milling slot question

I've got a little job I need to do/get done. I am working on the wing
strut fittings for the bush-plane. There are 4 struts - so 8 strut end
fittings. They are made of 1X1 6061T6 - 4 abot 4 1/4 inches long, and
4 about 5 1/2 inches long.
2 need 1/4 inch slots, 4 need .195" slots, and 2 need 3/16 " slots -
all 1 3/8" deep.
I may have the use of a bridgeport style mill that used 3/8" shank
cutters, and I have located a 3/16" end mill that has 5/8" cutting
depth (end mill)
How close to 3/16 will I likely be able to get? (thinking the cutter
is going to want to "walk" a bit in the cut) Would it help a lot if I
drilled a row of 1/8" or 5/32 holes down the center of the slot first
to reduce the chip load????
Or do I just farm it out to a CNC shop??
If I had access to a horizontal mill it would make life a lot easier,
but nobody has them any more.
Reply to
clare
Loading thread data ...
snipped-for-privacy@snyder.on.ca fired this volley in news: snipped-for-privacy@4ax.com:
How do you figure to get a 1-3/8" deep slot from a cutter that only has a 5/8" cutting depth?
If you take the cuts in shallow increments, AND you don't have any play in your spindle, you should be able to get within a half-thou. of the cutter diameter, or so.
But not that depth!
L
Reply to
Lloyd E. Sponenburgh
I think I would do it on a table saw. You could try making one out of wood and see how accurate you can make the slots.
Wear eye protection
Dan
Reply to
dcaster
formatting link

Reply to
Jim Wilkins
I'm going to assume the slot depth is 3/8", not 1-3/8". While the 3/16 end mill may cut close to .188, as measured with a block or pin, unless you have flood coolant with plenty of velocity available (unlikely on an un-enclosed mill) the sides of the slot will be quite rough. I'd use a 5/32 2-flute cutter. Bring the slot to within .010 of depth with a couple passes with the cutter on center line. Widen the slot by offsetting the cutter about .005 per side and measure the result. Set your final offsets taking into account the result of the previous cut and bring the slot to final depth at the same time. You can climb mill the final passes if you find you get a better finish that way. Brush on some alum-tap or kero or WD40 before each pass.
Don't bother with the drilled holes unless the slots have blind ends. If they do, a hole to depth at each end gives the end mill a place to dwell at the ends without rubbing, and acts as a visual cue.
Not knowing the condition of the mill it's hard to predict how close you'll get, but with a bit of care I'd expect to get within 3-5 tenths on my DRO equipped pretty-tight mill. Within a few thousandths without paying a lot of attention.
Reply to
Ned Simmons
From those details if you want to do the job I would have thought you would be better off using an arbor and a slitting saw or side and face cutter.
Reply to
David Billington
Lay the 1X1 in the vise, with the desired slot vertical. Mill the slot from the end to the stop-hole. Keep milling bit by bit 'till you reasch full 5/8" depth for the full 1 3/8" length of the slot. Release the vise and flip part end to end, reclamp and repeat, cutting from the other end, untill the depth of cut excedes 3/8" and there is no more metal in the slot.
Reply to
clare
The fun comes in holding the piece in place verticaly, cutting the slot 1 3/8" deep into the end of the workpiece while dodging all the flying hot and sharp chips, and getting an acceptable finish AND accurate slot width.. This needs to be "aircraft precision", not " lay it out with a crayon and cut with an axe" These 8 pieces keep the wing from folding up in flight, or falling to the ground on landing.
Reply to
clare
The cutter would have to be at leadt 2 3/4" plus the diameter of the arbor to do the job. Unlike an end mill, you can't cut to a straight end cutting through the 1 inch dimension, and you can't flip it over to cut from the other end.
I thought about trying to jig the parts up to slit the ends with the 14 inch cutoff saw (abrasive wheel) but the thought of loading the wheel with aluminum changed my mind on that pretty quick - not to mention the flexability of the fiber abrasive wheel..
A "cold cut" saw would work - it turns a bit slower than the average table saw, and the blade is made for cutting metal - but I don't have one and the quality of the finish of the cut would likely leave something to be desired.
Reply to
clare
The slot depth is the full 1 inch thickness of the stock, and the length of the slot is 1 3/8" The mill doesn't have a DRO. It is old but lightly used and well maintained. Being a 3/8" mill holder, it is almost impossible to buy an end-mill smaller than 3/16 with a length of 1/2" or more, which is required to cut the full slot, cutting from both sides. Our local machine tool supplier doesn't carry them, but an old machinist friend has a 5/8" long cutter from a box of cutters he bought at a close-out auction over 10 years ago - brand new never been used, that he has given me.
Reply to
clare
Cold saws are cutoff saws. With a few exceptions (Amada makes one such) they don't leave a great finish.
What you want, I think, is someone equipped with a horizontal mill who does a lot of slotting work. As for the geometry, shank-type cutters for a vertical mill can cut slots, but I've never seen one that could handle that depth. Arbor-type slotting mills are the tools that would give you the accuracy and finish you're talking about, and they're mostly horizontal-mill tools. They come in a wide range of diameters.
I'm speaking not as one who has done it, but who has seen thousands of milling cutters and tool setups -- run by other people. d8-)
Reply to
Ed Huntress
If I has an arbour and 3 inch (minimum) cutter that I could mount in the Myford I could do it, but I'd still have to figure out a way to square the end of the cut because it would have a 1.5" radius which may or may not be centered in the piece, depending how I managed to clamp the piece to the cross-slide. The bigger the cutter, the closer to straight the end of the cut would be.. Hard to move the part virtically toclean up the end of the cut.
I just talked to a friend from my highschool years who is a machinist (usually works a lathe on parts up to 3 1/2 feet in diameter and up to 20 feet long - both turning the outside and boring) and he said he'd set up on the "little" cnc mill and do them for me in his spare time over the next week if I just drop them off for him - So that's THAT problem solved.!!!
I've done a fair bit of computer stuff for him over the last few years, so now I'm getting "payback"
Reply to
clare
Just make a number of passes. Say 1/8" depth of cut at a time and if necessary use an air hose to blow the chips out of the cut. Use a cutting speed and feed rate that doesn't put a great strain on the tool.
In another message yo talk about this being a part on an airplane. I've made similar bits for military aircraft this way with no problems.
Reply to
John B.
You have a solution with your friend doing it. But do not knock using a ta ble saw with carbide tipped teeth for cutting aluminium until you have trie d it. It is noisy, but quick. And the finish is not bad. Try searching o n " cutting aluminium table saw ". You will get a couple of pages of links to that topic.
Dan
Reply to
dcaster
I've done it several times. I had a 10 inch "Beaver" table saw and used it to cut 2 inch blocks of aluminum for the engine mounts.(sold the table saw almost 10 years ago - did I mention we are 16 years into this build???) The whole garage was full of sharp shiny chips of aluminum.
I also cut some 3/16" aluminum plate for an engine cover - and that cost me over $100 for a new armature for my favorite circular saw -and spread chips all over the back yard. THAT cut was extremely noizy-.
The cuts were smoother than chopping with an axe, but would require a lot of sanding or grinding to make the surface quality I want for these parts - which would make any kind of accuracy very difficult.
Reply to
clare
O.K. That 1x1" -- is that square solid stock, or angle stock?
And the 1-3/8" deep suggests that the cuts are from the end, not through the thickness, even if it is solid square stock.
It should be able to use a number of other different shank diameters, presuming the availability of collets or end-mill holders in those sides. Most Bridgeports will use R-8 sized collets or similar end-mill holders (and the holders have the benefit that the end mill can't be pulled down into the workpiece as sometimes happens with collets.
Some (mostly old CNC Bridgeports) use NTMB-30 tool holders instead, and those also come in a number of sizes.
I'm not sure how common 1/8" end mills with 3/8" shanks will be. I would expect those to be 1/4" shanks or smaller, though you can probably get them with large shanks at extra cost.
You're going to need a number of passes first off -- and are limited to the 5/8" depth at best, so how you are going to get 1-3/8" deep cuts is open to question. If you mean that the slots will be 1-3/8" *long* instead -- that is easier.
In any case -- use something like WD-40 or kerosene as a cutting lube, and make sure that your end mills are two-flute center cutting ones. Yes, more flutes remove more material, but for slots, there is a particular benefit to the two-flute end mills. Yes, the end mill will deflect during part of the cut -- but that is when one flute is in the direction of the cut, and the other flute will be in air behind the cut. A four-flute or more end mill has flutes out to the side during the deflection while the one in the direction of cut is taking its heaviest cut, so the sides will show that deflection.
It is for this reason that the UK metalworkers refer to two-flute end-mills as "slot drills".
It might actually make things worse, as the flutes catch on the back side of the holes and try to pull the work deeper. If the milling machine has worn leadscrews and there is backlash this could be a problem.
Not *nobody*. I've got one. So does at least two other persons that I know semi-locally. (All hobbyists, FWIW.)
Good Luck, DoN.
Reply to
DoN. Nichols
Solid 6061T6
It is through the thickness, from the end, to make a "fork"
This one only has the 3/8" tool holder - all that has ever been used on it in over 35 years.
The cuts are through and through 1 inch, and 1 3/8" long, from the one end.
2 flute center cutting is what I have
The problem is nobody around here seems to have one. The one I know that used to be around here could only handle 2 inch cutters - not big enough to do the job (light duty mini hobby tool of some sort) - the guy that owned it is dead ond gone - no idea what happened to the tools.
Reply to
clare
O.K. Slots cut across the end and 1-3/8" from the end of the workpiece to the end of the slot.
There is a reason for short lengths with small diameters. They tend to break easily when longer.
Now -- you say it is a "Bridgeport type" mill -- and never say that it is truly a Bridgeport, so I may interpret that as meaning a vertical spindle mill of unknown size. If it is truly a Bridgeport, or a clone of the Bridgeport (there have been many), it should accept alternate end mill holders and not be stuck at 3/8" diameter. End mill holders or R-8 collets are both options -- and not that expensive to purchase for your friend if he does not have them.
You will probably do better with an adaptor arbor to accept horizontal milling cutters. Typical arbor diameter is 1", though there are smaller and larger diameter. A 1" arbor had clamping rings 1-1/4" diameter (and a key to keep the cutter from spinning on the arbor). It fits into the R-8 socket in the spindle of the mill. This produces a horizontal cut, so you will need the workpiece sicking out the side of the vise.
Now -- for 1-3/8" depth of cut, we need to take half the diameter of the clamping rings (0.625") and add to that at least the depth of the needed cut (1-3/8") which brings us up to a 2" radius (4" diameter) thus eliminating the smallest common cutters, which are 3" diameter. The other size which I normally see is 6" diameter, which would be plenty for your task.
Good Luck, DoN.
Reply to
DoN. Nichols
I would not recommend a circular saw for aluminium. But do use a table saw whenever it seems like the best way that I have. I have some sheet metal to keep sawdust out of the motor and it works for aluminium chips too. Th e aluminium chips are a big pain.
If you do not have any aluminium files, I would recommend getting one. The Type A is the best in my opinion. I have a bunch of files from Boeing Sur plus, but they do not work as well for good finishes as the Type A I bought many years ago.
Dan
Reply to
dcaster
And would never use them again. I'm not sure the brand and model of the mill - but it is european and the owner jokes he bought it from Noah's grandson.
And again, the tooling would likely never be used again - the mill is in the maintenance shop of a local leather products factory (belts) and is used to make tooling - I don't think they have added a "different" tool to it in 30 years - just replaced cutters as they wore or were damaged. I think all their tooling is Ti coated HSS - standard and short from 3/16 to about an inch diameter.
I am aware of that - I stated it would require a cutter of 2 inches plus the diameter of the arbour if I was going to do it on a horizontal mill, or on an arbour on my lathe - and the little horizontal mill that an old aquaintance used to have could only handle 3 inch cutters - he used it for cutting keyways in shafts and occaisionally making timing belt (toothed belt) sprockets..
Reply to
clare

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.