Plunge milling tips
Close
Login to Your Account
Results 1 to 11 of 11
  1. #1
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    154
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    26

    Default Plunge milling tips

    I'm working on a new part, aluminum. this part has an approximately 7" deep pocket 2x3 wide. I'm using an .750 iscar multimaster solid carbide bar with a 3 flute 1/2 loc end mill.

    After roughing everything as far down as I can with other tools I've found plunge milling to be the best method to remove the rest, aside from a little chatter against the walls it sounds great, albeit a little slow.... Maybe. I don't often use such long tools, so I'm curious to know what everyone else thinks of my feeds and speeds. I'll be going in tomorrow to kick up the feeds and speeds, I feel like 75 percent step over should be fine... Maybe, For now I'm at.

    350sfm (1782rpm)
    .0023 chip per tooth (12.3 ipm)
    .250 step over
    .350 plunge depth.
    Total material depth 2.100

    Mastercam morph toolpath, if anyone's curious.

  2. #2
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,670
    Post Thanks / Like
    Likes (Given)
    1238
    Likes (Received)
    2618

    Default

    Why not just use a Drill toolpath? Select points and drill.

    IMO your Speeds and Feeds are painfully slow. I'd probably start at 600 SFM (3056 RPM). And feed at .0175"(53.5 IPM). But if I used those Feeds, I would not step over more than 50%. I'm not sure how the Multimaster is going to do with Plunging. The insert ends on a straight shank, but I think the chips will spin off with the higher RPM. I'm assuming "plunge depth" means using a G73 chip breaking cycle, not G83 full retract...

    Plunge Milling is fast, fast. If it gives you the impression it's a slow process, that's the fault of the operator. Plunge Milling is/should be scary fast.

    R

  3. Likes Booze Daily, Jashley73 liked this post
  4. #3
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    3,659
    Post Thanks / Like
    Likes (Given)
    1261
    Likes (Received)
    1425

    Default

    Standard centre cutting endmill geometry is not optimal for plunging. The engagement angle on the face is the wrong side of zero, and the full side engagement causes the chatter you're experiencing.

    You can get high feed geometry heads for your multimaster, you should ideally switch out to one of those to get the most out of plunging.

    Stick to <30% stepover for plunging, so that you are always cutting near the peripheral edge of the cutter, that way you will not overload the centre and will have better chip control.

    You don't say what grade of aluminium, but say for like 6061T6 for example I'd be around 500m/min and ,07mm/t - 8375rpm, and 2345mm/m (92ipm) for a 4 flute high feed geometry head.

  5. #4
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    154
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    26

    Default

    Quote Originally Posted by litlerob1 View Post
    Why not just use a Drill toolpath? Select points and drill.

    IMO your Speeds and Feeds are painfully slow. I'd probably start at 600 SFM (3056 RPM). And feed at .0175"(53.5 IPM). But if I used those Feeds, I would not step over more than 50%. I'm not sure how the Multimaster is going to do with Plunging. The insert ends on a straight shank, but I think the chips will spin off with the higher RPM. I'm assuming "plunge depth" means using a G73 chip breaking cycle, not G83 full retract...

    Plunge Milling is fast, fast. If it gives you the impression it's a slow process, that's the fault of the operator. Plunge Milling is/should be scary fast.

    R
    I am drilling, in practice anyway. Why create a bunch of drill points when I can just select a drive surface an go. The motion is the same, I'm just using a different toolpath!

    As for feeds and speeds, I'm glad to hear that, I'll kick it up based on what you are telling me, but as always, especially with a $1000 tool I like to start slow. As for plunging depth, this would be the depth per pass, so I am plunging the entire path (each hole if you will) .350 deep before moving to the next depth. So the entire pocket gets roughed .350 at a time. My thought is to allow the chip somewhere to go given the stubby length of the cutter. Granted this likely isn't a real issue with the low step over.

    Thanks for your advice, I appreciate it!

  6. #5
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    154
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    26

    Default

    Quote Originally Posted by gregormarwick View Post
    Standard centre cutting endmill geometry is not optimal for plunging. The engagement angle on the face is the wrong side of zero, and the full side engagement causes the chatter you're experiencing.

    You can get high feed geometry heads for your multimaster, you should ideally switch out to one of those to get the most out of plunging.

    Stick to <30% stepover for plunging, so that you are always cutting near the peripheral edge of the cutter, that way you will not overload the centre and will have better chip control.

    You don't say what grade of aluminium, but say for like 6061T6 for example I'd be around 500m/min and ,07mm/t - 8375rpm, and 2345mm/m (92ipm) for a 4 flute high feed geometry head.
    Thanks, I definitely love the idea of high feed for plunging, However, I still need to finish the walls and floors, so high feed is out. I could buy a second tool, but man they are expensive.

    And yes 6061.

  7. #6
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,810
    Post Thanks / Like
    Likes (Given)
    4414
    Likes (Received)
    2911

    Default

    Quote Originally Posted by BRIAN.T View Post
    Mastercam morph toolpath, if anyone's curious.
    How did you tell Morph to do plunge milling? I love that toolpath.

  8. #7
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    154
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    26

    Default

    Quote Originally Posted by Mtndew View Post
    How did you tell Morph to do plunge milling? I love that toolpath.
    Yeah morph is the absolute best. It's in" Utility" bottom right of that page. Chain everything as you normally do.

  9. Likes Mtndew liked this post
  10. #8
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,670
    Post Thanks / Like
    Likes (Given)
    1238
    Likes (Received)
    2618

    Default

    Quote Originally Posted by BRIAN.T View Post
    so I am plunging the entire path (each hole if you will) .350 deep before moving to the next depth. So the entire pocket gets roughed .350 at a time.
    Might as well use a file or a spoon.

    Plunge milling is about moving material fast, not slow-doesn't make any sense. Use Gregor's advice with 30% step over, 100 IPM isn't weird.

    Drilling is the fastest way to move material on the Machine. Using a Plunge Milling is theoretically to replicate Drilling but faster, with step overs.

    R

  11. #9
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    10,197
    Post Thanks / Like
    Likes (Given)
    3459
    Likes (Received)
    3646

    Default

    QT: gregormarwick: [Standard centre cutting endmill geometry is not optimal for plunging.]

    I used to end sharpen for plunge milling with adding a couple degrees extra end clearance..and for aluminum avoid small/tight corners in gum-out.

    Steel can use 5 to 7* end clearance for plane milling but for plunge 7 to 11 may be better, for aluminum plunge 8 to 15 might do better.

  12. #10
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    154
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    26

    Default

    Quote Originally Posted by litlerob1 View Post
    Might as well use a file or a spoon.

    Plunge milling is about moving material fast, not slow-doesn't make any sense. Use Gregor's advice with 30% step over, 100 IPM isn't weird.

    Drilling is the fastest way to move material on the Machine. Using a Plunge Milling is theoretically to replicate Drilling but faster, with step overs.

    R
    Haha spoon. I'll give it a try in about 30 minutes, thanks!

  13. #11
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,810
    Post Thanks / Like
    Likes (Given)
    4414
    Likes (Received)
    2911

    Default

    Quote Originally Posted by BRIAN.T View Post
    Yeah morph is the absolute best. It's in" Utility" bottom right of that page. Chain everything as you normally do.
    Of all the times I have used that toolpath, I never even knew that option was there lol

  14. Likes BRIAN.T liked this post

Tags for this Thread

Bookmarks

Posting Permissions

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