509,836 active members
3,295 visitors online
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Haas Mills > speed and feed recomendations
Results 1 to 6 of 6
  1. #1
    Registered
    Join Date
    Jul 2004
    Posts
    100

    speed and feed recomendations

    Hello, I am running a job in 6061 that has a .2 deep slot, 12" long and .625 wide.
    I drill an entry hole and plunge a 1/2" 2-flute (HHS TIN) to Z-.195 in and then do the G41 thing to a tangent point on the other end while going to Z-.2 to get a nice bottom finish.
    Running at 4000 RPM and 30 IPM. I am using Castrol Syntolo 10%
    Then continue the G41 moves to make the rounded end slot.
    With this cutter how hard can I push it?
    Regards, Ray
    ​"There is no such thing as a gun free zone."
    Ray Brandes, Ray-Vin.Com, PCB, FL 32408 USA

  2. #2
    Registered
    Join Date
    Apr 2003
    Posts
    1871

    Re: speed and feed recomendations

    Ray
    It would be my estimation that you are presently pushing it plus at -.2 and 30ipm.

    Ken

  3. #3
    Registered
    Join Date
    Jul 2004
    Posts
    100

    Re: speed and feed recomendations

    Ken,
    Well, after a couple of days with no replies, I decided I might have to sacrfice a cutter to find out where the edge is. I brought up Haas' caculator and started plugging in numbers. I was using 300FPM for aluminum, but the caculator suggested 600-900! Well, I went with something like 800 and it gave me 5500 RPM and 56 IPM. I plugged it in and the cutter took it just fine.
    I reviewed other tools in the program and found I could goose them up too and I did.
    My notes from the first time I ran this job showed 6-1/2 minutes per part and I have now got that down to 3:12.
    Regards, Ray
    ​"There is no such thing as a gun free zone."
    Ray Brandes, Ray-Vin.Com, PCB, FL 32408 USA

  4. #4
    Registered
    Join Date
    Apr 2003
    Posts
    1871

    Re: speed and feed recomendations

    Sounds like that was time well spent Ray!
    A bit surprised that you can get that kind of feed out of a standard HSS cutter, I've two respected programs that show substantially lower figures.
    Actually, they are showing at 5600rpm essentially the 30ipm (less at the 4000) you mentioned in your first post, as is said, it's difficult to argue with success so it's good news for you when you can cut machining time down that much.

    Ken

  5. #5
    Gold Member
    Join Date
    Nov 2007
    Posts
    1663

    Re: speed and feed recomendations

    Aluminum? With flood coolant and a 0.5" endmill, you should be running at whatever max RPM your machine has. In my machines, that's 10K RPM, A 2-flute at a very conservative 0.003" per tooth should slot at 60 IPM. The demos that Haas runs at all the trade shows run much higher numbers than that. The only caution I would add is that you need to have the part very tightly held. With aggressive cuts, come aggressive pushing and pulling forces. If the part comes out, the cutter is almost always scrapped. Go to Youtube and watch some of the Haas demo videos to get some idea what kinds of cutting speeds you should be running.

    Also: you shouldn't need the starter hole. The endmill should be able to plunge at 10 IPM or better. The only exception to this is high-helix endmills, where the cutting edge has very little support. They don't like being plunged. In either case, if you don't like plunging, you can ramp into the cut over some distance. That takes the center-cutting load out of it and allows good chip evacuation.

    Finally, cutters matter. Everybody has preferences. I have used some real junk from major brands. What I have found that I'm totally hooked on, is the Niagara line of cutters. I really like their 3-flute 0.5" endmills. They leave an amazing finish and the difference in cutting is immediately noticeable, just in the audible sound the cut makes. They're noticeably quieter and leave both a great wall and floor finish. Until I found those, we were getting terrible side-wall finish. Warning: they aren't cheap but, if cycle time and finish are important, you can't afford to NOT use them.

    So: if you ran the Niagara 3-flute, you now have an additional cutting edge in there. You run it at a conservative 0.003 per tooth, 10K RPM = 90 IPM. Eliminate the pre-drilled hole. That cuts out both the drill time and the tool-change time. Those two changes should cut a minute or more out of your cycle time. At the end of the day, that will add up.
    Greg

  6. #6
    Registered
    Join Date
    Jul 2004
    Posts
    100

    Re: speed and feed recomendations

    Greg,
    Thanks for the feed back. I got a couple of nice 3/4 Niagra 3-flute roughers in a batch of tools I bought and I love them.
    This job is done, but it comes back several times a year so I am putting in my notes what try.
    Regards, Ray
    ​"There is no such thing as a gun free zone."
    Ray Brandes, Ray-Vin.Com, PCB, FL 32408 USA

Similar Threads

  1. Replies: 1
    Last Post: 02-11-2015, 02:38 AM
  2. Replies: 0
    Last Post: 11-01-2014, 09:10 PM
  3. feed and speed for high speed
    By Darth Yoda in forum BobCad-Cam
    Replies: 2
    Last Post: 12-05-2012, 05:14 PM
  4. Speed & feed THEN
    By riche543 in forum Calibration / Measurement
    Replies: 1
    Last Post: 12-16-2011, 12:29 PM
  5. Speed And Feed
    By superrotary in forum Uncategorised MetalWorking Machines
    Replies: 0
    Last Post: 09-28-2007, 04:23 AM

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
  •