[Mahonroy]

Hey guys,
I am creating aluminum face plates for a device I am building, and I am doing this with a CNC routing machine (using 1/8" shaft sized bits). Here are some photos of what the face plates look like:






It has been a challenging task to get the machine set up to cut out the various shapes/pockets, and its still not working correctly and is definitely not a reliable process. My problem is that I keep breaking bits, so initially I started slowing everything down, and the bits would stop breaking, but it would then start generating a lot more heat and the cuts didn't look very clean. This also added a lot of machining time to it, and still periodically bits break.

Here is some info on my machine.
I am using a Chinese 3040 CNC routing machine that I have upgraded. I swapped the stepper motors and controller over to the Gecko g540, and upgraded the spindle to a 450 watt, 10,000 RPM spindle. The machine seems to be solid and well built. I also have an RPM reader on the spindle. I am also using "Cut 2D" software to generate GCODE.

The cuts that are giving me the most trouble are the 0.125 end mills, and the 0.0394 end mills. For the 0.125, my pass depth is 0.01", and feed rate was 8" per minute. Everything is 10,000 RPM. I was using a single flute HSS end mill. This worked alright, but was slow, generated a ton of heat, and the cut was not clean at all (lots of melted metal looking burrs everywhere), but the bit rarely would break. I then tried switching over to a double-flute bit, and it seemed to work better. I then tried using some speed/feed calculators and found that I should try a faster feed rate; so I tried 14" per minute and it appeared to be cutting great.

The problem is that after a while, little aluminum bits start to build up in the cutter, and everything starts to get hot, and then the bit breaks. I am averaging 2 face-plates before this starts to happen then the bit breaks. I also wanted to note that the RPM's stay right around 10,000 RPM, it doesn't really slow down once its cutting.

Here are a couple pics showing the jig setup... and notice how the cuts start out fine, but then quickly goes down hill by the 3rd and 4th plate. Also note, that total cut depth is 0.06" deep, so this is 5 passes:



I recently ordered a couple of 4 flute bits to experiment with... but honestly I just don't know... seems like I just don't know whats going on and figured I would ask you guys. I am also tempted to try and reduce the pass depth even more (from 0.01" to like 0.005")... but that's already a really small bite out of the metal and it seems like it should be able to handle this better?

Anyways, any help is greatly appreciated, thanks!

[Ed VanEss]

and your doing this with no coolant?...I usually spray wd40 on the part. prevents heating and loading up the tool. just be carefull of fire..

[svenakela]

This is a classic. The cutter will clog up if you are running your machine this way. Lower the RPM, raise the speed a lot (way more than you think) and use a coolant. One of the best coolants there is for aluminium is ethanol and no, it will not set your machine on fire. Second best is compressed air with water mist, but compressed air works too. I can assure you that with ethanol you will get mirror surfaces.
A specific aluminiun two flute cutter is the way to go and get a carbide cutter (no cheap HSS). If the plates are vibrating there are also reversed cutters where the flute is spiraled the opposite way. These kind of cutters are extremely well performing with thin sheets as they push the material downwards during operation.

Don't worry, you'll get great result if try some coolant and more feed rate.

As an example, the voids in the left part of the mold is made with ethanol only. There's not a single mark or scratch.

[svenakela]

Nice little device, by the way.

[victorofga]

make some tests...
make shallower passes.. 12000 rpm is ok, just make shallower passes and use the wd40..
it might takes longer but you get trough, and less faulty pieces..

alcohol (denatured spirit) or ethanol also works very well.
they have a great cooling effect also they preventing build up..

with a rigid milling machine you could cut trough in one pass with a proper bit..
but you have a router.. so everything is different

[Mahonroy]

Thanks a lot for the replies!

Yes you are correct, I was not currently using any coolant.

So I heard that if using a single flute mill bit, that I want closer to 20,000 RPM, and a dual flute mill bit closer to 10,000 RPM (for a 0.125" diameter end mill).... do you still think I should go slower on the RPMs? That is interesting with the reverse 2 flute cutter, I will try and source one to try it out.

I will definitely try out the ethanol idea. I was originally worried that using a coolant would make a mess, would mess up my jig, and would stain the anodized aluminum, but it sounds like ethanol might be a clean solution.

[victorofga]

mdf good for jig.. when you use for wood..
I would suggest a pvc sheet or even aluminum if you have a lot of this..

pvc cost about 20-25 for this task

PVC Type I | Plastics International

mdf can swell by coolant..

[Superman]

1+ for the coolant ( WD40, even kero ), anything to stop the re-melt of the chip

So I heard that if using a single flute mill bit, that I want closer to 20,000 RPM, and a dual flute mill bit closer to 10,000 RPM (for a 0.125" diameter end mill).... do you still think I should go slower on the RPMs?

Just to put you onto the correct track

The cutter diameter is NOT altered, so the RPM does not change
it is the feedrate that gets increased

ie. a 1/4" cutter is set to S10000
( the calculation for feed per minute is FEED(per tooth) X RPM X Number of teeth
--- single flute set to 0.0025" feed per tooth or ( .025 X RPM X 1) = 25" per minute
--- 2 flute would be 50" per minute
--- and so on

Personally, I don't like 2 flute cutters, too thin in the web, & they flex too much....but you do need a decent cavity in front of the cutting edge for the chip.... the 4 flute gap is a little small, so would clog up much quicker that a 2 or 3 flute
- use 3 flute CBD centre-cut uncoated, that is ground for alum

Your part looks anodised ?
- this will destroy HSS cutters real quick, this "skin" is 60-70 Rockwell

[svenakela]

1+ for the coolant ( WD40, even kero ), anything to stop the re-melt of the chip


Just to put you onto the correct track

The cutter diameter is NOT altered, so the RPM does not change
it is the feedrate that gets increased

ie. a 1/4" cutter is set to S10000
( the calculation for feed per minute is FEED(per tooth) X RPM X Number of teeth
--- single flute set to 0.0025" feed per tooth or ( .025 X RPM X 1) = 25" per minute
--- 2 flute would be 50" per minute
--- and so on

Personally, I don't like 2 flute cutters, too thin in the web, & they flex too much....but you do need a decent cavity in front of the cutting edge for the chip.... the 4 flute gap is a little small, so would clog up much quicker that a 2 or 3 flute
- use 3 flute CBD centre-cut uncoated, that is ground for alum

Your part looks anodised ?
- this will destroy HSS cutters real quick, this "skin" is 60-70 Rockwell

I can't say I like that formula. I run Alu with two fluters at 250 IPM @ 10 000 RPM.

[Superman]

I can't say I like that formula. I run Alu with two fluters at 250 IPM @ 10 000 RPM.

If you read it correctly, it was stated as an example of feedrates, not the cutting speed, that alters...nothing more

250 IPM (6350mm/min) or 0.0125"(0.315mm) feed/tooth....not bad.....what's it like at cornering ? cutter life ? DOC ? cutter Ø ?

[CosmosK]

Your part looks anodised ?
- this will destroy HSS cutters real quick, this "skin" is 60-70 Rockwell

That'd be my guess why the cutter only makes it through 3 parts.

[CosmosK]

I usually go by the end mill specs too. Here's an example: maritool.com/images/speeds-and-feeds-1004.pdf
This shows .0015 chipload for 1/4 end mill in Al. If you do the calculations, the SFM number might show you 10k rpm is too fast.

I calculate with .002 chipload, 6500 RPM is the max before bypassing the 430 SFM. Feed comes out to be 25 IPM.

[Mahonroy]

My bits are 1/8" not 1/4"
So I found that the chip load is 0.001" for 1/8", so (0.001 X 10000 X 2) = 20" per minute. How do you know if the RPM is right or not though?

I found this:
http://www.endmill.com/pages/trainin...d%20Drills.pdf

It says SFM is 600-1200 for aluminum.

[CosmosK]

There are several calculators out there: Here's one, look at equation #2 Milling Formula Calculator

1/8" will be a better fit to run on the router. I see 13K RPM

What RPMs do have have as options?

[Mahonroy]

There are several calculators out there: Here's one, look at equation #2 Milling Formula Calculator

1/8" will be a better fit to run on the router. I see 13K RPM

What RPMs do have have as options?

Currently I can only do 10,000 RPM's, so I would need to change some stuff to get anything different.

[CosmosK]

If 10k RPM is fixed, 20 IPM will give you .001" chip, 40 IPM .002" chip.

I'd find a carbide bit for getting through the anodize.

I would not go 250 IPM. Maybe it can be done, but seems way too much stress for a little 1/8 end mill. Good luck

[victorofga]

aluminum cutting speed is 2800 ipm for carbide tools.. that does mean 7121 rpm..

however carbide takes lot more heat than hss so even higher rpm can be accepted.. his machine doesn't works what machinist using generally..

he breaking bits due to flexes when machine lets ""extra"" movement, when the machine can resonating..

a rail versus a cast iron slider not rigid at all.. that is his main problem.. very possible the feed-rpm combination on a milling machine would go.. but on a router can not..

for him indeed higher rpm shallower passes, and high federate.. federate need to be lowered when you can make deeper passes.. so, the 250 ipm and the 10 ipm both can be true with properly associated depths..


well I calculated from values for turning.. but I guess milling is close


the anodizing for me looks weird, because use to be, anodizing is the last process.. so why is it not anodized after all cuts?
he has to find experimentally what his machine rigidity can take..

[CosmosK]

2800 IPM? Do you mean SFM? I think I've sen that number for carbide.

I'd defer the the manufacturer's numbers to be on the safe side, at least to start.

A router is not a mill, true. So, you probably won't be running at the max settings. Lower chip means lower cutting force, so less deflection of your rig.

Probably will take trying a few things.. good luck.

[victorofga]

yes I made mistake here ...

that is not ipm but sfm.. and by that the numbers saying 80 K rpm..

and I post here a video I watched many times.... tool steel machined with incredibly fast feed..
due to high rpm.. the machine has spindle with 60K rpm..

https://www.youtube.com/watch?v=0cugaYJzeIg


so very small tools can be moved fast

so if original poster can afford, then probably another spindle could solve his all problem... even using a 3/32 or 2.5 mm endmill
because of the high rpm makes possible less force with higher feed..

Water Cooled 300 watt 60000 rpm Spindle Motor with Collet ER08 for CNC Drilling of PCB Board, Fast Shipping-in Other Machinery from Industry & Business on Aliexpress.com | Alibaba Group

I make frequently mounting hardware of anodized aluminum angle, and I didn't find that anodizing would be tough on carbide mill.. but it was only my experience..

[CNCMAN172]

Mahonroy,
You can cut that think aluminum without coolant if you use a two flute 1/8" solid carbide bit. I normally run 10,000 RPM, DOC is .020, and the feed is normally about 15. The feed really depends on the rigidity of your machine. It is also nice to add small amount of air to clear the chips even a small aquarium air put can do the job. You just do not want to cut the chips again.Attachment 282374
Here is an example of a custom RC helicopter frame I made using that thin aluminum. Someone else pointed out you have anodized aluminum, you might want to cut the aluminum prior to the anodizing process as well as that makes it harder.

Russ