Machsupport Forum

Mach Discussion => General Mach Discussion => Topic started by: kolias on January 09, 2016, 02:53:23 PM

Title: 1/4" 2 Flute End Mill
Post by: kolias on January 09, 2016, 02:53:23 PM
I used a 1/4" 2 flute end mill to make a 6” long slot on a 3/8” thick piece of aluminum. The end results were good but I had a hard time with the router which was not going smooth thru each pass. I used multi passes each about 1/32” and the router at about 15K RPM

Perhaps a 2 flute end mill is not the right choice? I also have similar end mills with 1 flute and 4 flute

Any suggestions?
Title: Re: 1/4" 2 Flute End Mill
Post by: BR549 on January 09, 2016, 02:58:49 PM
Unless you are cutting at about 150 IPM your RPM is way to fast for that cutter. What feedrate are you cutting at ??

Title: Re: 1/4" 2 Flute End Mill
Post by: ger21 on January 09, 2016, 03:13:54 PM
Is it a 2 flute router bit? What exact bit are you using? 2 flute endmills come in hundreds of varieties. Some will work for what you're doing, some won't.

For a router, your best choice is a single flute "O" flute bit, at about 10,000 rpm and 60-80ipm. Unless your machine is really rigid, you may need to take shallower cuts than 1/32".
Title: Re: 1/4" 2 Flute End Mill
Post by: kolias on January 09, 2016, 05:55:22 PM
Sorry Gerry, no clue what it is. By the way I used my router to do the slot and the bit is carbide which I bought a few years back. Never new that endmills come in so many varieties
2 years ago I did the same job with the same router and I remember the router was going so smooth. Perhaps I did use the single flute endmil and I will do the same now since I have another similar slot to cut
Thank you
Title: Re: 1/4" 2 Flute End Mill
Post by: kolias on January 09, 2016, 07:30:17 PM
I found the box of my 1/4" 2 flute end mill and it is: 1/4" SE 2FL, SQ. Searching on the web I found no reference what these letters mean
Title: Re: 1/4" 2 Flute End Mill
Post by: Jarhead on January 09, 2016, 07:37:08 PM
1/4" Single End, 2 Flute, Square
Title: Re: 1/4" 2 Flute End Mill
Post by: joeaverage on January 10, 2016, 03:44:05 AM
Hi kolias,
unless the cutter is 'brand new' sharp then you risk getting a built up edge where aluminium sticks to the tool. There are cutters designed
for aluminium but any sharp, I mean REALLY SHARP cutter works pretty well. Coolant helps both with the aluminium sticking to the tool
and flushing away the chips, a real must and hard to achieve when slotting.
My experience is that if a tool goes off song stop and replace it otherwise it will load up and break often wrecking the part as well.
Spinning a tool fast is very appealing but unless you feed fast you cut tiny little slivers which get stuck in the works. With good flush  coolant
and good chip removal ie not deep pocketing or slotting I run at 15000 but any other, in fact most normal ops, I run around 10000 with 1/4 inch
tools.

Craig

Title: Re: 1/4" 2 Flute End Mill
Post by: rcaffin on January 10, 2016, 04:18:22 AM
Coolant may not get the chips out fast enough. Try a good air blast with a little oil mist to keep the cutter wet.
Yeah - SHARP cutters not previously used on steel.

Cheers
Roger
Title: Re: 1/4" 2 Flute End Mill
Post by: ger21 on January 10, 2016, 07:31:06 AM

Yeah - SHARP cutters not previously used on steel.

Or wood, especially mdf or plywood.

When cutting aluminum or plastics, never use bits that you've used on wood products before, as it will already have a dull edge, even if it seems sharp.
Title: Re: 1/4" 2 Flute End Mill
Post by: kolias on January 10, 2016, 11:24:45 AM
Thank you all for the help

Today I had to cut my second 1/4” slot.

Yesterday I used the endmill shown in the attached picture at the right (spiral) and did not go well but managed to finish the job and got a good slot.

I thought I had 1 flute 1/4" end mill but the one I have is only 1/8” so I used an old 2 flute 1/4" endmill shown in the attached picture at the left. This one is not spiral, it has just 2 cutters straight up from the bottom and did a beautiful and smooth cut.

I plan to buy now 1/4" endmills similar to the one at the left and I will buy single flute and double.

What type of endmills are the ones shown in the picture and what is their use?
Title: Re: 1/4" 2 Flute End Mill
Post by: ger21 on January 10, 2016, 11:45:19 AM
The one on the left is just a carbide tipped router bit.
Title: Re: 1/4" 2 Flute End Mill
Post by: kolias on January 10, 2016, 01:08:08 PM
Is this the right bit to use for aluminum if I get one with single flute?
Title: Re: 1/4" 2 Flute End Mill
Post by: ger21 on January 10, 2016, 02:19:15 PM
No, not really, but it will work.
A spiral "O" flute is the better option.

However, if your machine lacks rigidity, then you may get better results with the carbide tipped bits.
Title: Re: 1/4" 2 Flute End Mill
Post by: kolias on January 10, 2016, 02:33:07 PM
Thanks Gerry, as I said I'm using a hands router and I wonder why the carbide tipped bit did a much better job than the spiral

The spiral I used was a brand new bit and the carbide tipped came with the router among other bits which were of no good quality

So I will buy a new good quality carbide tip single flute + 2 flute
Title: Re: 1/4" 2 Flute End Mill
Post by: rcaffin on January 10, 2016, 03:30:59 PM
Hi Kolias
The one on the right is an absolutley stock standard end mill for metal.
The one on the left is not used very often on metal: too much impact, but you could perhaps use it on sheet metal and I am sure it gets used on wood.

Hi Gerry: 'not on wood' - yeah, i had noticed that some timbers were not nice. You should see what old dead Oz wattle does to anything: some of them are full of silica and are rough on carbide (and they just eat HSS).

Cheers
Roger
Title: Re: 1/4" 2 Flute End Mill
Post by: Raychar on January 12, 2016, 12:17:51 PM
Hi,

I have Kress spindle which is supposed to be able to run at 12000rpm?, but in order to have longer service life for it. For example, for cutting with 6mm diameters cutter, i turn the dial to 2 or 3 out of 10. I don't exactly know how much rpm it is, may be around 2000. I use 4-flutes standard H.S.S milling cutter to do a lot of milling in aluminum. I know 2 flutes or single is better, but in term of cost, in my country, 4 flutes is a common one and is cheaper than the others. Of course, sufficient flood coolant is needed.

Even though, for 3mm cutter, I do it in this manner...rpm is around at dial #4 to 5 and flood is critical...
Title: Re: 1/4" 2 Flute End Mill
Post by: rcaffin on January 12, 2016, 03:24:33 PM
> flood is critical ...
Funny about that. I don't use any flood at all. I don't even have flood. Too messy, too expensive, not needed.
But I do use air blast and MQL. That works very well.

Cheers
Title: Re: 1/4" 2 Flute End Mill
Post by: Raychar on January 12, 2016, 08:45:44 PM
It depends....Most important thing is that, I work the machine in an office where it hasn't installed compressor,also, my spindle is too noisy when it is at high revolution. This method works for me under these parameters and, frankly , i know many people adopt other methods.....During the learning period of my cutting work, i did mostly on aluminium, many milling cutters were broken because of lack of proper coolant. Today, i can use one piece for a longer period of time. This is a tutorial fee i paid for...

White color milky type coolant works well in carrying chips and heat away the cutter especially in doing micro type millings.
Right, much installation is needed at the early stage, building srroundings to collect coolant, filtering, re-circulation for re-using the collected coolant. In long terms, it is cheaper....
Title: Re: 1/4" 2 Flute End Mill
Post by: rcaffin on January 12, 2016, 10:19:37 PM
Hi Ray
Quote
many milling cutters were broken because of lack of proper coolant.
Not entirely. Many milling cutters are broken on aluminium due to Built-Up-Edge. To be sure, BUE can be reduced by coolant, but it is actually mainly caused (imho) by the Al alloy you are cutting. If it is a 1000- series or a 5000- series alloy - chewing gum! That stuff sticks to the cutters like mad.

Air blast prevents recutting existing chips: a better finish. Pulsed MQL keeps the cutter wet so the metal does not stick. Selection of a machinable alloy though makes all things magic.

Cheers
Title: Re: 1/4" 2 Flute End Mill
Post by: BR549 on January 13, 2016, 12:29:08 PM
The only way the buildup occurs is because of heat and the  melting point of that particular aluminum.  Too fast RPM for the feedspeed causes a great deal of rubbing(heat)  .  Dull tools or wrong tool form creates heat. 

Just a thought, (;-)TP 
Title: Re: 1/4" 2 Flute End Mill
Post by: rcaffin on January 13, 2016, 03:34:55 PM
Hi Terry
Well, yes , and no (imho).
Rubbing is seriously bad of course, but having intercepted a few cases just before the cutter broke (really), I don't think it is that simple.

What I have seen ias a build-up of aluminium at the tip of the cutter - little chips sticking to the carbide. It is known that some carbides have a slightly rough, almost porous surface, and the aluminium can get wedged into the pores. That's at the microscopic level. Then the built-up aluminium starts to rub on the stock, and that does create a LOT of heat and a run-away situation.

Yeah, I kid you not: there was this slightly melted blob of aluminium wrapped around the tip of the carbide cutter! Getting it off was hard: it was really stuck on in a conformal manner. I switched to a polished HSS-Co cutter for the rest of that job - with some pulsed kero/oil mist to keep the cutter wet.

I agree that the sharper edge on a cutter meant for Aluminium works better - a polished flute also seems to help. Some of those 'aluminium' cutters break down quickly when used on steel. The edge is too thin.

It all gets expensive. Now I have cutters labelled 'steel', 'titanium', 'aluminium' and 'plastic', and have to keep them separate. But it seems to work.

Cheers
Roger
Title: Re: 1/4" 2 Flute End Mill
Post by: BR549 on January 13, 2016, 04:15:05 PM
YEs cutter FORM can be specific to teh material. Here I use a cutter specifically for aluminum. Very sharp and very polished, most of the time they are colbalt or HSS. Carbide as a last resort.  BUT the root cause is always heat. I have seen some instances where even flood coolant could not cool teh actual cutting surface. It created a steam pocket and the actual tip was not cooled. Most GOOD coolants have a surfactant to break down the surface tension of the liquid to help in those areas.

Yes brass tools, aluminum tools, Titanium tools steel, tools Low carbon steel , and tools Hi carbon steels.  I think I have more money in tools than Machine (;-)TP