View Full Version : light cuts in alum.

08-17-2005, 07:31 PM
Using WD40 doesn't help. When I am plaining aluminum heads is when I have the problem. For what every reason I can not always get a smooth cut when I am only lightly palaining (.005 or less) but no problem with deeper cuts. I am using HSS cutters sharpend to the 9's. Is there a better cutter, indexable or otherwise for this purpose? I have my cutter set up in a fly cutter configuration in my boring head on my mill.

08-17-2005, 07:42 PM
you may get a better result if you use paraffin as a coolant on aluminium, also check the cutting edge on the tool as a build up of alum seems to weld its self right on the cutting edge and this can sometimes cause a trashy finish. other than that im sure someone else on here will be able to give you more guidance.


C. Tate
08-17-2005, 08:30 PM
Increase the clearence angle. You may be dragging.

Cutting changes the material condition troughout the shear zone. Aluminum as well as other materials will have compressive resdiual stress built up from cutting. You may need to go deeper to get past that layer.

[This message has been edited by C. Tate (edited 08-17-2005).]

08-17-2005, 09:46 PM
If the .005 cut is the first cut you could be running into a lot of oxide and this is affecting your tool as it is hard and abrasive. The deeper cuts get under this layer and the chips carry the oxide layer away without affecting the cut. Look at your chip from the light cuts and compare them to the chips of the deeper cut.

Added, are these virgin cast heads that have never been machined before. If that is the case the surface will have all kinds of impurities in it and the .005 is way to light to get below this layer.


[This message has been edited by WJHartson (edited 08-17-2005).]

08-18-2005, 07:02 PM
This is the problem however. I do not have the option of going deeper. My max cut is .005. In fact that is a large amount and it is driving me nuts. They would prefer I cut even less. I am constructing custom racing engines for snowmobiles. If the work I am doing could be done while the castings were rough and I could cut whatever to my finished depth there would be no problem. They come into the shop finished and I have to complete the custom work. Is there a cutter with a finsh that would be more friendly on alum.. This "paraffin" is it the same as what you use to seal jamb jars? If so how is it applied or do you desolve it in a suitable liquid?

08-18-2005, 07:09 PM
Are you running a "wipe" on the cutter? or how about a rounded cutter.

Michael Moore
08-18-2005, 08:34 PM
.005" maximum sounds like you could put them on a surface plate covered with W&D sand paper and just sand them down. Change direction while you do it and finish with some finer paper and they might be plenty flat enough.


08-18-2005, 08:58 PM
'using a fly cutter'- I'm wondering if it's possible for you to set an angle on the cutting edge such that it shears rather than chisels the material away. If you touch the cutting edge down to the workpiece, then look from that point of contact towards the axis of the flycutter, does the leading edge of the cutter parallel that view? What I'm suggesting is that looking along the leading edge of the cutter your view should take a line behind the rotational axis of the flycutter (spindle axis). I hope this is understood, and I don't know if there's a way you can adjust for this short of grinding this shearing angle into the cutting bit. Note this is not relief angles I'm talking about. I'll post a pic of what I'm suggesting if it comes to that.

C. Tate
08-18-2005, 10:04 PM
If you have a good mill i.e. bridge or similar not a three-in-one or table top then:

Ditch the single flute HSS boring head rig. Buy a multiple flute indexable face mill. There are some very good aluminum only tools out there. Iscar makes the best I have seen. It is not cheap nor are the inserts but it will do the .005 pass and the finish will be supurb. If you do not want to make that investment then buy a true fly cutter and use brazed carbide tools. The home brew fly cutter and hand ground tools are going to be a battle. Boring heads are for boring and hand grinding good tools is an art.


C. Tate
08-18-2005, 10:06 PM
Ditch the homebrew fly cutter for true facemill. Iscar makes supurb mill for alum. If the investment is to great buy a true fly cutter and use brazed tools. Boring heads are for boring and hand grinding tools is an art.


08-18-2005, 11:23 PM
I suggest if your machine will not take a smooth .005" cut, but will take a deeper one that you've got some slop in something. Maybe spindle bearing, or whatever.

What happens sometimes is the heavier cut will force all the slop out of the setup, while the light .005" skim cut isn't enough to take the looseness out and gives a less than smooth cut.

So, assuming your cutter has relatively correct geometry, it sounds like you need a more rigid machine or tooling setup. I don't think buying an expensive insert cutterhead is going to solve your problem (it will lighten your wallet substantially though).

BTW, on my biggest CNC we face aluminum quite bit to high tolerances. Passes of less than .001" depth can be done good results (although it's hard to measure down that fine on some of our workpieces). My point is it possible to take very fine skimming cuts, even with hand ground single-bit, flycutters provided the machine is absolutely rigid.

08-18-2005, 11:33 PM
What speeds/feeds are you using? Sometimes fast is the problem on cast aluminum,especially alloys containing high amounts of scilicon like cylinder heads.

You might try,no more than 100 rpm and .0025"/rev feed.A carbide tipped tool will outlast HSS if the head made from one of the alloys mentioned.

08-18-2005, 11:46 PM
I use turpentine paint thinners on aluminum alloys,works a treat.


08-18-2005, 11:47 PM
BTW.DO NOT use laquer thinners on alloy,it will melt away before your eyes!


08-19-2005, 10:05 AM
I second the suggestion of a multi-insert face mill. The flex in that fly cutter setup is killing you. If you go this route, you will need to kick the speed and feed WAY up. Use compressed air to keep the chips off and forget about the coolant. Recutting will ruin your cut quality on something this light.

There are usually a lot of face mills on Ebay, but since this is for production I would buy from a dealer. I have been eyeing the Iscar CHAMMIL cutters that will use four different insert types in the same pocket. That would seem to be a very flexable tool that might give you a bit better ROI.

Maybe if you give a little more detail on the machine you are using the guys here could be a bit more helpful. How wide is the surface you are trying to face?

Here are a couple of face mills on the Bay





[This message has been edited by jkilroy (edited 08-19-2005).]

08-19-2005, 07:16 PM
My mill is a Cincinnati and very ridged. It is possible the Hss cutter is not shapened properly for the job. I have an indexible face mill 5.25" but the reason I was using the boring head with a fly cutter set up was to cover the 6" head in one pass. C Tate: is there a particular indexable cutter you have in mind? Right now my unit has cutters and wippers set for mild steel and I do get a good finish even on light cuts. I would love to do that on aluminum. Darryl: is it possible you could post a picture of that cutter sharpening detail you are talking about? I'm not quite ready to give up on the hss just yet. When it comes to aluminum and plactic HSS is still my preferance.

08-19-2005, 07:23 PM
Pure ethanol is the best lube I have found for aluminum. It's a bit hard to get though.

08-19-2005, 07:26 PM
You need a cutter thats made for alum. hertel has some good ones.

3 Phase Lightbulb
08-19-2005, 07:46 PM
I get a mirror like finish with alum when I use flood coolant. It may have just been my setup, but for light cuts, the tiny chips would hang around and the cutter would grab and drag them making swirl marks in the finish. When I tried flood coolant, all of the tiny chips immediatly got washed away and I had a mirror like finish. I also tried blasting air from my compressor while cutting and that works just as good.


08-19-2005, 09:51 PM

Here's a pic hopefully (haven't done this for awhile) showing some details of the angles ground on the flycutter bit. This is the type of flycutter I have with the stick of hss sticking out the side of it at a downwards angle. Pic A is looking at one side with the cutting edge out to the right, pic B is a side view looking end on at the cutter, pic C and D shows what I was talking about, the red circled area shows an additional angle ground into the bit in addition to the clearance angles depicted in other views. Pic A shows a small flat ground on the bottom of the cutter and the end of the bit has a vertical relief angle. This one is good if you're boring with the flycutter. Where the bottom edge makes a sharp corner with the end of the toolbit, a small radius should be stoned on.
I hope that all makes sense.
By the way, the flat bottom I've shown in pic A is exaggerated, it shouldn't be that long. There's probably a rule somewhere about that, depending on rpm, feed rate, etc.

[This message has been edited by darryl (edited 08-19-2005).]

C. Tate
08-19-2005, 09:53 PM
This is the one. Only lists 5.0 dia as largest. If you have a Cincy get some PCD inserts for your facr mill and run it fast the .005 finish will be not problem and the finish will be supurb. Expect to pay $90 to $100 per insert. I still think the boring head and tool angles are your problem.


08-20-2005, 06:55 PM
Darryl:Looks good and explains the explanation. I'm goint to give it a try on some scrap I have before I hit the next job. Evan: are you sure about the ethanol. Sort of dangerous from a stray spark standpoint.I know that is an extremly remote possiblily with aluminum unless you hit your steel mounting hardware. Ethanol is no problem up here if it works. 3 Phase: That air is somthing I havent tried but a good idea. Thanks all.