[Kingjamez]

I've been pouring over Bob Warfield's wonderful site www.cnccookbook.com for the last week. He talks about dry machining aluminum, but it seems his definition of dry is "not flood". I'd like to machine aluminum actually dry and wonder how I should change my feeds and speeds in G-Wizard? From reading Bob's post it seems like I should alter my SFM, but by how much when completely dry is not spelled out.

I will be taking 0.05 WOC, .1875" DOC passes through 6061 with a 3 flute 3/8" endmill made for Aluminum at my roughing stage. G-Wizard suggests 49 IPM @2000RPM on my X3 mill. Any suggestions for a better IPM or DOC (WOC is fixed in my setup)? Can I really run that fast dry?

Attached is a picture of my project for this weekend:

[photomankc]

You gotta show that off after this weekend!! I'm wanting badly to do an AR-10 myself. Gonna be one of my CNC projects when I get it going.

[2ndSteel]

In my experience the 2 biggest problems with cutting aluminum without coolant are buildup on the cutting edge and clearing chips. You need to use some type of lubricant to prevent the buildup of aluminum on the cutting edge. I have used small amounts of WD40 succesfully. You also need to remove the chips from the cutting path as they will get pushed through the cut again and mar the surface finish. You could use a vacuum to remove the chips and then small amounts of wd40 sprayed on to keet the edge lubricated. Cooling really isn't that big of a problem on aluminum unless you want to cut at very high spindle speeds.

[webgeek]

What you describe above is EXACTLY how I do most of my aluminum cutting - a few squirts of WD-40 at the start to the process and vacuum up the chips every few minutes. You do get some roughness on the edges if you don't vacuum frequently enough but for quick stuff this has worked really well for me on the X2.

-Mike

[tony978]

To give you an idea of what you can get away with on 6061, I have a flashcut 6500 and found I could take full with of cut 0.035 " doc at 15,000 rpm @ 35 ipm with a 2fl 1/4" carbide end mill I picked up at homedepot .
If you want to machine dry 7075 works with no chips sticking to the part like 6061

[mwood3]

with a 2fl 1/4" carbide end mill I picked up at homedepot .

Wait...HD sells endmills?!?

wow i will have to check it out...

[webgeek]

A router bit rather than an endmill I suspect

[mwood3]

A router bit rather than an endmill I suspect

I kinda thought the same... i really wish i had a local vendor I could walk in and buy machine tools...but seems theres is not much in my neck of the woods...I really hate internet orders...

[tony978]

ya it is a 2 fl up sprial router bit . I didn't want to wait for an order from duramill other wise I would have used that . point is I used junk tooling at high rpm and no melted tool in work pice !

[SCzEngrgGroup]

For dry cutting, keep the same SFPM as for any other cutting. Calculate feedrate based on the manufacturers maximum recommended chipload (typically on the order of 0.004-0.005" for a 1/2" HSS endmill), and do a shallow cut. Go progressively deeper until either the spindle starts to bog down, vibration gets excessive, or the tool starts clogging. I can cut 0.125" deep, 1/2" slotting, at over 30 IPM with HSS. If you get clogging, INCREASE the feedrate. The tool gets hot when you feed too slow. When you feed fast, the chips will come off VERY hot, and the tool will stay cool, until you get into pretty deep cuts.

G-Wizard does an excellent job of calculating the best-case cuts you can do. I would start with its recommendation, but a shallower cut, then sneak up on the final depth you want, to make sure the machine can handle it. This will avoid tool breakage.

Regards,
Ray L.

[Kingjamez]

Thanks for the suggestions (especially Ray). I'll start off with running at the full speed that GWizard says I should run, but use 75% of the cut depth I calculated with. If that goes well, I'll push up the cut depth and see how things go. Thanks!

[mattbesquare]

I've been pouring over Bob Warfield's wonderful site www.cnccookbook.com for the last week. He talks about dry machining aluminum, but it seems his definition of dry is "not flood". I'd like to machine aluminum actually dry and wonder how I should change my feeds and speeds in G-Wizard? From reading Bob's post it seems like I should alter my SFM, but by how much when completely dry is not spelled out.

I will be taking 0.05 WOC, .1875" DOC passes through 6061 with a 3 flute 3/8" endmill made for Aluminum at my roughing stage. G-Wizard suggests 49 IPM @2000RPM on my X3 mill. Any suggestions for a better IPM or DOC (WOC is fixed in my setup)? Can I really run that fast dry?

Attached is a picture of my project for this weekend:

For my CNC machine, I found I had to drastically cut the cut depth when dry machining aluminum. I broke 8 1/4" HSS end mills finding the approximate ratio and debugging my own issues. make your cuts really light. And dont walk away if you aren't clearing chips. As the cuts got deeper they caused a lot of heat to condense on the cutter. As the bit heats up it can still dig and break. I ran a hose to my air compressor and it did wonders, but my "flood coolant" system is ready and can't wait to see how much more/smoother I can cut or how much longer I can make my end mills last.

[zerodegreec]

i really wish i had a local vendor I could walk in and buy machine tools..

In some ways yes and no. I live in a big center and well its gotten expensive because I CAN just walk in and buy most anything (or its next day pickup)... It can get a little draining on the wallet

In some ways the impulse to buy a special tool is easier than making what you have work...

[Unabiker]

I cut a lot of .080" 6061 aluminum on a cnc router dry. I use an Onsrud O-flute, single flute cutter spinning at 19,600 rpm. Feed rate varies between 130-170 ipm. For the .080" thick material, I will drop the bit .095" so that it goes completely through the material. For pocketing routines, I use the same spindle speed and feed rate with a 90% step over.

[tony978]

Can some tell me why people don't use coated carbide and use hss ?
On a hobby mill or full size cnc mill .

[mattbesquare]

Can some tell me why people don't use coated carbide and use hss ?
On a hobby mill or full size cnc mill .

Price..

And below a certain speed HSS can hold its own against carbide. I think above 4k rpm is when carbide begins to perform better than HSS.

I am considering trying some of the more exotic coatings. At first I thought they were snake oil because it always seems like it wears off at the edges right away. Then after doing more reading, some aren't supposed to do the cutting, but instead keeping the chips from heating and sticking within the flutes-a common problem in aluminun (with me) when I push the ipms harder than my mill speed can keep up and the bit starts to heat.

Now that I have my speeds mostly worked out, and my flood coolant going I am going to move over to high helix us made 3 flute carbide to see if they really are superior than I am used too.

I am a noob, so please correct me if I am wrong people.

[tony978]

I want to say I have more hss/ alum end mills then with carbide wile trying to run it dry and not trying to take 50% dia in depth with full with of cut .

what I was asking was more of why wast money on hss when you get more out of carbide solid or indexable ?

[mwood3]

for me it makes more sense to run HSS on aluminum...I think carbide is over kill for the home hobbist, and the occasional hard spot or (forbid it ...hitting your vise jaw, clamp etc.) would kill carbide...not that i know from experience

Edit: sure there are plenty of uses for carbide tooling in the home shop...im speaking purely about softer materials...

[photomankc]

[QUOTE=mwood3;814712]for me it makes more sense to run HSS on aluminum...I think carbide is over kill for the home hobbist, and the occasional hard spot or (forbid it ...hitting your vise jaw, clamp etc.) would kill carbide...not that i know from experience
QUOTE]

Yeah, it's nice to have the tool politely comply and mill a small slot right into the side of your vice.... not that I know from experiance


I think most of is are limited in spindle speed to really get much use from carbide I also prefer the fact that HSS is easy to work with and forgiving. Now over on the lathe I use a lot of carbide. Lack of a grinder and my general laziness about needing to make something to make something to make something leads me to try to get what I can from carbide.

[SCzEngrgGroup]

I want to say I have more hss/ alum end mills then with carbide wile trying to run it dry and not trying to take 50% dia in depth with full with of cut .

what I was asking was more of why wast money on hss when you get more out of carbide solid or indexable ?

"why wast money on hss when you get more out of carbide solid or indexable" - Because on these small, flexible, low-powered machines with their very low-speed spindles there is little, if any, benefit to carbide. Most benchtop machines do not have enough spindle speed to run carbide properly, especially small ones. Even a 1/2" carbide endmill wants to run 5000-8000 RPM in aluminum. HSS will generally take a heavier chipload, and they're FAR more forgiving. And, a HSS endmill, properly run, will last a LONG time. So, how do you "get more" out of carbide?

Regards,
Ray L.