I am the head coach for a high school robotics team. We have been using a CNC router for several years with varying levels of success. Last night we were cutting 0.190" 6061 aluminum plate without any problems. We are using a 4mm, single flute, carbide bit, V carve, and Mach 3 software. The router is running at 21,000 rpm, in a single pass, at roughly 50 ipm, and we were flooding it with coolant.... no problem. We then switched to .25" 6061 aluminum plate started having chip weld/pile up. This isn't the first time we cut .25" aluminum 6061 plate. Just the first time we have ended up with this problem We tried varying feed rate (all the way up to 80 ipm) and the number of passes (1 pass to 4 passes). With the attempt at 4 passes, it was on the 3rd pass when we went back to having problems. We decided that it might be the plate, so we switched to another .25" 6061 plate and are having the same problem with it. So we switched back to the .190" plate we were cutting and are now having the same problem with it. We have gone to Vcarve and regenerated the g-code. Same problem. As of right now we are 10 bits into this issue.
With our competition quickly approaching, I am needing help figuring this out so we can keep focused on our deadlines and our goals.
Is your gantry properly secured? Slow your sfpm or spindle speed to keep the cutter from heating up too much. Make sure coolant is properly reaching the mill or try without coolant in a new set up. Make sure your bits are sharp as aluminum isn't a fan of dull cutters. Try some of this and good luck!
chip load = Feed/(RPMxN) N is number of edges The tables attached say a CL of around 0.05 to 0.1mm is OK and your at 0.06mm so I expect your cutting settings are good. Check your edges have no build up on them and soak in caustic to remove stuck aluminium. Tools need to be sharp and clean. You can get tools with more angle on them for Al. Is the machine vibrating more than usual? Careful with plunging don't plunge use a ramp to introduce cutter to job. Re-cutting swarf is a big no no. Even with flooding the groove may still have swarf in it that's being recut that you can't see (I'm guessing the flood is the issue) . (you can hear the recut if you listen, if feed is correct then you get a steady stream of chips flying out of the tool, use slow motion phone camera to observe cut) Use an air nozzle at the tool to keep the chips away from being recut. This is messy but best. A mister and high flow air is sometimes better then flood. Good luck Peter
edit - Now Guhring have different ideas. They say 0.02 to 0.04mm Fz - say 0.03mm so this means at 21000rpm the feed should be 630mm/min. Maybe try slowing down feed? Guhring also have this Fz at one diameter deep. So the 4mm cutter would be 4mm down. Maybe DOC at 2.5mm is OK. I think DOC does not matter its chip clearing, sharp tool, and minimal lub... surface speed at 21000rpm is 263m/min which is close to Guhring 300m/min so thats OK
Last edited by peteeng; 01-20-2023 at 08:52 PM.
Reason: adition
Chip welding in aluminum is something that all of us have struggled with from time to time.
Sounds like something changed and you have to hunt that down.
1) Number one on my list is the raw material. Sometimes a batch comes in and it's a gummy nightmare. But you are still having the issue when you switched back to the original material.
2) Are your end mills all from the same batch. I'm not sure if you are using name brand or a random pack from ebay. Could be you went through your good cutters and are into a bad batch. I'm guilty of going cheap on cutters and I've seen the grind quality is all over the place.
3) Coatings, you should be using a bright polished endmill or something AL appropriate like ZrN. I've seen some single flute cutters from china that are TIN coated and they gall instantly. +1 for the single flute. Most of the time when I hear people having problems in AL it starts with a 4fl cutter.
4) Coolant strategy. Flood worked ok but on my machine mist with heavy air pressure was much better. My flood coolant was low pressure and a big clump of chips would act like a dam and keep the heat in one place. Air blast fixed that for me.
5) The geometry that you are trying to cut could cause a problem. This one bit me a couple of times. Aluminum is very thermally conductive so cutting parameters that work fine in a straight slot or profile could become a problem. Dwell in one area and get get localized heating. i.e. that U shape in your cut. Or it could be that the mill can't keep up and since it's slowing down in the U it spends more dwell time there and increases the heat, then instant galling. Also, thin sheet doesn't transfer heat as quickly as thicker plate will. Your total conductivity goes up. Deep hole drilling is another time when this bites me. On the first 1D peck the metal is cold, then on the next peck it's warm, then on peck #3 it's twice as hot.
6) Check the machine to see if anything is loose or damaged. After crashing 10 bits, you might have leadscrew or spindle mount that is loosed and your getting instant chatter. Probably not the issue, but it's worth checking once you've eliminated the other possibilities. It would explain why going back to your original cuts on 0.190 plate is a problem all of a sudden.
7) At this point we are really in the weeds you might want to make sure you are using the original known good gcode. Something like a CAD/CAM patch might have changed things. I've seen this happen when a Fusion360 update brings in an updated post processor. If an older file works fine then you know the machine and material are ok.
Does anybody use WD-40 to prevent galling chips on the cutter?
why single flute? High helix angle to eject the chip,
slow the feed down until the chips evacuate themselves.
Don't "crowd the chip" >>>> Old machinist saying.....
Hi Bostosh - Most people without flood cooling start with WD-40 as its on the shelf behind them. Its effectively kerosene. The contact pressures of cutting require quite a heavier lub to stop the surfaces contacting. It does evaporate so helps keep the temp low. If your chip thickness/feed is incorrect and there's lots of rubbing occurring then pick-up and galling are inevitable. Once you are making good chips your still not out of the woods because aluminium chips are quite plastic and are not as work hardened as steel chips so if they are still in the slot and get recut then they smear and adhere to the tool surface. This then builds up and at some point, the tool is seriously blunt and galled, welded or broken....Peter
re - why 1F bit? Because with routers the spindle speed is very fast so to get the correct chip thickness and chip clearing this helps. So just slowing the feed down may not be enough to help with a 2F or 3F bit.. Then there is machine rigidity to consider. Routers are not mills so if the tool/machine deflects and the tool rubs then your going down the galling garden path again....
You did not share your doc but my guess it is too much, also very much dependent of spindle horse power. Single flutes of a quality brand usually cut aluminum pretty well. Two flutes also work pretty well. Bet your cut are noisy that is the machine telling you you have something wrong. Much plate is not 6061, if it is printed on the plate with manufacture your material is probably good
CNC Router Chip Weld/Pile Up
Reply with Quote
