[Kingjamez]

I've got to make a .25"(w)x7"(l)x1.5"(d) slot. I was considering roughing out the slot with a 1/4" twist drill at .26" spacing then finishing the slot with a long endmill. Is that a reasonable approach? Any reason just to slot with a extra long endmill instead?

-Jim

[draughted]

can you give us a solidworks rendering?

[keebler303]

A slitting saw might work better for you.

Matt

[Cmailco]

Standard procedure for a slot like that with no particular finish considerations, within ±.010 is to simply slot with a 1/4" diameter 4 flute end mill (3 flute if non-ferrous) to the length-of-cut (5/8-3/4" down), then run the rest with a short length-of-cut end mill with 1.5-2" reach... the closer to 1.5" the better but you may have to go 2" to get an off-the-shelf grind. They're typically ground to ~.230" behind the flutes for whatever the length specification is.

Follow the manufacturer's recommendations for axial depth of cut and inch/tooth.

[Kingjamez]

Thanks Cmailco. Here is a jpg of the slot I'm trying to make. Are there any merits to doing a plunge rough with a twist drill and then cleanup with an endmill? It seems like that would greatly reduce the extremely light passes I'd have to make for the last 1" or so of the slot.

-Jim

[Cmailco]

Thanks Cmailco. Here is a jpg of the slot I'm trying to make. Are there any merits to doing a plunge rough with a twist drill and then cleanup with an endmill? It seems like that would greatly reduce the extremely light passes I'd have to make for the last 1" or so of the slot.

-Jim

Jim,

Hate to answer with a question but I'm curious to know; is this a production run? How many do you need to make?

What's the workpiece material?

Thanks,
Chuck

[Kingjamez]

It's a small production of 10 or less units and I'm doing it on my CNC'd X3 bench top mill. The material is 6061.

The slot above is just part of the job, there is another 4 hours of machine time for each part. I'm trying to minimize time everywhere I can.

-Jim

[Karl_T]

FWIW, I quite often chain drill when doing deep narrow slots. Works well for me.

karl

[Kingjamez]

FWIW, I quite often chain drill when doing deep narrow slots. Works well for me.

karl

It's worth a lot. Thanks!

[Mcgyver]

FWIW, I quite often chain drill when doing deep narrow slots. Works well for me.

karl

x2 , drilling is one of the fastest most efficient ways to remove material because the work is balanced torque along the spindle axis with almost no lateral loads on the machine...in other words the set up is the most rigid it can be permitting the highest removal rates ....and as you'll get say 100 sharpenings out of a drill its very inexpensive as well.

[MikeZee]

The slitting saw, I like that the best - probably where I would start. 1/4 end mill x 1.5 Lg. the slots gonna look s#$t by the time you're done.

[neilw20]

Lots of drill holes 15/64" or 7/32" to remove most of the material,
then passes with a 6mm end/slot mill.

A 3 flute one will run more smoothly (IMHO)

Then some final passes climb milling to give the final width of 1/4"
The reason for the 6mm and not 1/4" mill is so that it is always climb milling.
Lots of flood coolant to keep the chips from being regurgitated.
Make DOC about 3mm so as not to overload the cutter.

With the flood coolant you can run 3000 rpm or so, if your spindle will go that fast.

To identify the best feed rate examine the chips, and listen for smooth cutting.

Solid carbide will work better, but it won't take kindly to overloading on intermittent cuts.

Finishing pass with too much chip load will not give straight sides because the cutter will bend.

[jamesu229]

Mitsubishi makes small diameter feedmills that would be great for this. 6mm would be perfect for roughing and then use a .25 finisher

[Cmailco]

Drilling always seems like the faster method till you put the math to it.

Take an 8" long (center to center) slot, 1.5" deep, 3.07 in³ of material, drilled to a depth of 1.48".

32-34 drilled holes (.242 or 15/64 diameter drills respectively) @ 250 SFM, .006-.008 inch/rev, no thru-spindle coolant, minimum of 5 pecks adding some 2.5 seconds to each hole operation.

At .006 inch/rev, that's 3.75 seconds per hole + 2.5 seconds for pecks + 1 second repositioning chip-to-chip (fast machining center) or 7.25s per hole x 32 holes = 3m 52s or .79 in³/min material removal rate (MRR).

And you still need to 'mill' the slot...

Now drill two holes to 1.48", one at each end, center of radius; this takes 12.5 seconds using previously calculated data and we'll add 4 very generous seconds for repositioning or 16.5 seconds.

Plunge 1/4" 3 flute end mill (3/4" LOC) at the drilled hole, mill to the other hole and plunge again, no retract, etc., etc..
450 SFM, .002 inch/tooth, aDOC = .125 or 6 passes to .75" depth. Our material removal rate is 1.3 in³ and we're taking half the total material volume (3.07/2 for 1.535 in³) in this operation: 1.535/1.3 = 1m 11 seconds + 6 pecks @ 1.5 second each = 1m 20 seconds

+8 seconds for a tool change = 1m 28 seconds

Second tool is a 1/4" 3 flute end mill, reaches 1.5" with .5-.75" LOC... the shorter the LOC better for tool core rigidity.

SFM & inch/tooth reduced to 75% for this tool, aDOC = .0625 for .4 in³/min MRR. 1.535/.4 = 3m 50s + 12 pecks @ 1.0 seconds each = 4m 2s.

Drilled plunge holes at ends = 17 seconds
Tool 1 = 1m 20 seconds
Tool Change = 8 seconds
Tool 2 = 4m 2 seconds

Total time to slot = 5m 47s vs fully drilled & milled slot @ 3m 52s... so you'd need to mill the slot in 1m 55s to produce it in the same amount of time. Considering that it took 1m 20s with a very rigid tool, I don't think your chances are that good. Calculate the time with an OSG "Blizzard" 3 flute end mill: .25" LOC, 1.125" reach, and the times lean even further towards milling vs full-drill/mill.

Just making the point that drilling is not always the faster process. If we had thru-spindle coolant, things would certainly change a bit as we could easily drill these holes to depth without pecks, but then we'd probably be operating with a lot more rpm as well. Either way, it's always worth a little napkin math to find the faster process.

On a slow machines, pecks, clearance planes, rapids; lots of out-of-cut time operation, really kills the times.

*Granted, this example may not directly relate to the situation here but it's geared more towards "general" process costing, fwiw.

May not even be feasible, depending on slot tolerance, etc..