Printable View
So I have a Tormach 440 with Power Draw Bar. I have been teaching my self how to use the machine and have been finding recipes that seem to work. One that I have been using for drilling #37-39 holes in aluminum was 6 IPM at 10000 RPM. This was cutting through like butter up until today where I broke 3 bits. I have not changed anything that I know of and the drilling operation is pretty similar. Anyone know some common things that could cause this sudden change?
Thank you in advance
What kind of drills are you using? What kind of coolant are you you using? Are you peck drilling or drilling straight through? Are you using a G81 or a G83 drill cycle? How thick is your material? What kind of material? Aluminum, what alloy?
Titanium coated bits (ones that came with the mill, these worked fine before), flood coolant, tried both before was was doing straight and it worked fine, not sure what G81/G86 is use fusion360 for CAM, material is 18mm, aluminum 6061 if I recall (Sam material as before no issue)Quote:
Originally Posted by Steve Seebold
This is what's weird no factors have changed except for time I even tried new bits because I thought maybe they were dull. I had to drop the IPM down to less then 1 to stop breakage...
Milling is fine no issues there my only problem is drilling, I will say that I have had issue with drilling holes bigger then 5/16" before and still do I can not seem to find a recipe that works well
What size holes are you drilling? Can you post the line of code that has the drill command in it? I hate to say it but just because Tormach sells it doesn't necissarily make it the right tool for your application.Quote:
Originally Posted by FidgetThings
Chip welding? At 10K, 6 ipm is a fairly low feed (GWiz says 18 at 8K in 6061). Flood should help prevent welding, but if you're rubbing you'll destroy an edge fast.
Look at your code to determine what drill cycle you are using. G81 or G83 are g-codes.
I'd probably try slowing down the spindle, stick with 6 ipm feed and flood, and resharpen or replace the drill bit. Remember you can get bad grinds out of the box, too, so use a quality drill (PTD, Onsrud, something better than Home Depot quality).
Never used tormach drills, but I've found 250 sfm is about my limit with crappy drills. Otherwise, I get edge buildup and it's all over when that happens.Quote:
Originally Posted by FidgetThings
My $.02 on drilling 6061.
1) Set your RPM equal to 200 surface feet per minute (SFM). RPM=200*12/(tool dia*Pi) = 200*12/(.104*3.1415) = 9182
2) Calculate the feed per spindle revolution. I use .020 per 1.000" tool dia. per revolution. (.104/1.000)*.020=.0021/rev. Feed = 9182*.0021 = 19.3in/min
3) Use flood coolant for anything deeper than 3 diameters.
4) Use peck drilling (G73) for holes 3-5 dia. deep. Use deep hole drilling (G83) for holes greater than 5 dia deep.
I would useQuote:
Originally Posted by IMT
S5000M3
G83G99X?Y?Z-?Q.1R.1F10.
Fill in your X and Y coordinates and your Z depth. I would use a parabolic flute drill and if you're using jobber length drills you'll need to either spot drill or center drill your holes.
I know this works because I make some model boat parts that I have to drill a .100 diameter hole 4 inches deep in a piece of 3/16 thick 7075 aluminum 3/32 from one edge and I have never had a drill break out the side of the part.