Milling Slots

[vtsteam]

I hesitate to describe this since the method may have been posted here before, or seem obvious, but it came up yesterday for me as I was milling four 3/8" by 2.5" long slots in some very tough (meaning poor quality) 1/2" plate steel.

I milled one slot by the method I used to use, which was basically milling the slot down about 20 thou deeper for each pass until I was through. Well, 20 thou into 0.5" is 25 passes to get through per slot. Each pass is slow on my old mill drill in this material. So it's quite tedious. It also puts a lot of wear on the sides of the flutes. Not only does the end have to cut, but the sides are continually rubbing with swarf as the cut deepens through each of the 25 passes.

Then as a comparison, for the other three slots I used a chain milling method with the same two-flute end mill. Basically plunging straight down 'til through, and then moving the table a little less than half the mill diameter further along the slot, and plunging again. Let's say I moved it over 0.15" per plunge on a .375 cutter. That's 17 plunges. Then I ran a cleanup pass down the length of the slot.

Each plunge takes maybe 1/2 the amount of time a slot pass takes. That's 17/25 x 0.5 = 0.34 or about 1/3 the amount of time slotting by the old method takes, plus a cleanup cut. This method also places most of the wear on the tip of the end mill instead of the sides, which is an advantage for me. In addition, swarf can always clear down the hole as opposed to building up in the slot with conventional slotting.

Since I have a very simple homemade end mill sharpener that is able to grind the flute ends, this slotting method greatly preserves the usefulness of my milling cutters by reducing flute edge wear when slotting. Well I think it also does reduce end wear as well, but I can't prove it.

The main disadvantage of slotting this way (with my machine's relative stiffness) is that the slot will have a slightly wavy edge with a single cleanup pass. I can take two cleanup passes, one for each edge so it looks perfect, but the slot will be slightly oversized. For the piece I was working on, the slot width wasn't critical so I did the two passes. I found a .003" cut per side did the trick.

Now this is not as great a disadvantage as it might seem, since I have a whole cardboard box full of donated machine shop end mills. Many of them have side sharpened flutes and are therefore slightly undersized. All I have t do with these is sharpen the ends, do the plunge slotting thing, and then two passes brings the slot to accurate size. And it takes just about 1/3 the amount of time of conventional slotting, while increasing the mileage before a re-sharpen of the end. For me that's a win-win. Or is it win-win-win....?

I hope this helps somebody else

[Lew Hartswick]

It's probably even faster if you use a drill for the "chain" drilling. A drill is the fastest way to remove material.  I have done that many times, of course it was on a Bridgeport.
   ...lew...

[mklotz]

Lew beat me to the punch but I'll offer this anyway...

Drills are the best bulk material removal tools plus they're cheap and easily resharpened.  Chain drill and then use the endmill to clean up the slot.

Use a 3/8 drill and move it one diameter plus a bit for each hole, say 1.1 * 0.375 = 0.413. Then you need 2.5 / 0.413 ~= 6 holes.

[vtsteam]

I'll try it Lew, but I'm not sure I could have milled easily between the much greater spacing required by drilling this 1/2" steel with my round column mill drill.

The advantage of using the end mill for my particular project yesterday (and possibly with other limited capacity hobby milling machines) was that the overlapping plunge cuts made the final slotting passes quick and easy, and the slots more accurate than simple chain drilling would have.

Aluminum, or a Bridgeport, different story.

[vtsteam]

Guys, I just gave it a try with .375" drill and chaining over .413 for three holes in the same 1/2" steel plate. The holes took a little over 2 minutes total to drill, then changeover to a fairly new US made carbide mill another minute. but after milling about a quarter the way between the first and second holes I had to stop because I didn't like the sound and feel. Definite warning signs of impending unhappiness.

I think for my particular machine, when doing difficult materials in sufficient thickness, I'm going to stick with the end mill plunge method. I appreciate your mentioning the chain drill alternative, and maybe it will work well for others. 

[crueby]

With my little Sherline I have combined the two on thick steel - chain drill, then do plunge cuts with a smallish end mill just to connect the dots, taking out just the narrow section between the holes. That lets me remove the center block, and come back doing side cuts to trim off the remaining scallop shapes to get a smooth edge.

[internal_fire]

I'm going to stick with the end mill plunge method.

Something I have done a few times is to chain drill first with a smaller drill and then follow with an endmill plunge. Most endmills are much happier using a starter hole when plunging.

Gene

[I see Chris beat me by 31 seconds.  ]

[crueby]

I'm going to stick with the end mill plunge method.

Something I have done a few times is to chain drill first with a smaller drill and then follow with an endmill plunge. Most endmills are much happier using a starter hole when plunging.

Gene

[I see Chris beat me by 31 seconds.  ]

I guess I must type just that little bit faster!   

[Jasonb]

The problem with using a similar size drill and then cutter is that you still end up with parts of the cut that mean full cutter engagement which is where lighter less rigid machines may struggle so end up having to use a shallow DOC for those parts which partly defeats the object of drilling first. I tend to use stitch drilling more for larger areas where there is a lump in the middle that can then be knocked out and you only have a max of 1/2 cutter diameter when clean ng up the edges. You can also find the cutter is pulled sideways in these areas of full width engagement

Faced with a similar slot I would tend to drill and plunge the ends to diameter and then run a smaller diameter 3 or 4 flute cutter down the middle which should allow a deeper cut and then finally offset until I get to width with full vertical depth cuts.

Recent example was this pair 80mm long x 8mm dia x 6mm deep.

First drilled 6mm at the ends and then milled out with 1.5mm deep ( 060" ) passes



These were actually part of a fabrication so roughing undersize also helped should anything move during soldering. They were then plunge cut at each end with an 8mm 3-flute cutter



Finally taken out to finished 8mm width with a pass down each side at full depth of 0.8mm and then 0.2mm stepover.

[Charles Lamont]

"stepover" = climb milling?

[vtsteam]

Great to read this variety of working solutions!   

[Jasonb]

"stepover" = climb milling?

No "Stepover" is the amount the work or cutter is moved sideways per pass

In that example I had a 6mm slot that needed enlarging to 8mm so that is 1mm per side. Work was centered then I used a stepover( or Ae, sideways DOC, etc) of 0.8mm followed by stepping over again 0.2mm for the finish cut.

Job was on the manual mill which I don't tend to climb cut on very much.

Had I been doing the slots on the CNC than I would have climb cut it all but taken a very different approach to the tool path. Though in a way a similar principal of using the smaller cutter to give a small cutter engagement rather than just ploughing up and down with a full width cutter.

This is the outer slot that that part fitted into, first remove the bulk by having the 6mm cutter move down in a helical pattern until it is right through the work as this is easier on the cutter than just plunging in, then it moves in a series of arcs with a depth of cut no greater than 0.6mm (10% cutter dia) This is a roughing operation so I left 0.3mm all round for clean up.

Then the same cutter goes round the perimeter to finish the cut in two passes, one  of 0.2mm and then stepping over a further 0.1mm for the final cut.

All cutting movements are climb milling, I could set it to do conventional or "both ways" but find it is happier climb milling.

[vtsteam]

I'm going to stick with the end mill plunge method.

Something I have done a few times is to chain drill first with a smaller drill and then follow with an endmill plunge. Most endmills are much happier using a starter hole when plunging.

Gene

[I see Chris beat me by 31 seconds.  ]

I guess I must type just that little bit faster!   

Actually, reading again carefully what you two described, they are different methods (I think). Chris is chain drilling and then plunge milling out material between the drilled holes, And I believe Gene is saying drill smaller holes where you will be plunging a larger milling cutter to make that plunge easier.

I think I'm going to try some of the described methods with the 1/2" steel plate and a 3/8" mill to try to find what works easiest for my machine and this material. That would give me a personal best method for similar situations.

[internal_fire]

Actually, reading again carefully what you two described, they are different methods (I think). Chris is chain drilling and then plunge milling out material between the drilled holes, And I believe Gene is saying drill smaller holes where you will be plunging a larger milling cutter to make that plunge easier.

You may have noticed that I said "a few times". 

I almost always use the same method outlined by Jason. Far more reliable for accurate dimensions.

Gene

[vtsteam]

I did see that Gene, and just thought it was a good general tip for plunging mills into difficult material with a light mill.

As far as accuracy goes, I would think any roughing method that allows enough material for two final passes to clean up the sides of the slot will have the same accuracy.