Newbie Knots in my Aluminum?!?

Results 1 to 8 of 8

Thread: Knots in my Aluminum?!?

  1. #1
    Registered
    Join Date
    Jan 2011
    Location
    United States
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default Knots in my Aluminum?!?

    Hi. I need help diagnosing what happened (what I did wrong) making a simple part (a heat-sink) from some scrap Aluminum I had on hand. I have no idea what type of Al alloy it is, but assumed 6061. I ran two attempts with the following settings:

    Machine is a Sieg SX3
    Max RPM: 1800

    Run #1
    Two flute 0.125 endmill w/ 3/8" shank
    Speed 1000 RPM
    Feed 1.25 IPM
    Depth of cut: 0.050
    (Speeds and feeds come from another site where "rule of thumb" calcs are given.)
    Actual S & F given by calcs was 12,800 RPM at 16 IPM. Recalculating using 1000 RPM gave the numbers I used. I am just not comfortable yet running flat out with the spindle. I'm also concerned that Al tends to be gummy sometimes and will start sticking to the endmill and work if the spindle is going too fast. That's what I've been told as some time or other.

    Here is the picture of the first run. Disregard the half-holes surrounded by the blue box. This was scrap with a few shallow holes in it and they would not hurt the intended application.
    Knots in my Aluminum?!?-heatsink-1-marks-jpg
    The arrows show the intended path. I started off the part, made the first slot moved down (Z at same elevation) and started the second slot. At the red circle, I no longer had an endmill with any flutes. It flew off somewhere and was never found. I was hand flooding the endmill with WD-40 along the whole way.

    Here is a shot of the chips that were made. I think they look pretty good. The machine was not complaining, no chatter or vibration. Cutting well, but sloooooow (at 1.25 IPM!)
    Knots in my Aluminum?!?-chips-3-jpg

    So, I think maybe I had a bad endmill or the "rule of thumb" calcs were just off too much.

    Run #2
    I then used a software S&F calculator and to be honest, did not want to run the mill at 1800 RPM max, so I forced a recalculation for 1000 RPM and got a feed rate of 0.5 IPM. Really slow, but I have time.

    Loaded in a new endmill, same size and shank as the first one. Restarted the program from the beginning. The second endmill had nothing to do till it got to the end of the second slot where the other broke. As soon as it got there, it ALSO broke off!

    Here's a shot of where the endmills went to the great tool crib in the sky.
    Knots in my Aluminum?!?-end-cut-mills-broke-2-jpg

    I can see where the endmills pulled (down) towards the hole instead of going exactly straight before the "event." So they must have grabbed. The work was held in a vise and did not move. The setup was very secure.

    So, I have no idea what I did wrong. Too aggressive a DoC? Really gummy Al and not 6061 throwing off all S&F calculations? OR (my favorite) I hit a knot at that point in the blank.

    Help!

    And thanks for helping a newbie. I'm now out of 0.125 endmills, but have more on order. I'd like to keep them if possible...

    Similar Threads:


  2. #2
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Knots in my Aluminum?!?

    A knot in the aluminum is not out of the question. I found a ball bearing in one piece I was working on. But....I think you need to speed the spindle up to the max, and keep the feed at 0.5 IPM. Maybe adjust the DOC also. You might try a router bit, I use those all the time in aluminum and they're available at your local hardware store. Flooding with WD40 is the right thing to do. You have to keep the bit wet with coolant when cutting aluminum. In my machine, I would cut that at about 4000 RPM, with a chip load at about 0.001 per flute.

    Judging from the burr on the edge of the cut, it also looks like your end mill was dull or the feed was way too fast for the spindle speed.

    Last edited by Jim Dawson; 12-23-2016 at 06:33 PM.


  3. #3
    Registered
    Join Date
    Jan 2011
    Location
    United States
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default Re: Knots in my Aluminum?!?

    Thanks, Jim. I also left out the the endmills were HSS imports. Nothing special.

    Now when you say router bits, what's different about them? (I am not a wood worker and have never even held a router.) Also, when you mentioned adjusting the DOC, I assume you meant to be shallower, correct?

    I'm glad you caught that about the burr. I was thinking that was a benefit of cutting a slot; nice and clean on the Climb Mill side and grotty on the Conventional side. It did change sides when the mill changed direction, so that's what got me thinking about that.

    Thanks for the help! Very much appreciated!



  4. #4
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Knots in my Aluminum?!?

    Happy to help.

    Router bits have more chip clearance and a bit different cutting geometry and also typically will be razor sharp. In a 1/8 size will normally be single flute with a 1/4 inch shank. Available in HSS, carbide tipped, and solid carbide. But more importantly, they are relatively inexpensive, and when you break one on a Saturday afternoon you can run to your local hardware store and get a new one.

    I have found that some of the import end mills are not sharpened properly, but that normally is not a huge problem for utility use. Yes, a shallower DOC might be helpful, with an end mill that size, maybe try 0.020 or so. A nice sharp end mill under good conditions won't leave a noticeable burr.

    I should also mention that you should be using a 1 or 2 flute end mill in aluminum, or maybe a 3 flute in larger sizes.



  5. #5
    Registered
    Join Date
    Jan 2011
    Location
    United States
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default Re: Knots in my Aluminum?!?

    Will the router bits get dull faster than "official" endmills? Any reason to go with a name brand vs. house brand (if there is such a thing) at our local Lowes or Home Depot?



  6. #6
    Registered
    Join Date
    Jan 2011
    Location
    United States
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default Re: Knots in my Aluminum?!?

    Well, here it is. After a new, good, sharp end mill, lower depth of cut (to 0.020), RPMs to max (1775) a lot of WD-40 and about an hour and a half, here's what I ended up with:

    Knots in my Aluminum?!?-heatsing-milling-finished-jpg

    I still need to mill down the top some to match the bottom (it turns out that my blank was 0.1 taller than I designed for), and then cut it in half (top to bottom through the middle - it's actually two identical parts).

    Thanks for the help, Jim. You gave me a lot of practical advice on the settings and that made the difference. I'm trying to get a handle now understanding chip load and think I'm making progress. But what you said sure made a difference. Now I have parts I can use!



  7. #7
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: Knots in my Aluminum?!?

    Quote Originally Posted by jrmachinist View Post
    Will the router bits get dull faster than "official" endmills? Any reason to go with a name brand vs. house brand (if there is such a thing) at our local Lowes or Home Depot?
    I have found that router bits are just as good as endmills, but are not as robust. The web is a bit thinner than the same sized end mill, I assume this is for increased chip clearance. Home Depot carries Diablo brand, and Lowes carries Botch. Both seem to be about the same quality, but be advised, most are undersized a bit. I have seen the 1/4 inch solid carbides as small as 0.239 at the cutter end. The shanks all seem to be dead on. You just have to make adjustments in your cutter comp.

    Quote Originally Posted by jrmachinist View Post
    Well, here it is. After a new, good, sharp end mill, lower depth of cut (to 0.020), RPMs to max (1775) a lot of WD-40 and about an hour and a half, here's what I ended up with:

    Knots in my Aluminum?!?-heatsing-milling-finished-jpg

    I still need to mill down the top some to match the bottom (it turns out that my blank was 0.1 taller than I designed for), and then cut it in half (top to bottom through the middle - it's actually two identical parts).

    Thanks for the help, Jim. You gave me a lot of practical advice on the settings and that made the difference. I'm trying to get a handle now understanding chip load and think I'm making progress. But what you said sure made a difference. Now I have parts I can use!
    Glad to help out where I can. Happy it worked out for you.



  8. #8
    Member
    Join Date
    Apr 2009
    Location
    USA
    Posts
    5516
    Downloads
    0
    Uploads
    0

    Default Re: Knots in my Aluminum?!?

    Quote Originally Posted by jrmachinist View Post
    Well, here it is. After a new, good, sharp end mill, lower depth of cut (to 0.020), RPMs to max (1775) a lot of WD-40 and about an hour and a half, here's what I ended up with:

    Knots in my Aluminum?!?-heatsing-milling-finished-jpg

    I still need to mill down the top some to match the bottom (it turns out that my blank was 0.1 taller than I designed for), and then cut it in half (top to bottom through the middle - it's actually two identical parts).

    Thanks for the help, Jim. You gave me a lot of practical advice on the settings and that made the difference. I'm trying to get a handle now understanding chip load and think I'm making progress. But what you said sure made a difference. Now I have parts I can use!
    My "rule of thumb" on most harder aluminum is to use a chipload of .0028" for a 1/4" endmill, then adjust proportionately to the tool diameter. So an 1/8" endmill would be .0014", a 1/16" endmill .0008", etc. The federate equation is simple:

    Feedrate = chipload X number of flutes X spindle speed.

    In your example, at 1775rpm, and a 2-flute endmill 1/8" diameter, I'd go at about 5ipm. I'd adjust the depth based on machine rigidity, but for full engagement (slotting) I typically do between 1/2 to 1/4 the tool diameter for depth of cut. Also as much as possible, use a stub endmill, and stick it out just past the flute fadeaway, as that gives you the most rigid setup possible. The closer the collet to the work, the better. I always cringe when I see someone cutting a 1/8" pocket with a tool with a 1" flute. It's just an invitation to vibration and poor surface finish. Plus the tool will flex, severely limiting your depth of cut. Of course, there may be clearance or fixture issues that may necessitate such a thing, but it's usually best to rework your fixturing.

    If your tools are galling, surface is bad, or you're getting BUE (built-up edge), you should either lower spindle speed, raise the feed rate or both.

    True endmills for aluminum have very highly polished, rounded flutes ("O" shaped), very sharp edges. They would also have what are called "sweeps" on the tips that make the pocket floor nice and smooth. Coated tools (ZrN, TiN, CVD) help a lot because they have more lubricity than uncoated endmills, but as you discovered, using a lubricant helps a lot.



Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Knots in my Aluminum?!?

Knots in my Aluminum?!?