PDA

View Full Version : Slotting aluminum...bad finish...kinda.



browne92
12-27-2012, 10:46 PM
I'm making some new clamps for my POS Chinese CNC router (POS's are not limited to Bridgys :rolleyes:) and I'm cutting slots through 1/4" aluminum with a 3/16" end mill. I plunge, run the length of the cut, pull up. One side of the inside of the slot looks like metal always looks when I cut it with the side of an end mill. The other side looks smeared.

Is this just a product of one side of the mill cutting in the right direction and the other isn't? Or do I have some serious feed/speed issues? :confused:

I'm just a hack, so I'm going by feel as far as feeds and speeds. If you need to know the numbers, I can get them this Saturday when I make it back out to the shop.

lakeside53
12-28-2012, 12:09 AM
Are you using lube like wd40 to prevernt buildup on the tool. Numbers are important : what speed are you running? Are you climb or conventional milling - maybe both based on your comments? Have you tried staying with one or the other for both sides?

browne92
12-28-2012, 12:23 AM
Lakeside, I guess I'm doing both at once, because I'm only making one pass. Dry, wasn't using any kind of cutting oil. Again, I can get speed numbers, but not till Saturday.

For this project, it's not really important. Just wanted to know for future reference.

lakeside53
12-28-2012, 12:32 AM
OK, In missed the part about slot being the same width as the endmill. Try squirting with wd40 continously in sort bursts (not the aerosol can stuff; buy a squirt bottle). And.. try in say two passes deep, use a lightly smaller endmill and then a finishing pass.. etc.. You will generally get better results climb miling and using endmills smaller than the final slot.

Also.. what type of aluminum? Nasty gummy stuff or tough like 7075?

Black_Moons
12-28-2012, 01:26 AM
Recutting chips, smearing them into the opposite wall...

More lube, more air to blow out chips, or more passes so you can take a finishing pass that won't be cloged with chips to recut.

Jaakko Fagerlund
12-28-2012, 02:20 AM
The other side of the end mill is climb milling and the other is doing conventional, so the other side wall will look like asphalt as the chips are pushed in to it. If it isn't critical dimension, I would make the slot, then move the cutter a little bit (like 0.2 mm) to the bad side and come back to get a good finish.

Just FYI, on CNC one would use a smaller than the end radius tool to make such a pocket for the reasons mentioned - better quality, more room for chips to come out and climb milling.

Jpfalt
12-28-2012, 02:21 AM
When doing a cut like that, I predrill with a drill smaller than the endmill.

Then I plunge the end mill into the hole, raise the end mill, move the work about 1/8 to 1/4 the diameter of the end mill and plunge the end mill again.

I repeat this down the length of the slot.

When done, I place the end mill down to depth and do a finish cut from one end of the slot to the other.

I also use either kerosene or WD40.

This can really speed up the work on larger or deeper slots as the end mill can plunge at .002" per flute per revolution and helps minimize the deflection of the end mill that you get if you try to go sideways with a significant depth of cut.

J Tiers
12-28-2012, 08:55 AM
Agree on smeared carryover chips..... air will get them out, but also makes an unholy mess all over as the chips are blasted out in your face and all over. Doesn't matter where you point the nozzle., they still seem to fly all over..

WD seems to stick the chips to the cutter, making the issue a bit worse, although it does "poison" the surface so the chips don't weld-on as badly.

tdkkart
12-28-2012, 10:49 AM
Unless you can pull off some sort of magic and pull a miracle out of your butt, cutting a 3/16" slot with a 3/16" end mill will produce exactly what you are describing about 105% of the time, especially without any type of coolant, and with any machine that is not is PERFECT condition. In fact, depending on the length of the slot, I'm surprised you didn't ball up the end mill and snap it off.

Air, coolant, multiple passes, and a whole host of other things will increase your chances of success.

lbhsbz
12-28-2012, 12:31 PM
Like others have said, you're smearing chips. You're climbing on one side of the slot and conventional on the other side...this will always happen. Drill a pilot hole on each end of the slot, then plunge with your 3/16" endmill to establish the ends of the slot. Use a 1/8" endmill to machine out the slot, then finish one side at a time (light cuts) in whichever direction gives you the best finish. Use WD40 or some other light cutting oil, along with possibly some compressed air to help clear chips. If you finish one side at a time, you'll have a much better finish due to chip clearance around the cutter, as well as the finishing cut being in the direction that doesn't recut chips.

Bob Fisher
12-28-2012, 03:24 PM
When I need a precise width, which is seldom, I use a smaller end mill , preferably a regrind, and take finishing cuts. Regrinds are incredibly handy to have around. I'm fortunate to live near a reasonably priced cutter shop that sometimes has unclaimed cutters for sale, and I can get a quality end mill sharpened for about half the cost of a new one. Bob.

Oldbrock
12-28-2012, 03:42 PM
Speed should be 4000+ and try Relton A9. After you have finished the cut try retracing back to the beginning, the slot will be a few thou over because of the flex in the endmill but that with A9 should improve things. Peter

EVguru
12-28-2012, 04:15 PM
A vacuum cleaner can be very useful for clearing chips and doesn't of course spread them all over the shop!

majohnson
12-28-2012, 05:12 PM
Hopefully you get some 6061 its about the most friendly aluminum for use in standard machine tool. What type cutter also matters.

J Tiers
12-28-2012, 08:51 PM
Dunno about breaking the mill cutters....

I have used a nice sharp roughing cutter to slot before, when I wasn't particularly uptight about the exact size..... in mild steel, it cut about as fast as I felt like cranking the table..... slightly slower than the speed of "winding it back" for another pass.

OK, finish was a bit rough, but I'd bet you could clean it up nicely with a pass down each side.

Fasttrack
12-29-2012, 12:14 AM
When doing a cut like that, I predrill with a drill smaller than the endmill.

Then I plunge the end mill into the hole, raise the end mill, move the work about 1/8 to 1/4 the diameter of the end mill and plunge the end mill again.

I repeat this down the length of the slot.

When done, I place the end mill down to depth and do a finish cut from one end of the slot to the other.

I also use either kerosene or WD40.

This can really speed up the work on larger or deeper slots as the end mill can plunge at .002" per flute per revolution and helps minimize the deflection of the end mill that you get if you try to go sideways with a significant depth of cut.

That's interesting. I've never seen or read about this technique before ...

lakeside53
12-29-2012, 12:30 AM
I'm not sure I buy it. If it was more efficient that's how my cnc machine would probably do it (someone put a lot of thought into the tool paths/algorithms....) and it sure doesn't. If not roughing/finishing, for narrow it goes up one side and down the other. For wider- straight up the middle then both sides. Finishing passes run around the slot, climb milling unless there's a good reason. I don't have flood coolant so it's air blowing (via an old mister) and wd40.

Paul Alciatore
12-29-2012, 12:47 AM
I'm not sure I buy it. If it was more efficient that's how my cnc machine would probably do it (someone put a lot of thought into the tool paths/algorithms....) and it sure doesn't. If not roughing/finishing, for narrow it goes up one side and down the other. For wider- straight up the middle then both sides. Finishing passes run around the slot, climb milling unless there's a good reason. I don't have flood coolant so it's air blowing (via an old mister) and wd40.

What do you mean your CNC does not do it that way. You set it to "drill" a series of holes with the end mill and then you set it to do a slot across those holes. Bingo, it does it. If you use an end mill with a diameter smaller than the slot width, it would likely produce an excellent slot.

Besides, they are discovering new techniques every day. I recently read about drilling holes with a CNC by using a smaller end mill and a helical tool path. They claimed it both decreased the time for the job by a factor of two or three and increased tool life. Always room for new ideas.

lakeside53
12-29-2012, 02:26 AM
Maybe I should have been clearer. I can set my machine however I like, but it has a nice conversational mode where guys smarter than me have figured out many optimal ways to do things like slotting. I've also stared endlessly at many high-end cnc machines in production environments and never seen the drill/cleanup method used for basic slotting, and we are talking basic slotting here (not excessively deep wrt width, easy materials... etc).

The probem with the drilling a series of non-over lapping holes with an end mill then slotting is that it that burns z axis time for no advantage, and generates a lot of interrupted cuts. The post I was responding too did not generate much in the way of interrupted loading as he was stepping the end mill in fractions of the OD, but in doing so increased the z movement by a factor of 4-8 for each hole. A 10 inch slot say 1/4 wide steping by 1/8 or 1/4 OF a 1/4" end mill the would take about 160 - 320 plunges . I've done my share of manual machine slotting, and still do, so this isn't just about cnc, but basic technique. I sure wouldn't manually "drill a slot" as I just described. I also don't consider end mills to be very effective "drills".


If somone can tell me why it's a good technique over other approaches, I'm all ears.

Not sure what you were reading, but there's nothing new about drilling holes with a smaller end mills and helical pathing. I do that all the time and that's been around at least since the the 80's! Yes, there's most certainly always ongoing improvements, but the basic stuff for pushing an enmdmill has been figured out long ago.

ikdor
12-29-2012, 04:20 AM
I haven't seen the OP mention the number of flutes on his mill. If it's more than two, maybe he could try the two flute version.

Igor