I build a C-Beam last year. It's stock with a Dewalt DWP611 router. I use Scetchup and ScetchUCam. Haven't done a lot with it but have cut plexiglass, balsa and plywood. Time to move to aluminum sheet which is what I really wanted it for. I want to be able to cut 3003H14 .032 sheet. Assume if I can cut that I can cut thinner and cut thicker in multiple passes. My first attempt was .32 2024 T3. Yes I know this is harder than 3003H14. I used a 2 flute chip breaker carbide 1/16 bit w/fish tail from Drill Bits Unlimited. My router is turning (I think) 15000 rpm and that is what SchetUCam is set at. I used a feet rate of 8 13/32" and a plunge rate of 100". The cut was basically dry though I was spraying water on the bit with a spray bottle. It was a miserable first attempt. Plunged about 9 holes and cut one ruff slot then broke the bit on the second slot. I'm using a 1/16" bit because the some of the holes need to be .098" and will be finished drilled by hand with a #40 so a smaller pilot hole is plunge cut. So how can I make this work? What bits? Please don't send me to a bit site and say I can find bits here. I'd like more specific recommendations like a certain bit available at this site has worked for me for a similar work. What feed and plunge rate? I've attached the parts I'm trying to cut. They will be assembled together to make a cowl baffle for a Cessna 170. Thanks for helping. Bruce
An update: I found the C-Beam plate cut example and looked at the settings use to cut it in ScetchUCam. Figured if it would work for that it should be close or work for my aluminum sheet. The .032 sheet was carpet taped to some foam core board then that board carpet taped to my spoil board. I did this to give the sheet some thickness so my bit wouldn't be cutting into the spoil board. Using an used 1/8 single flute carbide bit I cut three parts. The tool I used in in the picture. First to the left was cut using the C-Beam plate settings of 27" feed and 9" plunge. I used some vegetable oil (I didn't have and canola) as was done to cut the C-Beam plate. As you can see, not a good cut but the bit didn't break. Thinking I needed more speed I cut the middle part at 40" feed rate all other settings the same accept I added tabs for some dumb reason. Also for the middle cut I set the 0,0,0 point a bit high and it did not cut all the way through. I stopped the cut, reset the 0,0,0 down on the material and restarted the cut from the beginning. This is cut is still to ruff. Last I thought maybe a fresh new bit and more speed. So the right part (part had been pulled) I put in a fresh bit and cut at 60" feed. The last was only slightly better than the first two. You can still see how ruff the cut was on the outside, the part on the inside as equally as ruff. Looking for suggestions. Do I have the right tool? Am I feeding to fast or to slow? Thanks Bruce
Actually looking at the part on the right, it does not look bad on the right side of the cut. The part however looked like the left side of the cut which is ruff. Thanks for any helpful suggestions. Bruce
I've had pretty decent cuts with Kyocera endmills and Desteniytools. The 1/8" i use are these: (10) 1/8" (.1250") 2 FLUTE CARBIDE ENDMILLS - NEW - 1600.1250.500 | eBay I use abaut 700mm/min(27.5591 in/min) feedrate at 19000rpm 1/4" is thisone: 1/4" carbide coated 3 flute endmills for aluminum milling - long flute - V31620S | eBay This 1/4" makes for excelent surface finish and i use 785 mm/min(30.9055 in/min) feedrate at 19000 rpm only downside its long flutes which couse high deflection but i havent found shorter version then this. Unfortinetly i see a lot of deflection in the plate maker i have with the wheels .i will either add more or go for linear rails instead.
Thank Darathy, just what I was looking for. Do you know what kind of aluminum your cutting. 20XX, 30XX, 50XX, or 60XX and might yo know the hardness? Yes I see flex and plenty of room for improvement in th C-Beam and of course there has been plenty of improvement by many in the machine. There is only so much time and so many projects. I reentered the hobby of RC model flying after 25 years absence. This was the unexpected drain on my time this past year. And of course when I did start the router it was to try to use it to make RC plane parts out of balsa and plastic, not real airplane parts out of aluminum.
That is 6082 6082 aluminium alloy - Wikipedia. And i forgot to mention i take 0.2mm depth of cut dont think the flex and the dewalt 611 can take more than that.
More info. Apparently I'm not cutting at 15000 rpm but 27000 or close to it. This is the top speed of the DWP611. According to the Shpeoko site I found some have found their routers 6 speed settings to be 16200, 17700, 19450, 21100, 23500 and 26900. All routers are slightly different but I think this is close enough for me for now. So in addition to feed speeds and plunge speeds, what rpm have you guys had success with specific bits. I am aware of the feed formula found at www.hsmworks.com/docs/cncbook/en/#Ch03_CuttingSpeedsAndFeedsFormulas. I'm trying to figure out which of these formulas would be appropriate. The pure milling speed/feed formula is quite can be quite a bit different that the one which considers spindle speed. Assuming a single flute carbide bit is appropriate for aluminum here are the feeds for the bit I tried using HSMWorks formulas.: Tool Dia 0.125 in Mill Speed 24448 (rev/min) Num Flutes 1 Drill Speed 9168 (rev/min) IPR(CL) 0.002 in Mill SFM 800 ft/min Mill Speed/Feed 49 (in/min) Drill SFM 300 ft/min Max Spindle Speed/Feed 54 (in/min) Max RPM 27000 rpm Drill Speed/Feed 18.3 (in/min) If this is a good formula and my results weren't so good I can only conclude a single flute bit is not appropriate. Also in this case there is not much difference when you consider max spindle speed. In the following example I've changed the bit to .25 and 2 flute to show how the formula starts to show a big difference when you consider spindle speed. 49 vs 108 in/min. Which should I use in this example? Tool Dia 0.25 in Mill Speed 12224 (rev/min) Num Flutes 2 Drill Speed 4584 (rev/min) IPR(CL) 0.002 in Mill SFM 800 ft/min Mill Speed/Feed 49 (in/min) Drill SFM 300 ft/min Max Spindle Speed/Feed 108 (in/min) Max RPM 27000 rpm Drill Speed/Feed 18.3 (in/min) Thanks again for any help and exact examples of bit/spindle sp./feed rate vs material Bruce
For cutting aluminum you MUST turn on ramping in SketchUcam. I wrote it for aluminum, just for the C-beam (-: Milling bits do not like to plunge (even end cutting ones), so ramping in is the best thing to do. If you have ramping on, then do not drill any holes the same size as the bit . Either make sure all holes with be spiral bored by making sure they are larger than the bit, or separate your drawing into 'all the drilled holes' ie the ones the same size as the bit, and 'everything else'. Then make 2 Gcode files, one for drilling, one for milling. Even in ramping mode, holes the same size as the bit will be plunged. Rather use an actual drill bit for those holes. (a stubby bit is best, so the tip does not wander off center) Drill all the holes first, then run the mill code with the milling bit. This is safest, just in case you forgot a hole and it tries to use the mill bit to plunge it, the hole already exists, Use the calculated feeds! Use kerosene to lubricate the cut. Clear the chips! Adjust depth of cut to suite the stuffness of the C-beam. Mark uses 0.5mm layers (0.020 inch). RPM and feed speed is critical for getting a good cut. Depth of cut is adjusted to suite the machine stiffness. Your surface finish results from 3 things: flexibility and cut direction and chip clearance. How long is your bit? Shorter is better. How far down does the Z axis come? less is better. pack up the workpiece on MDF so Z does not have to come down much at all. This is stiffer. Try unticking 'overhead gantry' in the SketchUcam parameters dialog. Your outside cut will then cut in the opposite direction. Clearing chips: it is essential to clear the chips , vacuum all the time, or at least between passes. Recutting a chip is fatal to surface finish. Think about it this way. If you take a chip and put it on the surface of the aluminum plate and take a craft knife and cut it in half, the pressure of the blade will make the chip dent the surface before it cuts the chip. right? That is exactly what recutting chips does. You can also try doing a finishing pass. Make a copy of the drawing. on copy A remove the outside line. set the bit diameter to 5 thou larger than the actual bit add the outside cut line. set multipass on, ramping on, and so on, as normal. generate Gcode. on the copy B, remove the cutline, set the bit size to actual bit size set multipass OFF, ramping ON generate Gcode. (obviously this file does not need the holes in it) you can now join the 2 files using the joiner, A then B. A will cut the shape 5 thou too big, then B will come and cut 5 thou smaller in one pass to smooth out the surface. You can also try doing the rough and then finish cuts in different directions, just tick/untick 'overhead gantry' as needed.
David, thank you for the tips. I have a friend who use to cut a lot of aluminum sheet on a big industrial router stop by. He say's I'm probably not using the best bit. I'm also trying to cut softer aluminum which he points out is harder. My method of holding down the sheet needs improvement. I'm using carpet tape which holds chips in the or about the cut. Anyone have a better method to hold a thin plate to sacrificial MDF. I've rediscovered ramping in. As I'm only cutting a sheet .030 thick, I'm cutting it in one pass not multi pass. I've figured out I will have to do the drilling in a different gcode run and swap bits to the smaller bit for the pilot holes than the bit used to cut out the part. Your guidance confirms all this. I would have never thought of a rough cut by over sizing the bit size a few thousand then doing a finish cut at actual size. Great tip. Here is a question though so I understand this. When an cut along a path is created does it consider the tool diameter at the time it's created? For example I create all rough cuts with the bit over size that I want oversize and then those that I don't the bit sized correctly. Then the gcode is created with the paths of each size tool bit. Or are all tool paths created fresh with the tool bit size at the time the gcode is written? In other words it doesn't matter the size of the bit while I'm creating the tool paths because the bit size is applied to all paths when gcode is created. When I join two gcodes using the joiner does it move from one path to the next without stopping of does it stop to allow a tool change inbetween? I'm thinking I could only use this when the tool is not changed between gcode. I'd have to load two different gcodes, one to run the drill holes. Stop and change bits. Then load and run the rough cut joined to the finish cut. Last when you say use the calculated feeds, would you use the calculation that takes spindle RPM into consideration? When drilling holes using an actual drill bit rather than a router bit, is there a special plunge calculation to use for this? I'd think the drill bit would need a slower plunge rate than a router bit. This doesn't have to do with cutting aluminum. I noticed my machine might be cutting a bit undersize. I cut a test piece .75 x.75. What it cut was about .002 under that. What are the tolerances I can expect? Where do I go to make the adjustment, if one is possible, to correct for that .002 shortfall which seems to be in both X and Y and maybe even Z? Thanks Bruce
Using the kerosene is then more important as it prevents the chips sticking to the bit. why yes.... Holding parts on the CNC router For outside/inside cutines, the bit size is used when you add the lines, the Gcode then just follows the lines. For plunge holes, the bit size is used when Gcode is generated once you have created a cutline it stays exactly as it is until YOU erase and replace it. There will be no stop between the files UNLESS you include a toolchange instruction. Read the help about the quicktools toolbar and the tool change options. However, GRBL does not support toolchange, but some GUI's for it do. Still easier to run 2 files for 2 tools IMHO. But for roughing then final cut, joined files are perfect. Yes. You have to. The calculation goes like this: find SFM for the material you are cutting (for the bit type, HSS or Carbide) find RPM from the SFM and the diameter. find feedrate from RPM and flute count and cut per tooth. Calculate it from the RPM. But use a low cut per tooth, say 0.001", maybe more or less. Note that the drill operation will peck drill if you turn on multipass. There is also an option for quickpeck where it does not do a full retract. This needs testing since the purpose of the peck is to clear chips. Read the help on setting hole feature options to find out how to change this. Big blue question mark in the toolbar. There is a resource for calibrating: HOWTO Calibrate your CNC Machine for MACH3 or GRBL but don't forget that the bit size is 'nominal', ie it is labelled 1/8" but may be 0.126", nothing is perfect. You cannot expect any cut to be closer than one 'step/mm' away from the desired size. So if you are running 8x8 leadscrew, 200 step motor at 8x microstepping, that is 200 steps/mm or 0.005mm per step. In other words, you cannot get closer than a multiple of the step size.
To setup and dial in your machine also be sure to use this handy Calculator Resource Especially below Fine tune and dial your machine in using the very handy - Axis Calibration Tool
Thank you Mark and David for the resources. There was a time when I'd remember thousands of details of all sorts of operations. As I've aged, like my iPhone5, 16m, I think my brain can only handle so much stuff at once. I need to rely on just remembering where the resources are to access. David, I'd been looking at the HMSWorks page formulas. In their examples they have an example where the calculated RPM exceeds the spindle rpm capabilities. On review, I was misreading this. Basically and simply their formulas says when this happens just use the max rpm your spindle can produce to get a feed rate. DUH. Misreading was the source of my question. My DW611 router rpm range is 16000-27000. Using a 1/16", 2 flute bit with a sfm of 800ft min for aluminum and an IPR of .002 the calculated RPM of the spindle should be 48508 and at that rpm a feed rate of 194 in/min. So I set the router to 27000 and recalculate the feed using 27000 and get 108 in/min feed rate. Is this right? Is this a compromise yielding the best cut possible but not idle? When kero is mentioned as a cutting oil I wonder, would Jet A work as well. As a pilot I have access to gallons of free sump Jet A. Jet A is kero but does not have the same lubricating value and requires additional lubricant to be added when burnt in an diesel engine but operating it in a diesel and using it for a cutting fluid are two different things. Anyone every use Jet-A as a cutting fluid on aluminum? I'll have to report back after trying it. Thanks Bruce
Remember, cutting fluid is intended to be a coolant not a lubricant. As long as you're getting good evaporation/cooling and not pushing the flash point you should be fine.
The kero mentioned is used for its lubricating nature. I do not think that jetA contains lube. In general one uses it only for either surface ops or the last finishing pass as Aluminum rarely needs cooling. Use WD40 or the like if you can not find kero at home. For good results get a dedicated aluminum bit like this: Sorotec - END Mill They have a special dedicated aluminum cutting and evacuating geometry as well as polished channel-surfaces for clean cuts. Much more fun than using something that sorta works... Always tightly clamp down your work-piece. Vibration is bad for surface and for your mill-bit. Aluminum needs high feed-rates the bit needs something to chew .. try not to pulverise the aluminum. If right you will hear a sot of "smacking" sound. Adjust depth of cut to your machines cababilyties. Read up about climb- and conventional milling to get better surface and tool lasting, I cannot explain that as i am not a native english speaker. There is a nice vid on y-t by a guy neo7cnc which does not explain but at least nicely shows the difference. I quite remember it is called something like better results in aluminum ... there it is: always use climb cut on a gantry router Use the right kind of aluminum. Cheap aluminum for home-improvement stores usually contains too much lead so they will smear and kills your bit. greets flo
Thanks Flo, as you suspect Jet A does not have the lubricating properties of kero yet it will cool as Rick points out. I'm not worried Jet-A will flash and worse than kero as far as that is concerned. I guess I'll just have to try it. Appreciate the pointer to a good bit and the video. I do understand the difference between climb and conventional milling as I've a few hours experience operating a Brigdeport mill. However as the router is turning so fast and I'm not holding the router, I must admit I've thought little about it. My first attempts at cutting sheet did not show evidence climb or conventional would have made a difference. Agreed all aluminum is not created equal. However I was not trying to cut cheap aluminum, it was 2024 T3, Alcoa. However that does not mean 2024 T3 is the appropriate sheet to be trying to cut nicely with a router.
Hi, your pics clearly show ridges around the cuts indicating the following either your bit is not sharp enough (guess it is new though) or aluminum is to soft/ containing a lot lead also it looks like the chips produced being more of the dust variety... get in more feed forget about the JetA - cooling simply isnt necessary with aluminum. Getting the chips out of the channel if going multiple passes is important though. WD40 isnt going to break your bank and you`d need it only on surfaces or a finishing pass. I was not talking about the price of your aluminum.. there are specific aluminums for bending, coating, soldering, milling or even withstanding salt water ,,... - all of them expensive and not avialible in your DIY store. So try getting something like: AlMG4,5Mn0,7 or even better AlSi1 MnMg
Thanks Flo. We both have the same thoughts on aluminum, we are just not understanding each other. I'm a pilot and aircraft mechanic. I understand differences between aluminum alloy and hardness of each. You are right the picture is of unknown alloy but my unpictured attempts where cutting 2024 T3 Alcoa .020" sheet and that didn't go any better showing the same result. Wrong bit, wrong speed, lack of coolant/lubricant and bad hold down method and attempting to cut aluminum, perhaps even the 2024 sheet, that will not cut well. WD40 will not break my bank. However it is over used by many (not necessarily those commenting here) as a lubricant, a purpose it was not designed. It may be the perfect, or at least very suitable fluid for this purpose and I have taken note of it's suggested use here and other forums for cutting aluminum. Just when I here "spray it with WD40", 9 times out of 10, it's not the best solution. I'll spray my next attempts next week when I get new bits and more aluminum with WD40, Kero and JetA and see what the difference if any appears to be. Ultimately, I'd like to be able to cut out small aircraft parts for my own use such as the winterization cover plate I posted on my first post. Not necessarily this project, but many need to be cut from softer aluminum such as 3003H0 or H14 which is commonly used in aircraft skin construction and can be bent. I'm learning I may never get the cut I'd like to see right off the machine but thanks to everyones help maybe I'll figure out how to get close enough that a little file work to finish it is all thats necessary. Thanks Bruce
Hi, yes it is difficult comunicating in writing only... Well, the term "use wd40" is used widely around here to indicate using some/ any-kind of lubricant of the oily sort. I a actually really like to use my "degript oil" an old bottle of so called sewing machine oil. It is all soft to the touch but still sort of thick ( think a rich olive oil). It gives spectacular results in aluminum. I merely tried to point out the fact that a lubricant makes more sense than a coolant on aluminum... if you get the heat into the chips and the chips out of the cutting channel that is. greets flo
Guys, thanks to your help I was able to cut a sheet of .032 aluminum of unknown quality, good enough to clean up with a file and create a Cessna winterization plate. Flo, I used WD40 for the lubricant. I held the sheet down to a MDF backer using the tape and CA glue method shown in the video and I held the MFD backer to my router table with the same tape and CA method. I used a fresh bit I had on hand. Ramped in and used a rough cut, finish cut method. About the only thing I did contrary to advise was I ran my feed rate about 1/3 the speed (20 in/min) than the 50 in/min dictated by the calculations. I did this because I buddy who ran a router table professionally cutting tons of aluminum sheet and block, said I was feeding way to fast. When the bit hit the sheet the first cut at 50 in/min he dove for cover. No progress pictures but below is the finished part. Thanks Bruce
ahem, cough, 50"/min is slow (-: search youtube for 'datron cnc'. Yes, big stiff machine, but that is how fast you can cut aluminum if you use sprayed ethanol for cooling. (and if you spray ethanol make sure you use an explosion proof vacuum to vent outside Saying aluminum does not need cutting fluid is not correct. Some alloys don't, the high magnesium ones tend to cut cleanly, but most do need coolant/lubricant because the aluminum is prone to sticking to the bit. I often get that on my lathe, it welds onto the tip of the tool and then the cut is actually done by the welded aluminum chip and gets very rough (and the wrong size too). For some lighter cuts I rub on some beeswax, for heavier cuts I use kero which works better, even when the heat of 3mm deep the cut is making the kero smoke (-: Note that this is at only 600rpm, how much more heat can a 20000rpm router produce?
David, I understand what your saying about 50"/min. All the advise here and elsewhere says most people don't cut aluminum fast enough and I'm not totally surprised with my friends first hand reaction. But as he professionally cut aluminum sheet on a 12" x 16" cnc router every day for over 5 years for one of the USAs largest sign making companies, it's hard not to follow his advise while he's standing there. Remember we don't know what kind of aluminum we were trying to cut. However, once I successfully cut this aluminum faster while he's not watching, as we have been close friends for over 38 years, I'll be sure to tell him he doesn't know what he's talking about. Be a few days till I can get to it but the next cuts I make I'll compare WD40, Kero and Jet-A as lubricant/coolant and report back. Thanks all. Bruce
