the cutter results in a strong lifting force, which would pull a loose piece out of the fixture. That's the problem with using a single bar to restrain the parts. However, if you can place a clamp over each one, that won't be the case. Running them singly, or in pairs, will work, however. In either case, it 's still quite important for you to clamp them adequately. There's a lot of resistance to the cut, which translates in to a pulling force on the part.

The VN mill would be better suited to this operation, assuming you can get it operational. Having support at each end of the saw blade is always a good idea, and the general robustness of the VN as compared to a BP is a huge benefit. Besides, it may have the capability to provide flood coolant, which would be a distinct advantage.

Glenn provided good advice. Start with blocks finished to size, so you can use any feature to hold and orient the parts. That's good shop practice.

I'd be interested in hearing how this all shakes out for you.

Harold

[LarryMck]

I did it. Got all the oil changed, replaced sight gauges, made new jaws for the vise, lubed everything and a quick cleaning, now it runs.

Using Harold's recommendations on the slitting saw I was able to make 10 slits in 304 stainless without a problem. Thanks for the help.