aluminum nightmare

[twelchPTM]

I am trying to cut plates for mounting casters to a cart with. Simple triangles with 4 holes. I am using a .25" up-cut endmill from Harvey Tools. Pulled the feeds and speeds right from their web page. I know those are just a guide or starting point so i played around with them as much as I could. Problem is instead of throwing chips it is creating globs in the flute of my tool, even broke the tips off two of them. what am I doing wrong? any suggestions?

[twelchPTM]

also for the holes, If I have a center cutting endmill can I peck drill the holes? I bet you tell me no but the question is why?

[carlcnc]

Thomas
first what type of aluminum? 5052 it sounds like
here is what I would do;
milling, 2 flute at 12000 rpm,really light passes of no more than .040
at about 50 ipm[.8sec] still you need to squirt a bit of wd-40 ,spar-n-wash[really] about every 10-15 sec. helps a lot

for peck drilling,I would do .03 per peck at 10 ipm,[.16 sec]

good luck
Carl

[twelchPTM]

thanks carl. my feed and speed all seem to fall into the median here on the forums. I think it was the pecks that messed me (and my bits) up. I realize that one should use drill bits for drilling aplications but I for some reason am really anal about cutting my spoilboard (i know its called a spoilboard for a reason) and figured with the end mill I could go just deep enough to not fudge up my board. Lesson learned - a few little divots ion the spoilboard is better then 3 spanked bits

[Brady Watson]

You want a 3/16" single spiral O-flute tool to Inside Profile cut 1/4" holes. You MUST choose a spiral ramp on the profile toolpath options ramp tab. You can use the 2-flute from Harvey, but you'll want a smaller diameter. The 3/16 should be plenty beefy to profile cut the outside.

The problem you are having is from plunging straight down. You NEVER plunge straight down into AL or you will permanently weld AL to the bottom of the tool.

-B

[twelchPTM]

I did chose the spiral ramp on the profile cut, I figured plunging straight down would be a problem which is why on the holes I chose to peck drill rather then go straight down. I figured a mill with a center cutting profile should be able to handle that.
It was driving me insane all night because everything i tried fit in with all the suggestions I could find on the forums. What was different was the depth I was cutting at... the tool data from harvey says I can cut at 1xthe bit diameter per pass but that doesn't work. I am going at it again when I get in today, have wiggle room on the size of my holes so rather then wait for a 3/16 mill I am going to bump my hole size up to 5/16. I think I have all my settings figured out...
13000 RPM x,y 1ips z-.5ips pass depth .03

[Brady Watson]

Peck drilling...is still plunging straight down into the material! You never drill AL on the Bot. You want to do an inside profile with spiral ramp using a smaller tool.

You cannot go by the specs put out by Harvey because you are not running a big heavy milling machine. You are running a light CNC router & have to make provisions for this.

Your speeds for profiling those tiny holes are impossible. Turn down the XY speed to like .4-.5 IPS.

-B

[robtown]

I generally shave aluminum, not cut it. Especially softer alloys. You look about right there with .03 per pass.

I've tried all different types of bits, generally speaking I've better success with larger dia bits so I use the largest dia I can when cutting. (my setup is a 2003 PRT with 4G)

As for the holes... I would just mark the plates by drilling a .02 - .03 deep hole where each hole goes, and do the holes on a drill press or with a drill by hand. It'll be quicker and probably save you some hassle. The router is cool and all, but it's not always the best tool for every task.

[twelchPTM]

Well thank you all for your help my plates turned out good enough for what they are.
Didn't see you last message till after the fact (Brady) I ended up still having problems with the al welding on to the bit, but after talking to the guys at Harvey and ShopBot I slowed the RPM's down to 10,000 and spilled some WD into the channel after the first pass. The holes came out okay to, it did sound a little funky but all turned out good.
If they were being produced for anything other then holding casters on a utility cart I would not have been happy with the edge finish but now that I have a solid starting point I will invest in a TiB coated bit with geometry intended specifically for al.

Also so as not to sound like a dummy... I get that pecking is still going straigt down, the thought process was (and I emphasize the word "was") that pecking would remove a small amount of material and pull out taking the shavings with it before going back in to remove a little bit more.

I have to move on to the next project and although AL most likely won't come up alot, I'm sure it will come up again and I'll have lots more questions and probly a few more broken bits.......