Hey guys: I have my C-Beam Machine up and running, and have done a few test cuts in plywood. All seems to be well. My question relates to cutting bits. I have been looking around, and found several options for bits. I guess the main questions are: 1. Carbide or HSS? I have found some evidence that HSS is actually better for aluminum than carbide. Not sure why, since commercial CNC tooling is generally carbide. Also, carbide is recommended for wood and plastic. Opinions? 2. Spiral Up Cut, Spiral Down Cut, or straight cutter? I tend to use spiral down cut bits for wood, because they don't splinter the surface by tearing up wood fibers. My guess would be up cut for aluminum, to clear the chips better... 3. One flute? 2? 4? Which is the best for cutting aluminum? Why? 4. Anyone have experience with the Chinese CNC bits available on Amazon and Ebay? They are certainly cheap, I have seen 10 pcs. for well under $20, but are they just crap? 5. Anyone have experience using the 1/8" spiral bits made for RotoZip and other tools of this type? They are available in spiral up and spiral down cuts. I don't know if they have the right cutting face to do plunge cuts into aluminum, they are mainly used to cut sideways against the flutes. Again, these are cheap, I saw some in a store today for $13 for 10 pcs. 6. The g-code file that came with the c-beam software seems to use a 2mm cutter. Where do you get these, and where do you get the collet adapter to fit them? I would think these would be pretty fragile... Thanks guys.
I don't cut a lot of aluminum, but I've had good luck with these on wood and aluminum: http://www.amazon.com/gp/product/B00HGZA7TG?psc=1&redirect=true&ref_=oh_aui_detailpage_o03_s00 http://www.amazon.com/gp/product/B00QLVUUNO?psc=1&redirect=true&ref_=oh_aui_detailpage_o04_s00 and these, also in 1/8", they work especially well for Baltic Birch plywood: http://www.amazon.com/gp/product/B00SMDPF4I?psc=1&redirect=true&ref_=oh_aui_detailpage_o08_s00 I use 1/8" shank carbide pc board drills for drilling and making small lettering. I can cut letters as small as 1/8" tall with .3mm drill bits. I bought a couple if 1/8" x 1/4" adapter sleeves and only use 1/4" and 1/8" shank bits. You can get 1/8" collets for some routers. Make sure your bits are center cutting end mill cutters, I think that's the term, they are better at plunge cutting. While some are better than others, I don't think I've ever found one that didn't work at all. I mostly pick the size based on what I'm making. Smaller radii and smaller pockets require smaller bits. I use regular router bits for making signs and I have some special bits made for carving 3D items. They are expensive, but sometimes, you have to have them as nothing else will do. My suggestion is just get a selection and see what works best.
Hi, in general bits are selected by chipload per tooth vs. rpm and feed. Best results if used by the manufacturers specs. Turning your bit too slow will, at some point, raise the chipload above a healty point and either break the bit or stall your router.. Turning way to fast will lower the chipload to a point where there is no more cutting but only grinding (excess heat and wear)... Go fast for soft materials, slow for hard materials. Best results in aluminium i made with "polished"single flute dedicated aluminium bits. As aluminium needs to be cut using a relative high feed (soft material) and i have a hf spindle with only little torque but high rpm that is the best compromise. (less teeth per rpm cutting keeps the feed somewhat down in sensible areas, no excess heating no melting/smearing). Once you see the edges looking frayed (chips attached still to edge looking like waves) you need to speed up your feed as you have been basically melting the material instead of cutting. Use millable aluminum as the diy-store type will smear even more... Dedicated aluminium bits because the spiral is different and chip extraction is better than with universal bits. Same with plastics .. go fast to keep temp down... if you cannot go faster use less theeth... Steel on the other hand is soo much harder that one takes 4..5 tooth bits in order to keep the chipload down to something the bit can chew without stalling the machine (small bites per cutting edge per rpm) Bits should always have a cutting edge at the tip so we can plunge them (end cutting bits).... Otherwise up and downcut bits are selected as you already found out.. VHS seems to be senitive about cooling (either constant cooling or none at all- just spray ocasional while milling and it will break very fast- doesn`t like changeing tempreratures) HSS semms to be very forgiving in comparison.. Carbide is said to last longer ...who knows? TiAliN? seems to be the coating of the week... i only use them for drilling ops so i cannot comment. Hope that helps a little and sorry for the somewhat arkward esplanation but i am not a native english speaker greets flo
This is some great info guys! I'm a routing virgin so I have no idea what bits to use either. Is there some type of chart out there that shows the best type of bits to use for wood, aluminum, acrylic etc? Keep the comments coming.
I use mostly HSS and cannot complain. one thing to watch for is coatings. the typical yellow TiN coating found on HSS drill bits is not good for aluminum. one of each (-: yes, up cut for aluminum 1 or 2 flute for aluminum. because it is imperitive to clear the chips and not get one stuck and recut it. the smaller the bit, the more important single flute becomes, anything less than 1/8" should be 1 flute. recutting chips = think about what happens if you take a chip, place it on a nice aluminum surface, and take a knife and try to cut the chip in half (and somehow avoid pressign the knoife into the surface . the surface gets dented by the chip! when cutting aluminum it is important to control the heat. as the chips get hotter they start to melt and then start to stick to the tool. that stuck on piece can be hard enough to act as the cutter, but it always rough and the wrong size. to prevent sticking you need a coolant/lubricant. NOT OIL! kerosene works very well, ethanol too, and I use beeswax a lot when cutting aluminum. just rub it on the surface, one the cutter, and into any slots before the next cut. The nice thing about wax is that a high speed bit does not sling it everywhere (-: I added ramping to SketchUcam for precisely this job, to ramp into aluminium with bits that may not be good at plunging straight down. Then it turned out that using ramping on plywood etc is also very good, I use it all the time. And with the right combination of settings and hole sizes, you can generate gcode that has no plunges in it at all. (ramping on and all holes larger than bit size, it will always spiral into the hole without plunging) Most woodworking router bits are not end cutting, the two flutes do not go to the center at the end. But this works in wood because it chips out as the bit plunges. This will not work on aluminum, obviously, so ramping in at 5 to 10 degrees is the answer (angle depends on the bit, start with low angles if unsure, or you can calculate the max angle from a scale drawing of the bit). @Mark Carew will have to answer that (-:
Thanks a lot guys, good information from all of you. I will be ordering some bits right away. One big drawback, it's coming up on Chinese New Year, and the whole **** country shuts down for 1-2 weeks! So, anything ordered out of China will not arrive for 6 weeks or more There are a lot of single flute bits that have an angled flute that covers most of the diameter of the bit. It looks like these should be good for aluminum. They look like they are able to plunge cut, but I will try Ramping as David mentioned. I do need to speed up the feed rate a bit as I was seeing the rough edge cuts that Steve mentioned. As of yet, my router is not variable speed so the only variable I can control is feed rate. Thanks again, guys, as always a veritable cornucopia of information just for the asking...
BTW, anyone know of a good speed control that can handle 1hp universal motor, preferably PWM with a 5v PWM speed control input? I was looking at 180V DC motor controllers, but I would have to convert the Arduino PWM output to 0-5vDC or 0-10VDC to use them...
if you know how fast your router is going you can calculate the feed rate to match that speed. this is important because if you feed too slow the tool rubs instead of cutting, which creates heat and makes it blunt long before time. I have used my woodworking router at 24000 rpm to cut aluminum, works just fine so don't be scared of the speed, going slowly can be very bad. there are many decent feed rate calculators online.
I usually use 1/8th or 3mm cutters for most projects. To be honest I have been testing a lot of different manufacturers lately and want to find one to recommend but most of the ones I have found out there are not very good quality at all and wear down too quick. So I am still looking. I have tried these in the rotation and they seem to work pretty good - Precise Bits The collets I used were from Galaxy Products Hope this helps
Anybody give me some ideas on feed speeds? With the Bosch router, I am guesstimating 20000 RPM. Mine is not variable speed. Feed speed calculators need an exact RPM. Anyone know what the Bosch RPM is? I have cut some pieces in 1/8" aluminum with 100mm/min, 200mm/min. The holes come out perfect, but the outside cut is pretty rough. The 200mm/min was better, but not much. I am using a 1/8" carbide cutter with a single flute. I think part of the problem is getting my Z axis correctly zeroed. The first cut seems way too deep. I am also going to disable ramping in the G-code, it seems to be flakey for some reason. I have the G-Code set for multipass, 0.8mm per pass. The first cut, however, is almost 1.5mm deep. I'm going to get a probe set up so I can properly set the Z axis height. Mark Carew | OpenBuilds, do you guys cut all your plates in house, or do you have them done by a machine shop? They seem too perfect to come out of an Ox or other router...
Well this was a disaster... What the heck am I doing wrong here? I have been slowly ramping up cutting speeds as it was recommended that faster feed speeds result in a cleaner cut. Perhaps I went too fast? Hole speed was 300mm/min, and it totally produced junk holes, with a lot of the aluminum cuttings sticking to the hole sides. Eventually, the bit welded itself to the hole and broke. At 100mm/min, it takes half an hour to cut 6 holes and an outline. This was a brand new bit... ****, I'm going through bits like crap through a goose, I'm going to have to order a bunch more. I wonder if the new bit had something wrong with it? Didn't have this problem yesterday... the one on the left was done yesterday at a feed speed of 200mm/min. The holes were perfect but the edges were pretty rough. Today's holes were way undersized and not round at all. I am going to try reducing the feed speed, turning ramping back on, and reducing the cut depth from 0.8mm to 0.5mm. It's going to take all bloody day to cut one piece...
Hi i `d say you are still too slow. I run 800mm at 20000rpm on a 4mm SINGLE flute bit... two flute would need doubling the feedrate...adjust depth according to your machines stiffness and spindlepower. Use cooling! and avoid recutting chips. I guess your first pass of aprox 1,5 mm depth and slooow feed killed the bit and the rest was simply grinding ... About inside and outside roughness - go counter-clockwise for inside profiles and clockwise for outside profiles: beeing called conventional milling vs. climb milling. On a gantry cnc we do climb milling. google it quite intresting. Lately i switched to tronchiodal milling for aluminum, witch is better for tool-life and more effizient. Less demanding on stability too and thus one can do much deeper cuts at faster overall speed. (just a small vid of my first try.. notice i forgot to go climb milling too , also notice how fast chips fill up in just a few seconds for videoing)
Hey Florian: Yes! that worked much better. I was still to chicken to run it at 800mm/min, I ran it at 500. I also reversed the rotation as you suggested. I am using a 3mm single flute bit. And, I used Methanol as a coolant from a hand spray bottle. I don't want to use an oil based product, because I like to use double sided tape to hold down my work, and oil would prevent it from sticking. And, the shop smells great (Wish I could get Ethanol, that would smell even better. I think the machining quality would suffer, however A quick spray for the work piece, a quick spray for the operator... ) Voila! Much cleaner outside cut, faster, and the bit seems to have survived unscathed. I think you were right, the previous attempt was just the result of a trashed cutter. A bit concerned by the fire hazard, but I do have a pretty good ventilaton exhaust over the machine, and a fire extinguisher handy. There are so many fine points to the art of milling, too bad nobody tells you this stuff right at the beginning... Would save a lot of time. I know you are going to say "the information is all out there", but you've got to know what you are looking for in order to find it. Trial and error is sometimes a lot faster than poring over the Internet for days. The Trochiodal milling looks really cool, I can see how it would allow bigger bites and the bit would stay much cooler. What did you use to generate the G-Code to do that? Anyway, thanks for the input Florian! Happy milling!
Hi, G-code is from ESTL cam wich is great!! Quite cheap too. By now i go much faster but i am regulary in awe still to watch it. 6mm deep trenches from a 3mm bit in one go! For conventional milling or surfacing and for finnishing action i have lately used oil. A good machining oil (like used on sewing machines in the old days -not the mos3 type) gives awsome finish. Much better than WD40 an the like. For milling conventional (cutouts...) i mist using diluted spirit. Don`t like the fire hazard aspect too. greets flo
Fascinating stuff; when things go wrong I'm always trying slower and slower feeds, more and more lubrication/cooling. It's interesting to see your results improving by going faster which seems counter intuitive (and not to mention scary). You're not kidding about going through bits. My worst was trying to mill in aluminium with a 1mm bit. I bought 3 at around £9 each. They arrived in the post at 11:33am and I'd snapped all three by 11:45
Hi, as mentioned best results if bits used by the mfg´s recomendation. It is important to read up and understand at least a little about chipload and feeds and speeds. Always try to match them ... and remember: your bit needs to cut - not grind. The depth of cut is adjusted acording to your gantry´s stability and power of spindle. So going faster using shallow passes hardly anything bad will happen...after a while you will know your machine enough to give an educated guess of how deep per pass will be ok. Live and learn... greets flo edit: older machinist will tell you that milling alumium is going right if you hear a kind of "smacking" sound (chewing open mouthed). The sound of the bit taking bits the right sice. And it is true - it is hard to describe but once you heard it you will know. So listen when milling aluminum.
Metalguru - What is the series of Aluminum you are cutting (6xxx, 5xxx, 3xxx)? 6061 is ideal for cutting, some grades can be VERY sticky by comparison and you may be amazed and how poorly they will machine. I have seen exactly the results as seen in your photos - when using 'sticky' aluminum rather then 6xxx series. Chip extraction and cutter lubrication are also important as you try to go with higher feed rates.
I believe it's 6061, but I'm not sure. I just bought some scrap pieces from a local shop that does cnc punching and and cnc brake work and builds a lot of electrical enclosures, etc. It is clear anodized. It seems to cut well when everything goes well. But it can go to hell fast. I was not using any cooling previously, I had tried using a bees wax formulation made for saw blades, but it just made a mess.
I'm not a big fan of the liquid cooling. Is it possible to just use an air nozzle directed at the cutter? Is this sufficient cooling?
I've been using Tap Magic cutting fluid and it seems to work pretty well. I haven't finished up my ox yet so I can't speak for how well it does in automated systems but just in using the Dewalt router by hand on aluminum it works pretty well. I keep it in a squirt bottle for routing and in a dropper tipped can for drilling. It's not oily and washes up with a bit of dish soap. It's also not flammable.
Seems like the liquid for cooling on a c-beam machine causes all the cuttings to stick together and collect in the cut, rather than letting them blow out. I'm thinking this can't be good for cut quality, having all those cuttings sitting in the slot waiting for the bit to come by and weld them back on...
Thanks for letting me know about ESTLcam - Just downloaded the trial and seeing that $50 to purchase is a great option for home/hobby use.
I hollowed out a block of aluminum 1 3/4" deep and never had a problem. If you keep the chips cool, they don't weld.
Why not use a brush to clean..? For cooling you`d have to be at the machine anyway so why not keep buisy?
aluminum is sticky, and has a low melting point. it likes to partially melt and then stick to the bit, forming a very rough new 'cutting edge'. things go pearshaped after that. the 'cooling' mist serves 2 functions, to keep the temparatures down, and to prevent sticking. cutting lubricant/coolant is an odd beasty. it needs to lubricate to a degree, and then allow cutting. ordinary car oil is absolutely the wrong thing, it lubricates way too well! same with the 3in1 equivalent mentioned, too good a lubricant. WD40 is a water displacer and sucks at pretty much everything else. kerosene is an excellent coolant/lubricant for cutting aluminum, I use it all the time. I also use beeswax (can use candle wax), just rub it on the surface and on the tool between cuts. advantage is that it does not get sprayed everywhere. methanol works very well.... but do ventelate! feed speeds. a lot can be said about this but I will try to keep it to the nitty gritty. a lot of science and testing goes into figuring out how fast to cut stuff. this is all about how different metals interact when one cuts the other, and gives rise to the term 'surface feet per minute' (sfm), ie how fast the cutting edge moves through the workpiece. HSS tools have their speeds, Carbide has higher speeds. A range of speeds it normally given, like 1000 to 2000 sfm for carbide in aluminum. do not use TiN coated tools on aluminum. so, for a rotating tool, sfm lets us calculate the RPM rpm = sfm * pi / diameterInInches so a 1/8" carbide bit should run at 32000 to 64000 RPM in aluminum. (with liquid, not dry!) How much should each tooth cut? Start with 2 to 5 thou. Now we can calculate the feed rate from the rpm and the fz, feed per tooth. So for a 2 flute cutter at 2 thou per tooth feed speed should be 128 (at 32000 rpm) to 256 (64000 rpm) inches per minute. that is 3200 to 6400 mm/min Now, depth of cut. This is flexible, whatever your machine and tool can handle. Obviously a 1/16" bit is not going to handle the pressure that a 1/4" bit can handle. An OX cannot do what a C-beam can do. A Haas VMC with 50 hp spindle can do a lot more depth if needed. So, start small, and test to find out what your machine is happy with. if it is struggling to stay accurate at 1mm deep, then go to 0.5mm . BUT DO NOT CHANGE THE FEED SPEED! and that is the secret to it all. rpm and feed speed are calculated, depth is determined by the machine and tool size. Just to complicate matters I must say this: the speeds above work very well but are really most suited to production environments where time=money etc and the machines use flood or spray cooling. Of course you can cut aluminum at slower speeds, but there is such a thing as TOO SLOW. Slowing down can lead to bigger problems than speeding up! for your entertainment and to give a visual impression of the feed speeds: methanol spray coolant, carbide tools.
way slow! see my other post for the calculations. also, I think some aluminum welded to the bit...... for cutting aluminum from Sketchucam, use the following settings: ramping ON at 3 to 7 degrees (just numbers I have seen for various tools) plunge holes in 'diameter first' mode.(2) multipass on at about 0.5mm per pass as a starting point stepover% = 30% kero or wax coolant/lubricant and, if you are making holes that are 'bit diameter' in size, do a separate drawing for those holes and use a real drill bit for that, then switch to the milling bit for the rest. with the above settings, and holes that are larger than the bit, Sketchucam Gcode will NEVER plunge directly into the work(1). Milling bits are really bad at this so try to avoid it. (1) 'never' is may a too strong term here, if you have small features with line segments shorter than 1/2 bit diameter then it might plunge because there is no space to ramp. though the cut start optimizer will look for a long enough segment to start on, if it fails it will plunge. a comment will be placed in the gcode to warn you of this. Example, 3.5mm hole, inside cut with 3mm bit, ramping on Code: G00 Z0.200 G01 Z-6.300 F1000 (ramplimitarc end, translated to plunge) G02 X10.153 Y7.2489 R2.0 F2000 G02 X10.0853 Y7.7632 R2.0 but, do that hole as a plunge hole and it will be a pure helical spiral, one cut if stepover% is > 50, 2 cuts if stepover% < 50. (2) diameter first does more side milling than helical boring. it helical bores the center of the hole, then spirals out to diameter for each multipass depth. in contrast depth first bores the center, then helical bores each stepover% down to depth. Use the Tools|Phlatboys|Options|Hole Features menu to change this setting (and read the help!) try them both and see what they do, then stick to diam first in aluminum (-:
I calculate 1000 to 2000 mm/min feed speed for a single flute at 20000rpm. flaky? what is flaky about it? prove there is a problem and I will fix it (-: with small bits and small passes in aluminum, setting z-zero correctly is critical. google for the 'cigarette paper method'.
I do hope they were single flute! anything smaller than 3mm should be single flute, it provides space for the chips to get out, which is critical. and paint on some kerosene, cooling is vital.
That's been one of the things I've found most difficult to understand with this hobby. I spent a lot of time on forums reading about feeds/speeds and got so much contradicting information I didn't really know where to start. I've since realised that each of us develops our own rules based on our experience, what we're actually making and the machine we've built. For example my workhorse bit for cutting aluminium when all else fails is a general purpose 2mm 2 flute bit (YG-1 E5424020) which violates your 1 flute under 3mm rule. I've broken pretty much my initial stock of every other bit (learning a great deal along the way of course!) but the three of those I bought are still going strong and seem to cut aluminium, mdf, wood and acrylic with impunity. My results changed dramatically when I gave up on dry cutting, but again, maybe that's just me I started with WD40 but am now on to water soluble oil through an automated mister, simply as it's cheaper and easier to clean up.
Simple (quite common) misunderstanding: The requirements of the milling bit do not change! It is build for a certain purpose - not to be changed by your desires.. It needs to cut at a certain feedreate in order to cut (chew if you like) a certain amout ot material for a good lasting. too much it snapps and too little it grinds and heats up and snapps too.... Try to match all parameters as closely as possible and than!! go as deep as stability of your cnc or spindle power will allow. (only this parameters really depend on your specific setup) So shallow passes are never to be a problem ... only consume time... ok they might wear tip more than needet... Cooling: anything better than none. dilluted spirits (that stuff that smells funny) works best for me for trenches cutouts , profiles... etc. For surface milling thoough oil ( a good old machining oil - no motoroil no mos3 type either) works fanstastic- have a look here (sorry i am on a buisness tripp so cannot access my pics at home , yt-link will have to do): greets flo
