ok, I might stick with the 2 flute .0625" cutter and run the holes via fusion 360s boring set up. I was ramping to .019" doc and pocketing the hole when I broke the cutter. But what you are saying is the smooth consistent helical bore is easier on the cutter?
Problem #1 is that that’s almost twice the doc you should be taking on that small endmill. I mean that’s almost 33% width, pretty heavy when you factor in things like total indicated runnout.
Imo set chipload to 1 thou, start height a little above top, in passes adjust pitch and you can even start smaller then work up, lead to center
3 Likes
ok thanks for the insight. I will give this a shot and see how it goes. Tough part with this set up is I have about 200 of these holes to drill per setup and I want to reduce cycle time as much as possible since I will have to run alot of them.
$40 for 10 pack of carbide drills
edit those might not be great for aluminum but they state they offer others, send them a message
1 Like
so if you could find a carbide drill like this you would opt to peck drill the holes vs. helical bore with a 1/16" cutter?
Do you have a plan C? Peck Drilling with a properly coated drill and a high pressure air/oil blast. There is no room for the chips and no strength for re-cutting them. Still probably the best option. Helical second. Just my opinion.
2 Likes
For an accurate hole the drill would probably be better but I haven’t run a drill yet. The endmill would probably need multiple passes and dialing in.
Airblast on both, doesn’t have to be crazy strong. The routers blow a decent amount on their own
1 Like
My plan c would be to drill them on a drill press with a traditional drill and a fixture. I would prefer to just do a tool change on my CNC and have it cut all the holes for me accurately.
I think Ill look into some drill endmills and give that a shot. If that doesnt work out I will go the helical bore route with the 1/6" cutter.
Even if you spot drill/mill them for a second op (drill) outside of the machine would be great. At least you’ll have them on center per the program/part.
ya that might be my plan C with plan D being the fixture drilling. That way you could drill down only like 1/4 or 1/2 the depth of the part and finish it up on the drill press.
Really curious how this worked out.
still setting up the project and waiting for the order to come through. I will keep everyone posted on how I handle it. Each setup will have 224 5/64" holes. Should be interesting.
Been a while and am wondering how this worked out. Now I have a few, maybe eight holes to drill like this. Were you able to come up with a working solution?
2,232 holes later the first batch went well! Almost ready to start on the next batch.
I ended up using a HARVEY TOOL 46505 5/64" X 90 DEG CARBIDE DRILL MILL
I peck drilled the holes at 18000 RPM, and a pecking depth of .030" with a plunge of 20ipm.
The biggest thing that i found that helped was to make sure there was plenty of lubricant on the cutter and the hole while drilling. The mister alone didnt seem to always work and things would get gummed up.
Picture to show results.
7 Likes
Wow, how many drills did you go through for that many holes?
still on my first one!
1 Like
thats awesome! great work. impressive you didn’t lose one.
i’d look into a loupe or microscope to check in on the quality of the tool.
ya visually it looks to be in decent shape still. Some aluminum build up, but nothing that cant be cleaned. To save some time i might only drill part way through on the next set and then finish drilling on a drill press, I havent decided yet.
1 Like
That’s crazy impressive!
Thanks for the update. It will help my next project.