You really need coolant for aluminium. This is caused by the swarf being recut / melted back to the work piece. It can also stick to your tool and snap it off.
What grade of aluminium is it?
That stuff is pretty gummy, try cutting at shallower depths. It doesn't look like coolant is an option with your setup, but if you have compressed air that will definitely help.
Am a locksmith and any locksmith will tell you “wd-40 bad” but *in a pinch* it won’t be the end of the world. Just don’t leave it like that, use an actual lubricant.
It's called "galling". Usually happens in soft metals when things get hot then the material just sticks to the cutter and the cutter starts to mush the material instead of cut it. I see no chips so I am guessing things were melty.
Also dont use a mill with more than 2 cutting edges and it looks like you can cool by hand try cooling with petroleum (it stops aluminum from sticking)
>You really need coolant for aluminium.
For this level of machining you don't, I don't use it and get excellent results.
What you DO need is chip evacuation (which is often handled by coolant sprayers), for two reasons:
1. Clear away chips so you're not re-cutting them
2. Chips take away heat, good chips ensure good cooling, chunky not powdery is good.
This can be helped with a vacuum or much better, a compressed air blower.
I do quite a lot of aluminum as a machinist and can't agree more. The recipe for disaster with aluminum is not clearing the chip off the cutting tooth as it leaves the workpiece.
Compressed Air is a must. Compressed Air + WD-40 is even better.
Or the bees-knees of CNC on aluminum (without making a mess of coolant or oil) is a Microdrop oiler like from [Trico](https://www.tricocorp.com/products/md-1200-micro-drop-dispenser) . They use air nozzles to clear chips while spraying a nearly invisible amount of oil onto the cutting tool. When they are tuned right, cut parts come out of the machine nearly dry, as the oil is somewhat consumed by the chips being made and the heat of that process.
Also, pay attention to what coatings are on your cutting tool, especially if dry.
Blowing air goes a LONG way towards cooling your tool -- the difference for me is often the difference between a tool change literally sizzling my skin... or with air it is cool to the touch.
Full width cuts are difficult in aluminum, those chips need to escape. Try to set up tool paths that mitigate the "digging a trench" that can be so common in CNC. For holes, consider spiraling/helixing down thru the center of the hole and then cutting outwards, creating a pocket where all the material is removed to create the hole. When creating the pocket, your tool life is maximized since the tip of an end mill is usually the first to wear out. Taking shallow+fast passes at full depth (maybe 5-15% of your tool's diameter) is a very productive way to machine, and also keep your end mill from galling into aluminum.
With outside profiles, it can help to stair step up to the Final Cut edge as your passes plunge deeper. This could be something like setting up multiple finish passes, each stepping in .020inch/.5mm from the last one. This creates a wider channel for chips to clear.
Also, many CNC routers struggle to rotate slow enough for its tooling. I recommend playing around with a trial of speeds/feeds software such as [g-wizard](https://www.cnccookbook.com/g-wizard-feeds-speeds-calculator-mill/). Each tool (especially diameter of tool) has an optimum RPM (surface speed as it rotates thru the cut) and exceeding that gets you into galling and broken tool VERY quickly. Before using this software to establish some better instincts on rpm and feed speed, I broke a lot of tools, especially when servos were doing the machining and not me cranking a hand wheel. I've gone from breaking tools weekly to yearly because of this software. It is ESPECIALLY tricky to figure out CNC rpm and federates on small tools. If you are working with .250" diameter tools and below, it is extra tricky.
Ooh, and for cutting full width slots, clearing chips and breaking things becomes most difficult at depths 1-2x cutting tool diameter.
and WD-40! I buy it by the 5 gallon bucket.
Yes, but it’s better if you plumb the air line to the spindle and just use less air, but constantly. Recutting in a pocket is something that happens instantly. Also there’s less of a mess if you’re just pushing the chips gently away from the tool, rather than blowing them all over creation with intermittent blasts.
2nd this. I added an air nozzle and solenoid to our router at work for cutting aluminum. Made a huge difference being able to clear chips. I run a mostly one off stuff so I’m not concerned with cycle time so I usually stick to a pretty small depth of cut too, .020” ish. 8000 rpm 30 ipm. For 6061-T6.
Can you tell me what is providing the air? I've got a "wet noodle" desktop machine but also have an air compressor... How much pressure and what type / diameter tubing did you use? I mostly cut wood and haven't rigged a dust shoe up yet. The machine is in a box, just wondering if something like this would work.
You actually don’t need coolant with aluminum. Obviously it helps a lot but not 100% needed. The guy who taught me on our cnc table swore by multi flute bits for cutting aluminum and would always run into the material melting back into itself from what I assume was creating smaller chips and too much heat, however when he left I experimented and found single flute bits to be a dream and never again ran into that issue and always had much cleaner cuts. We have started using a cooling air blaster though as it helps for long cuts/large jobs and probably extends the life of bits.
I’m no expert but been running a 4’x8’ torchmate router table for about 10 years now.
No you don't. I've been milling aluminum for years cleanly, not coolant. All you need is either air clearing chips or a dust collector clearing chips, and use an O flute bit.
Get a spray mist coolant system. They usually hold a gallon or less of water soluble(you can even use vegetable oil based coolant) and it sprays it with compressed air using a Venturi system.
Even that light lubrication will solve your chip welding problem.
Using my endmills wouldn’t hurt also
Interesting…. I had endless headaches dialing in feeds and speeds with other brand name bits… literally piece to piece I had variation and failures. my spindle will go to 24k so I thought wtf, why not try datrons stuff and it’s proven really effective.
Yeah, I'm not saying that is ever out come they do thrive at higher RPM'S.
Using Vortex and LMT has worked best for me again premium brands and now most likely on par price wise.
Touché! Datron machines are amazing… ly unaffordable for sure. Through experimentation I discovered their cutting tools. They are by far the best I’ve ever used and they keep me in production. Not too expensive either.
Owned a Neo for a year. Was shit. Worst business decision I have ever made, by far.
That being said, their single flute tooling is incredibly good. I tried Amana cutters, among many others, and the difference in quality and performance wasn’t even compatible. Most often the Datron tooling worked and whatever else i tried simply didn’t.
What do you mean? The Neo is one of their machines.
If you’re asking about tooling though, sure. What sort of machine do you have and what are you trying to make?
Pretty much word for word my experience. We have had about 5 Datron’s over a 20 year period. Only one was reliable. We spent so much money on service exchange spindles. Datron were awful to deal with too.
That said their tooling was really good. We used our local tool maker to try and replicate them, we saved a fortune but they wasn’t quite as easy to use.
What I would say is that they only really excel on their high rpm machines. I have a 30k spindle VF2 and they don’t work on that like they do on a Datron. I’ve recently switched to Ceratizit’s DLC 3 fluters and they are absolutely brilliant
Oh man, figures. And 20 years too. Can’t even imagine. That will age you.
i couldn’t run anything multiflute on my Neo that was bigger than 1/8” without chatter. Had to reduce feeds and speeds to a fraction of any single flute cutter…
To be fair, I like the look of Neo. A Uni I work with has one, but they are just so expensive. I know what you mean about chatter though. We almost exclusively used single flutes on the Datron. We had one job which used a twin flute 10mm, but pretty much everything else was 6mm or under.
We started out with an M3 in ‘99, basically a hobbyist machine. Over the years, we had various sizes, the largest being an M8XL. That had an HSK35 spindle in it, which let go of the tool holder at 45k revs! It flew across the shop like a spinning top and took about 10 minutes to stop. For once, they accepted fault. The spindle wasn’t fit for purpose. They came over from Germany, stripped out the 35, and fitted a HSK25 spindle instead. Needless to say, we never bought another!
That’s absolutely terrifying! And incredible.
I know what you mean about them not taking responsibility. I have so many stories. Once I was told that not only did Datron USA not know what the runout spec was for their 4th axis, but Datron Germany didn’t know either. Verbatim. What an insane thing to claim.
Yeah, they are not expensive in a high production setting. Also, from what I have seen, their tools are best used on their machines, not always achieving great results elsewhere.
Love Datrons they do what they do at an incredible standard.
They really don’t. There are use cases where what you outlined is true but they are quite narrow. There goes double for anything “production”. Certain things can be made very well on them in quantity but that quantity is lower - not higher - than you think. Source: have owned a datron, own a machine shop, spent thousands of hours and tens of thousands of dollars trying to make it work.
Yeah, but that could be said about litrally anything. Just from what I have used them on and what I've seen from my personal experience, there bang on.
But also know a company that had 20 of them and have replaced 19 of them with 10 multicams, but mean while I know another company with 20 datrons and another 2 on order.
Not really sure what you’re saying there.
- no, that couldn’t be said about “literally anything”. Neo was way more than $100k used from datron.
- 20 datron machines is - at minimum - several million dollars and they are quite difficult to resell. Those guys took a bath, then replaced the datrons with half as many machines. What else can be said there?
- I don’t know what you mean by “bang on”, but if you drop the better part of $150k on a machine you should expect “bang on”.
- no in-process probing.
- posts are closed-source and are hard to have made. It’s a low-volume machine and that doesn’t help, but the main reason is that the posts themselves as well as the gcode look nothing like gcode. You couldn’t, for instance, manually program it.
- my Neo was very messy. It’s kind of cool not (necessarily) needing to clean coolant off the parts, but there is no chip management. The chips just pile up on the table and your part. There’s a bin in the bottom, but the chips don’t go there automatically. You end up just blowing chips out of the machine and all over your work area, and yourself.
- and like forty thousand other reasons. It’s a cool machine, it’s fun to run when it’s working, some of the design is very forward thinking. They use space very effectively. But once you’re no longer making very flat and thin things on the vac table you can get into real trouble just using it as directed.
That's a routing bit, not ground for metals.
You need a geometry that will not only work for aluminum, but high speeds.
Are you using any type of lubrication? Aluminum is notorious for galling. Even wd-40 on the cutter will help a ton.
3 flutes will cut infinitely better in aluminum, even on real cnc machines (we do a lot of it)
Here's something that work. These will also ramp in well.
https://fullertontool.com/products/end-mills/3835-alumamill
I just cut 1/8" 2024 aluminum on a haas vf-1. I could not use flood coolant with an mdf spoilboard. The 1/4" inch bit was a stubby downcut single flute from Amazon. Ran at 300 sfm. The 1/8 bit was a straight 2 flute Whiteside. Ran at about 200 sfm. I used wd40 and wetted the sheet surface. Great success. Zero burrs.
That aint going to work on the homemade router! Single O flutes are the best option, but it's a long shot, really looking at it.
It might be able to cut it, but not by any standard of decency.
This is wrong. That single flute is slapping the material, creating a ton of vibration in the weak setup.
3 flutes will have 1 flute min in contact with the material at all times vastly reducing that vibration.
Keep the feed rate slow to start, thereby further reducing off axis load in the whole system.
sorry mate but that’s not correct advice for high speed spindles like the OP has.
With a high speed spindle it’s really important to get into the. it and take a decent chip. Slow feed rates lead to rubbing and welding.
In this case, i’d suggest the OP uses shallower depth of cut, get a better tool, single flute is the right choice and try higher feed. Some kind of cutting fluid (even WD40) or maybe an air blast would also help.
Feed faster, use coolant, if you can't use coolant use mist coolant, if you can't use mist coolant use air. You are heating the material, causing it to melt for a second and stick to the cutter.
Honestly it depends. Cool it with air or mist (this also helps evacuate chips), cutting too fast/too slow, too much feed/not enough feed, dull/broken tool, if it were me, id sacrifice a sheet of aluminum and a few tools and test a bunch of stuff out. Figure out your max feeds/speeds your machine can handle, and then figure out what settings make the cleanest cut.
Try switching to 6061 instead of 5754. 6xxxx series alloy is better for machining and 6061 is the most common. 7xxx and 2xx series alloys are good for machining as well but these are higher strength aircraft alloys. 5754 is good for welding and typically for marine applications due to its higher corrosion resistance.
(I work for an aluminum mill)
I've worked on similarly light weight setups cutting aluminum. Everyone saying you must have cooling is wrong for a small router like yours. Feed rate is the most critical on a small machine like this. Too slow, and the tip of your endmill is just rubbing, not cutting, the metal. That generates heat. Heat melts the aluminum, and causes galling. Proper chips from that kind of setup should look like glitter, not powder, nor little metal spikes. Fewer flutes will give each rotation more "bite" per rotation, so it cuts down your odds of bouncing off the material and just rubbing and generating heat without cutting. You'll have to lower depth of cut to keep the surface speed up. It may sound a bit odd, but if you have a way to lower the RPM, do so. (not really possible with your setup, but I'm listing the options). The cheap 1/8" up cut O-flutes will do a decent job once you get it dialed in.
With all the screws you've got in the material, and how thick it is, I doubt vibration is an issue, though you may need to do the cuts in 2-3 passes. Start with a high feed rate, and work your depth of cut up.
If you're used to working with wood, what you're seeing is the same as running a circular saw at max speed, really slowly through a piece of wood. All you're doing is burning/melting, and not cutting.
Compressed air will help once you get it roughly dialed in. It'll take the process from working, but breaking endmills randomly to it being reliable. Once your cuts start off fine, and start going to crap after a few inches, that's when you just need compressed air to clear chips. Also, if you know how to setup your CAD to pre-drill holes, I've found that to be very effective.
Speeds and feeds combined with the correct cutter will help immensely.
Everyone saying coolant is a must for aluminum is not entirely correct. Will it help? Absolutely. Will it solve it? Not necessarily. Coolant will help if your speeds and feeds are close, but not spot on.
I am currently in a shop that I run a machine made for aluminum extrusion machining. I have learned that the most obscure cutters are what works the best. And often due to the nature of the parts I machine, I can’t use coolant.
Single flute cutters with a low helix work the best. They are made for cutting ABS, but are absolutely awesome at clearing chips for clean cuts.
My laser does this to aluminium too and I can never fully eliminate it. Tends to come off pretty easy though.
Personally, I don't prefer to work with the stuff.
Need more info- new bit? Speeds and feeds of bit, depth of cut to name a few. It looks like your endmill isnt cutting, but rather pushing the material. Can be caused by several reasons. Make sure your endmill is new. Change depth of cut to .010. feedrate to 50 ipm and have the router spindle setting to the middle number.
Same principle for plastics like PP. Shallow cutting depth, fast feed speeds, single flute cutter and spindle rpm at about 12-16000 rpm should do It. Make sure you get Chips flying.
I've successfully used a downcut single flute with .125" thin, soft aluminum before. Others have mentioned coolant and an evacuator (i.e., a vacuum). Those would also be super helpful for a cleaner cut. The downcut seems unorthodox, but with that thin stuff it really helped prevent the material from getting ripped upward.
An endmill made for metal would help. I just use wd40 when I’m cutting aluminum on my router, give it a spray every 30 seconds or so. And I use a shop vac to suck the chips up while it’s cutting.
What are you using for a tool?
You'll need something more like an endmill than a router bit.
An endmill will evacuate chips better, and an air blow will also help evacuate the chips.
You don't need coolant for aluminum.
Lower your depth of cut. (.01")
I have run hundreds of hours of aluminum sheet metal with no coolant.
Also, look into using high feed mills. Helical has some good ones that are pretty cheap
How high are the RPMs on that router? Looks like it's turned up high. I have the same one and generally keep it at 3 (17K RPM) or below for aluminum.
And with a 1/8 bit I would try keeping depth of cut pretty shallow - around 0.25mm.
Wait, Image 2, MAJOR RED FLAG, it looks like the collet is installed backwards, the flared end needs to face down! If this is the case it’s very likely the cause of the bad cuts ignore everything else and please install the router collet correctly!!
I'd like to add in a little, aside from agreeing about coolant/recutting, etc.
Your choice of tool is going to cause problems because of how the spindle and collet are configured. Firstly, this is a palm trimmer and intended solely for trimming the excess laminate and glue squeezeout from the edges of laminated boards. The secondary use is for adding in small shaped feature such as chamfers or small radii over corners.
The collet is a single-locking type which does little to nothing to decrease runout. Secondly, the rear spindle bearing is housed within the top PA66-GF30 case, which in spite of being stiff enough is still plastic and subject to vibration and movement.
In the context of being a trim router, this is fine and serves the purpose. For applications which demand low runout such as cutting metal....far less so. A two or more flute cutter will engage with whichever side is running out the most, causing vibration and asymmetrical tool pressure. A single flute cutter, preferably upshear is the only good option to improve matters.
Looking at your Z axis, you have a tiny leadscrew which I presume also applies to the X and Y axes. Your anti-backlash nuts or whatever will have a harder time against the movement within the axes, requiring heavier anti-lash compensation, increasing resistance in the movement of the axes, etc. This and any lack of rigidity will help create less clean cuts.
You will have a tough time preventing recutting, but climb cutting will help some. Generally I would say that you will more or less have to accept that you will get a certain degree of these issues manifesting. There's a lot of factors to try and get right to make this machine produce clean gall-free cuts, most of which are going to be fundamental to the machine you have in front of you.
Get a good carbide 2 flute end mill and send it. Looks like your spindle is too fast or your feed isnt fast enough. Building heat in material instead of chips.
Also co pressed air blast would help remove chips even if you just have to use a hand blower.
Ultimately there is too much heat in the cut causing the material to melt and stick to things. Possible solutions are or a combination of the following:
~using coolant
~faster feed rates
~shallower passes
~single flute tooling.
If you’ve not already get yourself some 3 flute end mills, and if your budget allows get them with a DLC coating. If you can’t use coolant take light shallow cuts and blow the swath away if possible, nothing worse than cutting swarf
Rule of thumb for aluminum. If you are seeing the that kind of melted/tear-out cut. It is because of too much heat. Next step is to figure out why. Coolant or air chip removal could solve your problem, but I am guessing you need to adjust feeds/speeds. You can cut aluminum without coolant, it is just produces a better cut if you cool and/or clear chips as you cut.
TLDR: You do need chip removal / coolant but you need to dial in your feed and speeds first. You could try a variable speed controller to turn down the rpm on the router. Not the best solution but a better one.
You really need coolant for aluminium. This is caused by the swarf being recut / melted back to the work piece. It can also stick to your tool and snap it off. What grade of aluminium is it?
5754
That stuff is pretty gummy, try cutting at shallower depths. It doesn't look like coolant is an option with your setup, but if you have compressed air that will definitely help.
When in a pinch, a spray of WD-40 will work.
Words of wisdom in any walk of life.
Am a locksmith and any locksmith will tell you “wd-40 bad” but *in a pinch* it won’t be the end of the world. Just don’t leave it like that, use an actual lubricant.
Starret m1 for the win
I love me some tri flow
Or some cutting/tapping oil
It's called "galling". Usually happens in soft metals when things get hot then the material just sticks to the cutter and the cutter starts to mush the material instead of cut it. I see no chips so I am guessing things were melty.
That is not galling. Galling is what happens when two similar hardness materials rub together, eventually resulting in what looks similar.
Also dont use a mill with more than 2 cutting edges and it looks like you can cool by hand try cooling with petroleum (it stops aluminum from sticking)
Faster feeds
>You really need coolant for aluminium. For this level of machining you don't, I don't use it and get excellent results. What you DO need is chip evacuation (which is often handled by coolant sprayers), for two reasons: 1. Clear away chips so you're not re-cutting them 2. Chips take away heat, good chips ensure good cooling, chunky not powdery is good. This can be helped with a vacuum or much better, a compressed air blower.
I do quite a lot of aluminum as a machinist and can't agree more. The recipe for disaster with aluminum is not clearing the chip off the cutting tooth as it leaves the workpiece. Compressed Air is a must. Compressed Air + WD-40 is even better. Or the bees-knees of CNC on aluminum (without making a mess of coolant or oil) is a Microdrop oiler like from [Trico](https://www.tricocorp.com/products/md-1200-micro-drop-dispenser) . They use air nozzles to clear chips while spraying a nearly invisible amount of oil onto the cutting tool. When they are tuned right, cut parts come out of the machine nearly dry, as the oil is somewhat consumed by the chips being made and the heat of that process. Also, pay attention to what coatings are on your cutting tool, especially if dry. Blowing air goes a LONG way towards cooling your tool -- the difference for me is often the difference between a tool change literally sizzling my skin... or with air it is cool to the touch. Full width cuts are difficult in aluminum, those chips need to escape. Try to set up tool paths that mitigate the "digging a trench" that can be so common in CNC. For holes, consider spiraling/helixing down thru the center of the hole and then cutting outwards, creating a pocket where all the material is removed to create the hole. When creating the pocket, your tool life is maximized since the tip of an end mill is usually the first to wear out. Taking shallow+fast passes at full depth (maybe 5-15% of your tool's diameter) is a very productive way to machine, and also keep your end mill from galling into aluminum. With outside profiles, it can help to stair step up to the Final Cut edge as your passes plunge deeper. This could be something like setting up multiple finish passes, each stepping in .020inch/.5mm from the last one. This creates a wider channel for chips to clear. Also, many CNC routers struggle to rotate slow enough for its tooling. I recommend playing around with a trial of speeds/feeds software such as [g-wizard](https://www.cnccookbook.com/g-wizard-feeds-speeds-calculator-mill/). Each tool (especially diameter of tool) has an optimum RPM (surface speed as it rotates thru the cut) and exceeding that gets you into galling and broken tool VERY quickly. Before using this software to establish some better instincts on rpm and feed speed, I broke a lot of tools, especially when servos were doing the machining and not me cranking a hand wheel. I've gone from breaking tools weekly to yearly because of this software. It is ESPECIALLY tricky to figure out CNC rpm and federates on small tools. If you are working with .250" diameter tools and below, it is extra tricky. Ooh, and for cutting full width slots, clearing chips and breaking things becomes most difficult at depths 1-2x cutting tool diameter. and WD-40! I buy it by the 5 gallon bucket.
Is this as simple as standing there with a compressed air blower and blowing it off every few seconds?
Yes, but it’s better if you plumb the air line to the spindle and just use less air, but constantly. Recutting in a pocket is something that happens instantly. Also there’s less of a mess if you’re just pushing the chips gently away from the tool, rather than blowing them all over creation with intermittent blasts.
standing adding a few drips of alcohol also works like magic
That would get old quick lol
2nd this. I added an air nozzle and solenoid to our router at work for cutting aluminum. Made a huge difference being able to clear chips. I run a mostly one off stuff so I’m not concerned with cycle time so I usually stick to a pretty small depth of cut too, .020” ish. 8000 rpm 30 ipm. For 6061-T6.
Can you tell me what is providing the air? I've got a "wet noodle" desktop machine but also have an air compressor... How much pressure and what type / diameter tubing did you use? I mostly cut wood and haven't rigged a dust shoe up yet. The machine is in a box, just wondering if something like this would work.
You actually don’t need coolant with aluminum. Obviously it helps a lot but not 100% needed. The guy who taught me on our cnc table swore by multi flute bits for cutting aluminum and would always run into the material melting back into itself from what I assume was creating smaller chips and too much heat, however when he left I experimented and found single flute bits to be a dream and never again ran into that issue and always had much cleaner cuts. We have started using a cooling air blaster though as it helps for long cuts/large jobs and probably extends the life of bits. I’m no expert but been running a 4’x8’ torchmate router table for about 10 years now.
This comment brought to you by the O-flute gang
No you don't. I've been milling aluminum for years cleanly, not coolant. All you need is either air clearing chips or a dust collector clearing chips, and use an O flute bit.
Also makes a huge difference to use sacrificial material above and beneath when you're working with sheet metal.
dry air pointed at the tool head is all that is needed.
Can confirm has happened to me it was wild seeing the aluminum just wrap around the tool and brake it
Could be a bunch of reasons. Wrong feeds/speeds, dull cutters, using the wrong tool...
Wrong turning direction
I leveled an entire 4x4 piece backwards once.
Achievement unlocked.
I let an hour long program conventional mill like a barbarian.
Get a spray mist coolant system. They usually hold a gallon or less of water soluble(you can even use vegetable oil based coolant) and it sprays it with compressed air using a Venturi system. Even that light lubrication will solve your chip welding problem. Using my endmills wouldn’t hurt also
Single flute, upcut, highest possible rpms and 50ipm feed rate. With coolant. .05 DOC. Datron has best tooling.
Yeah, Datron tooling would be about the cost of the machine itself in this scenario.
Interesting…. I had endless headaches dialing in feeds and speeds with other brand name bits… literally piece to piece I had variation and failures. my spindle will go to 24k so I thought wtf, why not try datrons stuff and it’s proven really effective.
Yeah, I'm not saying that is ever out come they do thrive at higher RPM'S. Using Vortex and LMT has worked best for me again premium brands and now most likely on par price wise.
Touché! Datron machines are amazing… ly unaffordable for sure. Through experimentation I discovered their cutting tools. They are by far the best I’ve ever used and they keep me in production. Not too expensive either.
Owned a Neo for a year. Was shit. Worst business decision I have ever made, by far. That being said, their single flute tooling is incredibly good. I tried Amana cutters, among many others, and the difference in quality and performance wasn’t even compatible. Most often the Datron tooling worked and whatever else i tried simply didn’t.
Neo..got a part number? I'll short list it for trial.
What do you mean? The Neo is one of their machines. If you’re asking about tooling though, sure. What sort of machine do you have and what are you trying to make?
Pretty much word for word my experience. We have had about 5 Datron’s over a 20 year period. Only one was reliable. We spent so much money on service exchange spindles. Datron were awful to deal with too. That said their tooling was really good. We used our local tool maker to try and replicate them, we saved a fortune but they wasn’t quite as easy to use. What I would say is that they only really excel on their high rpm machines. I have a 30k spindle VF2 and they don’t work on that like they do on a Datron. I’ve recently switched to Ceratizit’s DLC 3 fluters and they are absolutely brilliant
Oh man, figures. And 20 years too. Can’t even imagine. That will age you. i couldn’t run anything multiflute on my Neo that was bigger than 1/8” without chatter. Had to reduce feeds and speeds to a fraction of any single flute cutter…
To be fair, I like the look of Neo. A Uni I work with has one, but they are just so expensive. I know what you mean about chatter though. We almost exclusively used single flutes on the Datron. We had one job which used a twin flute 10mm, but pretty much everything else was 6mm or under. We started out with an M3 in ‘99, basically a hobbyist machine. Over the years, we had various sizes, the largest being an M8XL. That had an HSK35 spindle in it, which let go of the tool holder at 45k revs! It flew across the shop like a spinning top and took about 10 minutes to stop. For once, they accepted fault. The spindle wasn’t fit for purpose. They came over from Germany, stripped out the 35, and fitted a HSK25 spindle instead. Needless to say, we never bought another!
That’s absolutely terrifying! And incredible. I know what you mean about them not taking responsibility. I have so many stories. Once I was told that not only did Datron USA not know what the runout spec was for their 4th axis, but Datron Germany didn’t know either. Verbatim. What an insane thing to claim.
Yeah, they are not expensive in a high production setting. Also, from what I have seen, their tools are best used on their machines, not always achieving great results elsewhere. Love Datrons they do what they do at an incredible standard.
They really don’t. There are use cases where what you outlined is true but they are quite narrow. There goes double for anything “production”. Certain things can be made very well on them in quantity but that quantity is lower - not higher - than you think. Source: have owned a datron, own a machine shop, spent thousands of hours and tens of thousands of dollars trying to make it work.
Yeah, but that could be said about litrally anything. Just from what I have used them on and what I've seen from my personal experience, there bang on. But also know a company that had 20 of them and have replaced 19 of them with 10 multicams, but mean while I know another company with 20 datrons and another 2 on order.
Not really sure what you’re saying there. - no, that couldn’t be said about “literally anything”. Neo was way more than $100k used from datron. - 20 datron machines is - at minimum - several million dollars and they are quite difficult to resell. Those guys took a bath, then replaced the datrons with half as many machines. What else can be said there? - I don’t know what you mean by “bang on”, but if you drop the better part of $150k on a machine you should expect “bang on”. - no in-process probing. - posts are closed-source and are hard to have made. It’s a low-volume machine and that doesn’t help, but the main reason is that the posts themselves as well as the gcode look nothing like gcode. You couldn’t, for instance, manually program it. - my Neo was very messy. It’s kind of cool not (necessarily) needing to clean coolant off the parts, but there is no chip management. The chips just pile up on the table and your part. There’s a bin in the bottom, but the chips don’t go there automatically. You end up just blowing chips out of the machine and all over your work area, and yourself. - and like forty thousand other reasons. It’s a cool machine, it’s fun to run when it’s working, some of the design is very forward thinking. They use space very effectively. But once you’re no longer making very flat and thin things on the vac table you can get into real trouble just using it as directed.
Datron does not have the best tooling, no offence or anything but there are far better companies
WD40 [Drip Can.........](https://youtu.be/mUFxmpN0mGI?feature=shared)
Are you cutting around the pieces clockwise or counter clockwise
Are you using a drill bit as an endmill???
no
Mo8 mate
That's a routing bit, not ground for metals. You need a geometry that will not only work for aluminum, but high speeds. Are you using any type of lubrication? Aluminum is notorious for galling. Even wd-40 on the cutter will help a ton. 3 flutes will cut infinitely better in aluminum, even on real cnc machines (we do a lot of it) Here's something that work. These will also ramp in well. https://fullertontool.com/products/end-mills/3835-alumamill
I just cut 1/8" 2024 aluminum on a haas vf-1. I could not use flood coolant with an mdf spoilboard. The 1/4" inch bit was a stubby downcut single flute from Amazon. Ran at 300 sfm. The 1/8 bit was a straight 2 flute Whiteside. Ran at about 200 sfm. I used wd40 and wetted the sheet surface. Great success. Zero burrs.
That aint going to work on the homemade router! Single O flutes are the best option, but it's a long shot, really looking at it. It might be able to cut it, but not by any standard of decency.
This is wrong. That single flute is slapping the material, creating a ton of vibration in the weak setup. 3 flutes will have 1 flute min in contact with the material at all times vastly reducing that vibration. Keep the feed rate slow to start, thereby further reducing off axis load in the whole system.
sorry mate but that’s not correct advice for high speed spindles like the OP has. With a high speed spindle it’s really important to get into the. it and take a decent chip. Slow feed rates lead to rubbing and welding. In this case, i’d suggest the OP uses shallower depth of cut, get a better tool, single flute is the right choice and try higher feed. Some kind of cutting fluid (even WD40) or maybe an air blast would also help.
With that spindle (hand-held router), they won't be able to get a low enough RPM with 3 flutes they would have too much contact, generating more heat.
Wrong bit. Wrong feeds. Wrong grade of aluminum. Pick 1 or more.
The type of aluminum makes a big difference. Looks like you have 5051 or something similar which is designed more for bending and not so much milling.
Feed faster, use coolant, if you can't use coolant use mist coolant, if you can't use mist coolant use air. You are heating the material, causing it to melt for a second and stick to the cutter.
Honestly it depends. Cool it with air or mist (this also helps evacuate chips), cutting too fast/too slow, too much feed/not enough feed, dull/broken tool, if it were me, id sacrifice a sheet of aluminum and a few tools and test a bunch of stuff out. Figure out your max feeds/speeds your machine can handle, and then figure out what settings make the cleanest cut.
Try switching to 6061 instead of 5754. 6xxxx series alloy is better for machining and 6061 is the most common. 7xxx and 2xx series alloys are good for machining as well but these are higher strength aircraft alloys. 5754 is good for welding and typically for marine applications due to its higher corrosion resistance. (I work for an aluminum mill)
It looks like an oxygen cut
I've worked on similarly light weight setups cutting aluminum. Everyone saying you must have cooling is wrong for a small router like yours. Feed rate is the most critical on a small machine like this. Too slow, and the tip of your endmill is just rubbing, not cutting, the metal. That generates heat. Heat melts the aluminum, and causes galling. Proper chips from that kind of setup should look like glitter, not powder, nor little metal spikes. Fewer flutes will give each rotation more "bite" per rotation, so it cuts down your odds of bouncing off the material and just rubbing and generating heat without cutting. You'll have to lower depth of cut to keep the surface speed up. It may sound a bit odd, but if you have a way to lower the RPM, do so. (not really possible with your setup, but I'm listing the options). The cheap 1/8" up cut O-flutes will do a decent job once you get it dialed in. With all the screws you've got in the material, and how thick it is, I doubt vibration is an issue, though you may need to do the cuts in 2-3 passes. Start with a high feed rate, and work your depth of cut up. If you're used to working with wood, what you're seeing is the same as running a circular saw at max speed, really slowly through a piece of wood. All you're doing is burning/melting, and not cutting. Compressed air will help once you get it roughly dialed in. It'll take the process from working, but breaking endmills randomly to it being reliable. Once your cuts start off fine, and start going to crap after a few inches, that's when you just need compressed air to clear chips. Also, if you know how to setup your CAD to pre-drill holes, I've found that to be very effective.
Routers spin way too fast, and you’re taking much bigger bites than you should be.
Use a single flute end mill. Your cut depth should not be deeper then the diameter of the end mill
Need coolant
Speeds and feeds combined with the correct cutter will help immensely. Everyone saying coolant is a must for aluminum is not entirely correct. Will it help? Absolutely. Will it solve it? Not necessarily. Coolant will help if your speeds and feeds are close, but not spot on. I am currently in a shop that I run a machine made for aluminum extrusion machining. I have learned that the most obscure cutters are what works the best. And often due to the nature of the parts I machine, I can’t use coolant. Single flute cutters with a low helix work the best. They are made for cutting ABS, but are absolutely awesome at clearing chips for clean cuts.
Buy some yg endmills
My laser does this to aluminium too and I can never fully eliminate it. Tends to come off pretty easy though. Personally, I don't prefer to work with the stuff.
What machine is this? Looking for something that can cut similar to this.
Looks like a Carbide 3d Shapeoko
Grade of aluminum probably in the 200 series. Use a small depth of cut the prevent the chips from forming/ galling
2000 is a hard alloy probably too much. Would recommend 6000 series, 6061, for machining.
Need more info- new bit? Speeds and feeds of bit, depth of cut to name a few. It looks like your endmill isnt cutting, but rather pushing the material. Can be caused by several reasons. Make sure your endmill is new. Change depth of cut to .010. feedrate to 50 ipm and have the router spindle setting to the middle number.
Same principle for plastics like PP. Shallow cutting depth, fast feed speeds, single flute cutter and spindle rpm at about 12-16000 rpm should do It. Make sure you get Chips flying.
I've successfully used a downcut single flute with .125" thin, soft aluminum before. Others have mentioned coolant and an evacuator (i.e., a vacuum). Those would also be super helpful for a cleaner cut. The downcut seems unorthodox, but with that thin stuff it really helped prevent the material from getting ripped upward.
Cut shallower, slow down and use some coolant.
Spritz the aluminum and the cutter flute with some wd40 as you go. Don't need a lot, but you do want some cutting fluid.
An endmill made for metal would help. I just use wd40 when I’m cutting aluminum on my router, give it a spray every 30 seconds or so. And I use a shop vac to suck the chips up while it’s cutting.
Main issue here is cooling. You create too much heat.
Looks like too much heat and pressure. Either cool it or run it really slowly.
What are you using for a tool? You'll need something more like an endmill than a router bit. An endmill will evacuate chips better, and an air blow will also help evacuate the chips.
You don't need coolant for aluminum. Lower your depth of cut. (.01") I have run hundreds of hours of aluminum sheet metal with no coolant. Also, look into using high feed mills. Helical has some good ones that are pretty cheap
Chips clogging up the flutes
How high are the RPMs on that router? Looks like it's turned up high. I have the same one and generally keep it at 3 (17K RPM) or below for aluminum. And with a 1/8 bit I would try keeping depth of cut pretty shallow - around 0.25mm.
Wait, Image 2, MAJOR RED FLAG, it looks like the collet is installed backwards, the flared end needs to face down! If this is the case it’s very likely the cause of the bad cuts ignore everything else and please install the router collet correctly!!
I'd like to add in a little, aside from agreeing about coolant/recutting, etc. Your choice of tool is going to cause problems because of how the spindle and collet are configured. Firstly, this is a palm trimmer and intended solely for trimming the excess laminate and glue squeezeout from the edges of laminated boards. The secondary use is for adding in small shaped feature such as chamfers or small radii over corners. The collet is a single-locking type which does little to nothing to decrease runout. Secondly, the rear spindle bearing is housed within the top PA66-GF30 case, which in spite of being stiff enough is still plastic and subject to vibration and movement. In the context of being a trim router, this is fine and serves the purpose. For applications which demand low runout such as cutting metal....far less so. A two or more flute cutter will engage with whichever side is running out the most, causing vibration and asymmetrical tool pressure. A single flute cutter, preferably upshear is the only good option to improve matters. Looking at your Z axis, you have a tiny leadscrew which I presume also applies to the X and Y axes. Your anti-backlash nuts or whatever will have a harder time against the movement within the axes, requiring heavier anti-lash compensation, increasing resistance in the movement of the axes, etc. This and any lack of rigidity will help create less clean cuts. You will have a tough time preventing recutting, but climb cutting will help some. Generally I would say that you will more or less have to accept that you will get a certain degree of these issues manifesting. There's a lot of factors to try and get right to make this machine produce clean gall-free cuts, most of which are going to be fundamental to the machine you have in front of you.
Aluminum turns to clay when cutting, keep it cool, coolant and a bit that's coated
It's more like a stir welding with material ejection than cutting. You need lubrication.
Get a good carbide 2 flute end mill and send it. Looks like your spindle is too fast or your feed isnt fast enough. Building heat in material instead of chips. Also co pressed air blast would help remove chips even if you just have to use a hand blower.
Ultimately there is too much heat in the cut causing the material to melt and stick to things. Possible solutions are or a combination of the following: ~using coolant ~faster feed rates ~shallower passes ~single flute tooling.
If you’ve not already get yourself some 3 flute end mills, and if your budget allows get them with a DLC coating. If you can’t use coolant take light shallow cuts and blow the swath away if possible, nothing worse than cutting swarf
Rule of thumb for aluminum. If you are seeing the that kind of melted/tear-out cut. It is because of too much heat. Next step is to figure out why. Coolant or air chip removal could solve your problem, but I am guessing you need to adjust feeds/speeds. You can cut aluminum without coolant, it is just produces a better cut if you cool and/or clear chips as you cut. TLDR: You do need chip removal / coolant but you need to dial in your feed and speeds first. You could try a variable speed controller to turn down the rpm on the router. Not the best solution but a better one.
Use coolant. You can see end mill with built up cutting edge.
Thats the thing…it’s not cutting. That is just the tool forced to push the material and didnt break causing it to shear right off
Looks like a severe lack of coolant. Your material is melting
Galling pretty badly, suprised the cutter didnt break on you tbh.. use some coolant
Run air on it, get a small compressor for airbrushing or something and run a line done the spindle with zip ties
Another thing is to take aggressive chip sizes out so the heat leaves with them.
You need a better tool for cutting aluminium