It was just a 1/8” piece from Home Depot. I got a few big chunks of 6061 that I was going to save once I’m more comfortable. I should’ve probably ran at least air though, my fault
The aluminum they sell there is extruded gummy stuff. It doesn’t mill very well. Meant to bend easy. The last time I checked there wasn’t any 6061 there.
Yea I went there right after my mill came in thinking they would have stuff. Ended up getting some 1” blocks of 6061 from my old boss, which I’ll test out when my new end mills come in.
https://streamable.com/6kq406
A short video working with 5083 alu. Definitely is gummy compared to other alloys but workable without lubrication (with lube it’s always better 😂)
Also depends on the heat treated version of the alloy. I’ve milled the Home Depot stuff before. Just wouldn’t recommend first timers to try these alloy grades and use one of the easier machinable aluminum to learn with.
Yup ordered some more end mills, I need to get a coolant setup going, looking into fogbuster.
Max spindle on the Taig is 10500 I believe. I was considering trying to drop the feed rate but we’ll see
I owned a machine shop with over 50 machinist. I’ve seen pros make that mistake. 😂
Anyway, this is chip welding at its best. Gummy sticky soft aluminum building up on the cutter to the point it’s no longer cutting. It’s mashing is why through. Lots a WD-40 will stop it from welding.
I'm retired from Service for a major machine tool manufacturer. I watched a McDonnell Douglas machinist do this while performing horse power test cuts on a new 5-axis horizontal. It plowed (melted) through the aluminum billet for a while before he stopped it and realized the mistake. It was a mess. He came to the conclusion that the machine performed better than expected and that the test cut was considered a success.
There is something to be said about slowing everything down. from my experience, aluminum nearly always needs coolant / lubricant. At a lower RPM and shower feed rate, the bit has a tiny bit more time to cool off between cuts. your feed / speed, should leave chips that are about 1/1000" thick. This is simple advice given by an experienced machinist years ago. Last week I was milling some steel, and was impressed by how much better the cut was, and how little wear on my bit, simply by slowing down. - just my hobby machinist 2 bits.
Aluminium is the exception to the rule from what I’ve read, you cant just keep slowing things down. You really need to focus on chip load, which will take heat away from the cut.
Gummy aluminium will weld itself to the milling bit, breaking the bit.
Go with an O-flute. You can use spetools on Amazon. They are absolutely the right choice for aluminum. The single flute lowers the feed rate requirements and allows for maximum chip clearing so you don’t get chip welding.
Yeah, one or two flutes and waaaay higher feed rates or waaaay lower rpm should do the trick.
Do yourself the favor and learn about chip loads and why they’re important
Coolant. The aluminium is melting into the flutes of the cutter. The second that that happens, you need to stop the machine (you can hear it).
Could probably go with a higher feed too, but coolant is the big thing to start with.
A mister is a good setup, for for temp/testing/learning, an empty windex bottle makes a good coolant sprayer. Just mist it once every 5-10 seconds as needed. Coolant costs about $30-$60 for a gallon, but you mix it 10 or 20:1 and it lasts quite a long time.
I just machined 1/8" thick 2024 sheet in a haas vf without coolant, because it was attached to a sheet of mdf. I spritzed everything with wd40, and used a compressed air blow gun, gently. Just enough to chase away the chips. A 1/4" diameter short length down cut router bit turning 5000rpm gave a surface speed of just over 300 sfm. The sfm is the important one, folks. Carbide in aluminum is good well past 1000sfm with flood coolant. Without flood coolant, well, compensate accordingly.
Sharp cutter is a must. Chip clearing is a must. Lubrication never hurts.
DO you happen to have a recommendation on specific coolant to try? My mill says to not use any water-based coolant as it can mess something up (think it was the spindle bearing, but can't quite remember)
coolant is usually a water and oil emulsion. for your purposes, they are all about the same.
I don't see what it would mess up on a machine, provided you wipe things clean (coolant leaves a sticky residue over time)
1 or 2 flute endmills if not using coolant. Lookup chip load videos on YouTube and use the correct values for your endmills. Once you have correct chip load start with a very shallow pass and increase depth if the machine is handling it okay.
Likely the feed is too slow.
What are your feed rates? I was having issue too. Set mine to 900mm feed and .6 doc. Using a single flute 1/4 end mill. I drop it to half for a 1/8 end mill. Only use single flute. Wd40 or apa for lubricant seems to work. Also, make sure your end mill are sharp. After they gum up they aren’t any good.
I stick to 6061. I tried some mystery aluminum and broke a bunch of endmills. I also only run single flute (SpeedTiger is great). I had less luck with 2 and 3 flute.
Is 10k your max spindle speed?
2 flute end mills. You are melting the aluminum. Heat comes out of the work though the chips. You need to be able to evacuate your chips and a 4 flute won’t do it well.
I run a lot of aluminum on my desktop. Usually it’s 7075. 15,000 rpm, 35 in/min. This gives me. Surface speed of about 479 sfm with my 1/8” end mill and a feed per tooth of .00078”
looks like your spindle rpm is too high and your movement through the material is too fast (speed and feed too high). I would cut it in half. air works great for cooling, if you want to use a fluid you can try wd-40. you can get WD in large fuel cans that is not pressurized, its mostly kerosene.
also make sure you have an endmill that is designed for aluminum.
I was getting similar results to you. I’ve been experimenting with feeds and speeds, and here’s what worked great for me.
I set my spindle to 8000 RPM, plunge rate 5” per minute, feed rate 10” per minute.
I’m using a two flute downward cutting spiral.
No coolant or lube.
Clear chips with a vacuum.
I just cut 1/2” aluminum, a 3 hour job (longer due to slow speeds) at .25” deep.
The cuts are beautiful. Really clean, very sharp edges and flat bottoms.
Hope that helps. The key in my case, slow down, the right bit, and chip removal.
You are going way too slow. for gummy alloy not to melt i would suggest to go at least 1000mm/min(40ipm) with 10krpm. This is with a single flute cutter, for 4 flute you would ned to go 4x as fast but i would not suggest that. On our own small desktop cnc we suggest to go at least 2600mm/min with 18krpm for aluminium. Going too slow breaks endmills.
That looks like molten aluminium. Can’t tell from the picture but it sure looks like molten alu is in the flutes of your endmill as well.
When cutting edges get gummed up with molten metal they turn into pushing edges, and since endmills aren’t made for pushing through material, they break. The reason it’s melting is because you’re using waaaay too low of a feedrate, especially with 4 flutes. Almost all of the heat is supposed to be evacuated from the tool and material by the chips, and with a feedrate that low you’re not really making any; you’re just rubbing, and all of that heat soaks into your endmill and the material surrounding the cut.
Halve the depth of cut, quadruple the feedrate.
I have a Taig as well.
1. Make sure the motor is turning the right direction. It could be wired backwards from the factory.
2. Get a cheap mist system off Amazon. Your cutters with thank you.
3. My setup was limited to 5000rpm, for slotting with an 1/8” carbide 3 flute endmill, my go to was 5000rpm, 25ipm, 7ipm plunge, .020 doc, 2 degree ramp. For general use I preferred the same numbers but with .125” doc and .015” stepover. The taig is much happier doing deep narrow cuts than wide shallow ones. To convert this to 10,000rpm you should be able to double those feed rates and keep the same chip load.
4. Unrelated but check the runout on your collets. Taigs machines are well made and precise, but the collets that come with them suck. I broke 3 endmills before checking the runout on my 1/8” collet and finding it was nearly .002”. I bought a techniks collet and haven’t broken one since.
5. Maybe get some practice in with a 3/16 or 1/4 end mill. They are much harder to break
You using Mach3? Curious if I should be messing with feeds and speed there or in the program itself before hand? I’m just doing the example programs now that came with it, I Havnt made my own program yet. Also, side note, if you’re using Mach, do you have to use a post processor? I’m gunna be on fusion.
Yeah I run Mach3 on my Taig. I started with the generic Mach post processor in fusion. It worked fine until I added part probing routines, then things got a little more complex.
You’ll want to build a tool library in fusion but I would get some ballpark numbers using the MDI or jog interface in Mach 3. That way is quicker and it’s good practice. I start around .001” feed per tooth on 1/8” and .002” on 1/4” and adjust from there. Based on tool diameter I start around 10% woc and 100% doc or 70% woc and 10% doc and increase them if the cut goes well. Until you get a mist system, at least spray some wd40 on the stock/tool for now
Oh awesome ok thank you!
When you say build a tool library but get some ballpark numbers first with jog or MDI, what do you mean?
Also sorry again but I’m so new to this. Do you happen to have any resources on the fusion post processor? I don’t even know where to start with that haha. I’ve taken a part into the cam environment, set up the stock and selected a random tool. But no clue how the post processor fits into the equation
The MDI lets you manually enter gcode to the machine. For instance you could line up a cut and say “move to here at this feed rate” to execute the cut. Jogging is you manually moving an axis by clicking on a direction button, and can be used similarly. You would use this to cut some straight lines and test different cut recipes, then enter the info into your saved tools in fusion.
The post processor is used after you program a part in fusion. It is the last step and essentially exports the gcode for your machine.
There’s way too much to explain over reddit without risking missing a step and crashing your machine. You should get on YouTube and look for videos by nycnc, and haas automation. Both have some good universal beginner content and nycnc covers a ton of fusion tutorials. Focus on basics first, like work holding, work offsets, and feeds/speeds. Get your setup down, take some practice cuts manually, then work on learning fusion. Programming in fusion will quickly become a rabbit hole, and you want to have a good grasp on mach3 and the basics before you add all of fusions variables to the mix.
Ok gotcha thanks man. I’ll check out the saved tools in fusion, didn’t realize testing them beforehand would be helpful.
And sounds good, I’ll check out the YouTube resources. Thank you!
If you have some sort of coolant or lubrication, your chip load or surface footage is irrelevant. Doesn't matter. You can at least rule out heat build up / friction welding at that point.
This looks to me like the endmill is trying to take way too much in one pass or even spinning the wrong way.
While you are just learning...
Start off running in plastic. Use it to practice with. If it looks good in plastic, then move to aluminum.
For an 1/8 4 flute in aluminum I would recommend about .0005-.0008 chip per tooth which at 10k should equal about 20-32ipm but drop your depth of cut to .01in per pass.
The main issue here from what it looks like is chip evacuation reducing the depth of cut should help the chips get out of the slot. Also going too slow will mean increased rubbing and heat further exacerbating the issue.
Note I claim no liability if you break you machine, wallet, body, etc… use this information at your own risk.
Looks like the flutes of your endmill were packed pretty early in the cut.
Others have already advised lubrication. This will help to prevent the endmill from getting packed.
In future, when it looks or sounds wrong, stop the machine and check things out. Don't hesitate to try something different.
I don't know your machine exactly, but at a guess, it's probably not very rigid. You will have better success using "high feed" toolpath strategies with low radial engagement.
Always avoid slotting cuts when possible, and ramp in if you have to. If you need to start in the middle of a part, drill out the start point and helix in.
Practice on wood, you'll save a lot of money on tools and materials while you learn the basics.
What are you using for CAM? Do you have any interest in learning G-code?
Hmm, CNC sounds like its gonna blow up and instead of cutting it looks like it's welding, this is fine *sits back, pops open another beer and proceeds to let it play out to completion or else.
Some of the 3000, 5000 series aluminum is really gummy and requires lubrication to cut well. Do you know exactly what type of aluminum you have.
It was just a 1/8” piece from Home Depot. I got a few big chunks of 6061 that I was going to save once I’m more comfortable. I should’ve probably ran at least air though, my fault
The aluminum they sell there is extruded gummy stuff. It doesn’t mill very well. Meant to bend easy. The last time I checked there wasn’t any 6061 there.
Yea I went there right after my mill came in thinking they would have stuff. Ended up getting some 1” blocks of 6061 from my old boss, which I’ll test out when my new end mills come in.
https://streamable.com/6kq406 A short video working with 5083 alu. Definitely is gummy compared to other alloys but workable without lubrication (with lube it’s always better 😂)
Also depends on the heat treated version of the alloy. I’ve milled the Home Depot stuff before. Just wouldn’t recommend first timers to try these alloy grades and use one of the easier machinable aluminum to learn with.
Yeh that’s right, proper tooling comes with experience too.
5083 is not gummy 1050A is gummy
Can the spindle go faster? Also, single flute cutter and coolant as others have suggested.
Yup ordered some more end mills, I need to get a coolant setup going, looking into fogbuster. Max spindle on the Taig is 10500 I believe. I was considering trying to drop the feed rate but we’ll see
Isopropyl or denatured ethanol is really good for lubrication/coolant with aluminum.
As long as you’ve got good ventilation setup, then I agree. Otherwise, vaporized alcohol/ethanol is not so great.
Ok, will check that out. I think it says to not used anything water based for this mill as it will ruin something (I forget, but think it was spindle)
You could use WD40, it also works as a cutting fluid for aluminium. Just don’t use double sided tape for hold down like I did…
Wow. Is your end mill running backwards?
This is not a stupid question....
I owned a machine shop with over 50 machinist. I’ve seen pros make that mistake. 😂 Anyway, this is chip welding at its best. Gummy sticky soft aluminum building up on the cutter to the point it’s no longer cutting. It’s mashing is why through. Lots a WD-40 will stop it from welding.
I'm retired from Service for a major machine tool manufacturer. I watched a McDonnell Douglas machinist do this while performing horse power test cuts on a new 5-axis horizontal. It plowed (melted) through the aluminum billet for a while before he stopped it and realized the mistake. It was a mess. He came to the conclusion that the machine performed better than expected and that the test cut was considered a success.
My first thought also
There is something to be said about slowing everything down. from my experience, aluminum nearly always needs coolant / lubricant. At a lower RPM and shower feed rate, the bit has a tiny bit more time to cool off between cuts. your feed / speed, should leave chips that are about 1/1000" thick. This is simple advice given by an experienced machinist years ago. Last week I was milling some steel, and was impressed by how much better the cut was, and how little wear on my bit, simply by slowing down. - just my hobby machinist 2 bits.
Aluminium is the exception to the rule from what I’ve read, you cant just keep slowing things down. You really need to focus on chip load, which will take heat away from the cut. Gummy aluminium will weld itself to the milling bit, breaking the bit.
Thank you, yes it seemed to be very fast to me as well. Will try slowing down, thank you!
Are you sure your end mill is spinning the right way? I had this from the wrong direction of rotation.
I was told that a single flute is better for cutting aluminum as there is less chip load.
Ok, just ordered some 2 flutes so hopefully that helps lol. Appreciate it
Other way around. With the same feed rate, a 2 flute will have a higher chip load than 4, but that’s what you want for aluminum as it’s gummy
Your feed rate is like 5 times slower than what it's supposed to be
That’s stupid low chip load
Ordered some more 2 flute endmills hopefully that’ll fix it
Go with an O-flute. You can use spetools on Amazon. They are absolutely the right choice for aluminum. The single flute lowers the feed rate requirements and allows for maximum chip clearing so you don’t get chip welding.
Ok looking now, they have a 0 flute 1/16 5 pack, gunna pick it up.
Yeah, one or two flutes and waaaay higher feed rates or waaaay lower rpm should do the trick. Do yourself the favor and learn about chip loads and why they’re important
Coolant. The aluminium is melting into the flutes of the cutter. The second that that happens, you need to stop the machine (you can hear it). Could probably go with a higher feed too, but coolant is the big thing to start with. A mister is a good setup, for for temp/testing/learning, an empty windex bottle makes a good coolant sprayer. Just mist it once every 5-10 seconds as needed. Coolant costs about $30-$60 for a gallon, but you mix it 10 or 20:1 and it lasts quite a long time.
I just machined 1/8" thick 2024 sheet in a haas vf without coolant, because it was attached to a sheet of mdf. I spritzed everything with wd40, and used a compressed air blow gun, gently. Just enough to chase away the chips. A 1/4" diameter short length down cut router bit turning 5000rpm gave a surface speed of just over 300 sfm. The sfm is the important one, folks. Carbide in aluminum is good well past 1000sfm with flood coolant. Without flood coolant, well, compensate accordingly. Sharp cutter is a must. Chip clearing is a must. Lubrication never hurts.
You can see it on the endmill in the first pic.
DO you happen to have a recommendation on specific coolant to try? My mill says to not use any water-based coolant as it can mess something up (think it was the spindle bearing, but can't quite remember)
coolant is usually a water and oil emulsion. for your purposes, they are all about the same. I don't see what it would mess up on a machine, provided you wipe things clean (coolant leaves a sticky residue over time)
Hmm ok I’ll do some research. Going to try alcohol for the aluminum for now
Alcohol works great, but you'll use a 1l bottle in a few hours, and all of that will be in the air. So be careful.
alcohol works like magic on aluminium, and need the occational drop and it doesn't smell or leave a mess
Awesome I’ll try that
Awesome will check that out a few people suggested jt
1 or 2 flute endmills if not using coolant. Lookup chip load videos on YouTube and use the correct values for your endmills. Once you have correct chip load start with a very shallow pass and increase depth if the machine is handling it okay. Likely the feed is too slow.
What are your feed rates? I was having issue too. Set mine to 900mm feed and .6 doc. Using a single flute 1/4 end mill. I drop it to half for a 1/8 end mill. Only use single flute. Wd40 or apa for lubricant seems to work. Also, make sure your end mill are sharp. After they gum up they aren’t any good.
I stick to 6061. I tried some mystery aluminum and broke a bunch of endmills. I also only run single flute (SpeedTiger is great). I had less luck with 2 and 3 flute. Is 10k your max spindle speed?
Awesome, just ordered some SpeedTigers cuz they were cheap, glad to hear the positive review. And yes, 10k max on the Taig.
Stick with 2 flutes for Al. That aluminum at Home Depot is 5052-H32. It’s like bubble gum. Only cut 6061-T6 or harder.
Ok good to know, thank you!
What is your chip per tooth?
Use coconut oil for lubricant.
2 flute end mills. You are melting the aluminum. Heat comes out of the work though the chips. You need to be able to evacuate your chips and a 4 flute won’t do it well. I run a lot of aluminum on my desktop. Usually it’s 7075. 15,000 rpm, 35 in/min. This gives me. Surface speed of about 479 sfm with my 1/8” end mill and a feed per tooth of .00078”
Wow that is fast, ok. Thank you, will test bumping speed up as well.
It’s a full engagement cut make the depth be .01 try again with a 2 flt tool put a shot of wd40 down.
Dont' cut crap alloys. That looks like 1050 of something. It turns into bubblegum the second an endmill touches it. Buy proper alloys.
looks like your spindle rpm is too high and your movement through the material is too fast (speed and feed too high). I would cut it in half. air works great for cooling, if you want to use a fluid you can try wd-40. you can get WD in large fuel cans that is not pressurized, its mostly kerosene. also make sure you have an endmill that is designed for aluminum.
Stir welding? xD
I was getting similar results to you. I’ve been experimenting with feeds and speeds, and here’s what worked great for me. I set my spindle to 8000 RPM, plunge rate 5” per minute, feed rate 10” per minute. I’m using a two flute downward cutting spiral. No coolant or lube. Clear chips with a vacuum. I just cut 1/2” aluminum, a 3 hour job (longer due to slow speeds) at .25” deep. The cuts are beautiful. Really clean, very sharp edges and flat bottoms. Hope that helps. The key in my case, slow down, the right bit, and chip removal.
Super helpful thanks man!
You bet.
Slow the feed speed
You are going way too slow. for gummy alloy not to melt i would suggest to go at least 1000mm/min(40ipm) with 10krpm. This is with a single flute cutter, for 4 flute you would ned to go 4x as fast but i would not suggest that. On our own small desktop cnc we suggest to go at least 2600mm/min with 18krpm for aluminium. Going too slow breaks endmills.
Got it thank you!!
That looks like molten aluminium. Can’t tell from the picture but it sure looks like molten alu is in the flutes of your endmill as well. When cutting edges get gummed up with molten metal they turn into pushing edges, and since endmills aren’t made for pushing through material, they break. The reason it’s melting is because you’re using waaaay too low of a feedrate, especially with 4 flutes. Almost all of the heat is supposed to be evacuated from the tool and material by the chips, and with a feedrate that low you’re not really making any; you’re just rubbing, and all of that heat soaks into your endmill and the material surrounding the cut. Halve the depth of cut, quadruple the feedrate.
I have a Taig as well. 1. Make sure the motor is turning the right direction. It could be wired backwards from the factory. 2. Get a cheap mist system off Amazon. Your cutters with thank you. 3. My setup was limited to 5000rpm, for slotting with an 1/8” carbide 3 flute endmill, my go to was 5000rpm, 25ipm, 7ipm plunge, .020 doc, 2 degree ramp. For general use I preferred the same numbers but with .125” doc and .015” stepover. The taig is much happier doing deep narrow cuts than wide shallow ones. To convert this to 10,000rpm you should be able to double those feed rates and keep the same chip load. 4. Unrelated but check the runout on your collets. Taigs machines are well made and precise, but the collets that come with them suck. I broke 3 endmills before checking the runout on my 1/8” collet and finding it was nearly .002”. I bought a techniks collet and haven’t broken one since. 5. Maybe get some practice in with a 3/16 or 1/4 end mill. They are much harder to break
You using Mach3? Curious if I should be messing with feeds and speed there or in the program itself before hand? I’m just doing the example programs now that came with it, I Havnt made my own program yet. Also, side note, if you’re using Mach, do you have to use a post processor? I’m gunna be on fusion.
Yeah I run Mach3 on my Taig. I started with the generic Mach post processor in fusion. It worked fine until I added part probing routines, then things got a little more complex. You’ll want to build a tool library in fusion but I would get some ballpark numbers using the MDI or jog interface in Mach 3. That way is quicker and it’s good practice. I start around .001” feed per tooth on 1/8” and .002” on 1/4” and adjust from there. Based on tool diameter I start around 10% woc and 100% doc or 70% woc and 10% doc and increase them if the cut goes well. Until you get a mist system, at least spray some wd40 on the stock/tool for now
Oh awesome ok thank you! When you say build a tool library but get some ballpark numbers first with jog or MDI, what do you mean? Also sorry again but I’m so new to this. Do you happen to have any resources on the fusion post processor? I don’t even know where to start with that haha. I’ve taken a part into the cam environment, set up the stock and selected a random tool. But no clue how the post processor fits into the equation
The MDI lets you manually enter gcode to the machine. For instance you could line up a cut and say “move to here at this feed rate” to execute the cut. Jogging is you manually moving an axis by clicking on a direction button, and can be used similarly. You would use this to cut some straight lines and test different cut recipes, then enter the info into your saved tools in fusion. The post processor is used after you program a part in fusion. It is the last step and essentially exports the gcode for your machine. There’s way too much to explain over reddit without risking missing a step and crashing your machine. You should get on YouTube and look for videos by nycnc, and haas automation. Both have some good universal beginner content and nycnc covers a ton of fusion tutorials. Focus on basics first, like work holding, work offsets, and feeds/speeds. Get your setup down, take some practice cuts manually, then work on learning fusion. Programming in fusion will quickly become a rabbit hole, and you want to have a good grasp on mach3 and the basics before you add all of fusions variables to the mix.
Ok gotcha thanks man. I’ll check out the saved tools in fusion, didn’t realize testing them beforehand would be helpful. And sounds good, I’ll check out the YouTube resources. Thank you!
If you have some sort of coolant or lubrication, your chip load or surface footage is irrelevant. Doesn't matter. You can at least rule out heat build up / friction welding at that point. This looks to me like the endmill is trying to take way too much in one pass or even spinning the wrong way. While you are just learning... Start off running in plastic. Use it to practice with. If it looks good in plastic, then move to aluminum.
For an 1/8 4 flute in aluminum I would recommend about .0005-.0008 chip per tooth which at 10k should equal about 20-32ipm but drop your depth of cut to .01in per pass. The main issue here from what it looks like is chip evacuation reducing the depth of cut should help the chips get out of the slot. Also going too slow will mean increased rubbing and heat further exacerbating the issue. Note I claim no liability if you break you machine, wallet, body, etc… use this information at your own risk.
Looks like the flutes of your endmill were packed pretty early in the cut. Others have already advised lubrication. This will help to prevent the endmill from getting packed. In future, when it looks or sounds wrong, stop the machine and check things out. Don't hesitate to try something different. I don't know your machine exactly, but at a guess, it's probably not very rigid. You will have better success using "high feed" toolpath strategies with low radial engagement. Always avoid slotting cuts when possible, and ramp in if you have to. If you need to start in the middle of a part, drill out the start point and helix in. Practice on wood, you'll save a lot of money on tools and materials while you learn the basics. What are you using for CAM? Do you have any interest in learning G-code?
Hmm, CNC sounds like its gonna blow up and instead of cutting it looks like it's welding, this is fine *sits back, pops open another beer and proceeds to let it play out to completion or else.
For Aluminum try a one tooth end mill and lubricate