A few machining questions!

Keith_H

Keith_H

Joined
Jul 20, 2007
Messages
3,121
I have some questions about machining, particularly using a milling machine.

I have to make some 1/2"x1.5"x12" pieces for my kmg clone in my high school shop class. So far I have cut two strips off a large 1/2" plate with oxy-acetylene, rough ground the edges, and machined them on our milling machine.

I have been using a 3" hss slab mill bit and conventional milling. My problem is that the strips are not wide enough to sit in the vise, I have tried to raise the piece up with a metal strip, but they didn't sit flat and I had to re-do them by cutting off another strip :mad:. Right now I am clamping half in the vise, doing one side, then flipping it around. Very painstaking.

Is there any other way of clamping it to the bed? My shop teacher said I could use a piece of wood to raise it in the vise, but most of the time says just to forget about it and get some 1.5" tubing :rolleyes:

Is it possible to use the side of a vertical mill bit? All of the bits in my school shop dull, some are so dull it is embarrassing. I am jealous of Nathan the Machinist's thread about drilling into a file.

When these plates are done, I will have to bolt them together to form a box for the tool arm. Can I drill that deep in the milling machine or do I have to use the drill press?

Another question, the milling machine vise is really hard to turn in the last inch, I blew it out with air and gave it oil, but i would still have to give it my weight to turn it shut. How can this be fixed? I have a block beside my piece in the mean time.

Thank you!
 
I'm not following the problem maybe. The size you need is available already. Cant you just go buy some 1/2" x 1 1/2" bar and cut it to 12" lengths?

There must be something wrong with that vice. It should close all the way.
 
thanks Bruce, I bought the plate at the scrap metal place, maybe I should have looked harder for the bar.
 
The vise may be missing one of the "soft" jaws or both.
Yes you can mill the piece on the bed. You'll need to put some kinda backer under it ( 1/4" masonite works well). Next you need a means of squareing it to the bed/mill. Lots of folks use 5/8 Dowel pins as what they call "feathers" wedged in the rear-most way. On most mills I've used this seems to be the correct size to just barely fit in the ways. You'll also want to clamp the part from this same way, so plan ahead with the placement of your T-nuts. With the part clamped securely in this manor, you'll be able to machine 3 of the 4 sides form this one set-up, then flip the part, reclamp and cut the last side to your final dimension. Most of the steel I've had to mill really prefers to be conventional milled. Leaves a better finish. Don't forget the oil.
Also remember to de-bur the part before reclamping. Those burs can really screw you if you don't clean then up first.
 
Im not sure if I follow- the dowels fit in the slot and the bar sits up against it? I only need to mill the bars parallel, I am almost done, but its the last pass that counts IMO, so i have to get it right!

(I actually had the pieces done, but they were both about 30-40 thousands of and inch wide so I thought I would touch them up- that went over like a lead balloon)
 
Yeah, you pretty much got it. Make sure it's snug against the dowels, and doesn't creep out as you tighten the clamps.
 
Keith_H said:
I am jealous of Nathan the Machinist's thread about drilling into a file.
Click to expand...


I'll point out that cut was milled, not drilled. The hole was 1/4", the cutter .157". It don't think I could have just plunged straight down in that application.

The new guy, little mac, has it right. You need to clamp to your table.

If it were me, I'd eyeball it along a Tslot and clamp it and cut from one side, add clamps from the other side, then machine the far side. That way it is done in the same setup and you don't need to worry about cutting a taper. Though his way is faster and lends itself to a run of several parts.

A 3" cutter is too large for side cuts in steel on any mill you're likely to have access to. I'd stick to a 1/2" four flute.

You need to raise the part above the table. Whatever you use, it needs to be fairly flat. I don't recommend lumber.

Most "dull" cutters are clapped out over the first 1/4" from the end. If you raise your part by half an inch and run your cutter 1/16" above your table you'll be using a less dulled area of your old cutters.

You should try to make your first cut about .010 in a conventional cut. Then a .005 finish pass as a climb cut. If your mill is badly worn and your cutter dull it won't climb cut well, so drop back and punt. But otherwise you should see a better finish this way.

Then cut the far side. Add clamps on one side, before you remove the other clamps. Make a skim cut, measure, calculate a cut to leave .005 and make a rough cut (~700 RPM), measure again, make your finish cut.

Because your finish cut is a shallow cut, you can crank the spindle up to about 1,200 RPM on a half inch HSS cutter for a better finish. (slow down your RPM if it squeals). Wear sleeves...
 
Thanks for the comments, guys. I talked to my metalwork teacher today and he told me no, and to just place a piece in the vise to raise it up using the horizontal 3" bit (im not sure if it is called a called slab mill). He says that we don't have the right clamps, but we have lots of those T-shaped bolt ends and those stepped block things (I have never been taught about them) I think that it can be clamped easy.
 
Are you using a horizontal milling machine!? If so, disregard the above advice, it was assumed you were using a vertical mill.

If you're using some old school stuff in your shop, the best way to flatten these things would be with a shaper. Now that's old school...
 
Shapers.... MMMMMMMMMMMmmhhhhh I love shapers I can hear them still ... KERCHUNK, slap, KERCHUNK, slap, KERCHUNK, slap!

1938_atlas_7_inch_shaper.gif
 
I thought that a milling machine was a shaper...

It is a turret type milling machine with both the horizontal and vertical.
I like the machine, except that the left hand side x-control is stripped completely, the auto feed is broken and the vise is partially broken. :)
 
Last edited:
1938_atlas_7_inch_shaper.gif


I had one of those in my highschool class , maybe a bit newer, maybe not...

At an auction I saw a working mini shaper that was done as hobby project about 4 feet long.
Would you believe it went for a few thousand, while some useful big iron went for scrap?
 
I switched the machine over to the vertical machine today, (I talked my teacher into it :)) I have a sharp sided 4-toothed bit that I am using (3/4") I hope that the machine will clear the clamps.
 
I set up the milling machine the way recommended, and have a few more machining questions.

I am turning the 4" drive and tension wheels on a lathe, but am not certain on the details.

So far, I have planned out that I will cut off a workable piece with the bandsaw off my aluminum round bar, then square the ends in the lathe, cut a counter bore for the inside chuck, drill out the shaft, cut the area for the bearings, then machine the wheel surface. 1. Anything that is wrong with that?

2. How do I do the crown on the wheels? (all I have done is a straight cut)

3. I am not sure how to fit the bearings in the wheels, should it be the exact size to the 0.001" then pressed in?

4. How should the keyway be cut?

I hope I am not taking advantage of you guys, but this is such a good resource! Thank you!
 
and if it is too much to ask, can I drill deep holes in the milling machine? I want deep 1/4" holes but our bit are regular size, can I use normal drill bits in the milling machine?
 
Now you're looking for trouble, especially on a high school metal lathe. It can be done a variety of ways, pending the tooling you have available for the lathe. Problem is most chucks don't run true after they have been tightened on stock that isn't perfectly round. Very few chucks can be re-adjusted to run true. A four-jaw chuck might be a major help here. If the chuck isn't running true, the center of your cut will change when you remove the part and turn it around to do the other side or even if you remove the part to check something and put it back. The cut is only true as long as the part is in that exact position. Might be possible to turn between centers but set-up might take a while and if someone uses the lathe between sessions you gotta at least check the set-up again and proably start over. Many lathes are not leveled properly and the result is a slight twist in the bed, If you lock down the tail stock and center it, it's only good in that same exact position on the bed. This is a major night mare if you have to share the lathe with other classes.If you decide to continue, I suggest you do as much as possible from one set-up (the last set-up). First face the first end and make the undercut for the inside jaws. Turn the part around and do all of the rest of your cuttiing from that position without taking the part out. Bearing bores can be tricky things and maybe Nathan will chip in here. I have yet to machine the wheels for my clone, but I have been considering boring the bearing hole all the way thru and then pressing a sleeve in the center to act as a bottom for both bearings, but a means of retaining the bearings is still to be worked out. Keyways in the wheel are usually done with a broach. I've done them with a fabricated broach. usually a square tool, with the business end ground at an angle like a chisel. A method of holding it might be a bit of a challenge, but it can be done. Once aligned on the centerline of the bore ( on the mill usually) you move to the interferance point and make a plunge all the way thru, then move 5 to 10 thousandth further and plunge again. Keep doing this until you have the appropriate keyway depth.
The deep holes can be done on the mill, but you migt have to drill from each side and you must be careful to keep track of your referance corner and either place the holes exactly on the measured center of the stock thickness or reset the zero from the same edge after you turn the stock over. Drill a little and clear the chip, drill a little and clear the chip ( peck drilling) will help keep the hole going straight. Use plenty of oil and mind your speed and feeds. Most folks tend to run the drill way too fast which will burn up the bit in a heartbeat.
 
thank you for the reply, little mac. I doubt that our lathes are level, they are pretty nice lathes, but there is play in the adjustment wheels and some parts are a little worn. There is a lathe set up with a 4 jaw chuck in my shop class but the inside jaws look a little big for a bore in a 4" wheel. I will check do see if we have a broach for the keyway. The reason that I want to know if I can do the holes in the milling machine is because they are all in line and it would be nice to try. I may just use a drill press. I am paranoid of other kids messing with how I have my work clamped in the milling machine, I only get 40 mins (77 counting start and clean up) and sometimes I have to leave my piece in there for the day!
 
You are going to have difficult achieving the necessary precision to make a good pulley in your school shop.

Also, bearing press fit is tricky. For this application, you probably want about .001" interference.

Like little mac said, a sleeve can be put inside the part for shoulders for the bearing. You might JB weld that sleeve in place.

If it were me, in your situation, I would:

1: Put the part in the lathe and turn the diameter close to size and face one end.

2: Saw the part off the bar, put it back into the chuck and face the other end.

3: In that same setup, drill, then bore a hole for the bearings all the way through the part.

4: when you have time to finish this next operation from start to finish in one setup, this is where all your precision will come from. You should probably have a few parts ready to go before going to this point. Turn a mandrel that you can mount your simifinished parts to. It will have a shoulder on one side for the part to sit against, a smooth section that tightly fits your bore (sliding press fit) and a threaded end with a hole for a center. You put your part on it, a washer and a nut (to chinch down your part), then run in your center. Because this was all made in one setup, your concentricity to your face and bore should be perfect. Take your finish cuts on the OD of your parts. The crown can be cut with your compound rest set to about 1 deg to one side, then 1 deg to the other side, meeting in the middle of your part. Turn the very center flat for about 1/8". I'm pretty sure that will work well for a crown on this part. BTW, there is no need to make a extremely fine feed and try to get a wonderful finish on these parts. They left coarse machining marks on my KMG, it is probably like that for a reason.

Once the mandrel is removed from your setup, you won't be able to return it and maintain perfect concentricity. So get it all done at one time. If in doubt, rough out a mandrel on one day, then install it the next day, take your finish cuts, and then get started on your parts.

For your keyway. You can grind a parting tool to cut on the end, rather than the top, and use that to "broach" a hole in a lathe a few thou per pass. You lock the spindle, turn the tool on its side and shim it up to your centerline and start shaving.
 
The mandrel is 2" wide or 1/2"?

I found this video very helpful, even though it is cnc.
http://www.youtube.com/watch?v=klzHjz1_G78&eurl=http://www.beaumontmetalworks.com/videos.html
does anybody know exactly how rob does the idler wheel, Nathan's way sounds great but I am curious about how he does them.

This week was the first time I have used a sharp bit on the milling machine, it was like seeing a beautiful woman after spending years stranded on a desert island...

I think i will use the forgotten HSS lathe bits because they are sharp, the carbide bits we use are pretty dull.
 
You must log in or register to reply here.
Back
Top