reality check... how fast/hard are you machining aluminum lately? - Page 2
Close
Login to Your Account
Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 41
  1. #21
    Join Date
    Nov 2005
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    1,560
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    183

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    how round a circle you get at those feed rates ?
    At feeds of 3000, 5000, 7500 mm/min I would imagine a robodrill or any properly tuned machines will be less than 10 microns (that isn't really all that fast), but it is all going to depend on the circle sizes, anything proportioned properly (cutter<25% of hole), will likely be even better than that, as the acceleration won't be tool bad, with smaller holes and cutters obviously you won't be able to travel that fast accurately as there will be too much acceleration, but properly setup AICC will slow it down.

    When I get the time, I'll run a ballbar test and we will see, mind you it won't be under load, but neither really is finishing if done properly.

  2. #22
    Join Date
    Dec 2004
    Location
    uk
    Posts
    14,057
    Post Thanks / Like
    Likes (Given)
    4552
    Likes (Received)
    6699

    Default

    Quote Originally Posted by DMF_TomB View Post
    expensive part where boss gets upset over scrap parts you machine different. for many even a 1% scrap rate is totally unacceptable.
    .
    usually i look at load meter and whether i can hold a part and not have it move in vise or fixture.
    Have you any idea what that sub 1% scrap rate is really costing you? Can't believe many people are machining parts with less than a 20% profit margin, do the maths, but getting or trying to get scrap too low can cost far more than having a sensible allowance and scraping a bit more than 1%, comes a point were reducing errors gets costly far faster than you save anything.

    IMHO fixture is the number one thing that seams to get overlooked, nearly all the videos of high speed machining on you tube are nice big solid blocks held low down in a large vice, not all of us get to attack things as soft as aluminium and held that rigidly, feeds and speeds need to be looked at from a complete process perspective, some times a more creative setup, some times less secure can let you finish not just part machine a part, losing a complete separate operation can free up a lot of time for slower cutting conditions, pays to some times step back and look at the big picture.

  3. Likes iMillJoe, Bobw, Limy Sami, SIM liked this post
  4. #23
    Join Date
    Jun 2013
    Location
    St. Louis
    Posts
    653
    Post Thanks / Like
    Likes (Given)
    472
    Likes (Received)
    294

    Default

    In general you can go much faster, but... things are going to be heavily machine dependent. Given the right tooling, the machine is going to be your weakest point. Few machines have the Spindle speed/acceleration/rigidity to make full use of the cutters we have to day. My idea is, you use what you've got the most of. If you have a big 50 taper with a slow spindle, use those fancy tool paths, just use wide step overs, and feed till you start maxing loads/breaking shit. If you have a little 30 taper, spin that spindle fast as ye can, crank that feed up as fast as you can, and make the stepover as much as you can handle. If you have a decent 40 taper, find some combination that works. Keep in mind, I've heard that software you're running referred to as "air cam" because it's always cutting lots of air. Cutting air does not make your boss money.

    I used a dynamic MC mill path for a pocket in AL for the first time in a while last week. 1/2 EM, 1" depth, .125' stepover, My starting point for feed was .008 per tooth (480 IPM). I forget exactly where I got after massaging the program, but in places, MUCH faster than that.

  5. Likes wheelieking71 liked this post
  6. #24
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    929
    Post Thanks / Like
    Likes (Given)
    1094
    Likes (Received)
    573

    Default

    Quote Originally Posted by adama View Post
    Have you any idea what that sub 1% scrap rate is really costing you? Can't believe many people are machining parts with less than a 20% profit margin, do the maths, but getting or trying to get scrap too low can cost far more than having a sensible allowance and scraping a bit more than 1%, comes a point were reducing errors gets costly far faster than you save anything.

    IMHO fixture is the number one thing that seams to get overlooked, nearly all the videos of high speed machining on you tube are nice big solid blocks held low down in a large vice, not all of us get to attack things as soft as aluminium and held that rigidly, feeds and speeds need to be looked at from a complete process perspective, some times a more creative setup, some times less secure can let you finish not just part machine a part, losing a complete separate operation can free up a lot of time for slower cutting conditions, pays to some times step back and look at the big picture.
    Depends entirely on the work. If your stock is $20/part, don't worry to much about it, most of what you're losing is time. I know folks however who work on projects with $50,000 per part stock, with a six month lead time on that stock. You do not want to mess that up no matter what.

  7. Likes Mtndew liked this post
  8. #25
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,366
    Post Thanks / Like
    Likes (Given)
    1169
    Likes (Received)
    2395

    Default

    Quote Originally Posted by mhajicek View Post
    Depends entirely on the work. If your stock is $20/part, don't worry to much about it, most of what you're losing is time. I know folks however who work on projects with $50,000 per part stock, with a six month lead time on that stock. You do not want to mess that up no matter what.
    He knows, and we all know what Tom works on--$100,000,000,000,000 USD parts that come from Taiwan and he sets upon the Toyoda and uses the Excel spread sheet to track which Tool breaks and why. With those type of parts "scrap" is not an option. But there are ways to machine giant shit and mess up before you call it scrap, duh.

    Totally off topic as usual, the topic is "how fast/hard are you machining Aluminum"

    R

  9. Likes Mtndew liked this post
  10. #26
    Join Date
    Dec 2004
    Location
    uk
    Posts
    14,057
    Post Thanks / Like
    Likes (Given)
    4552
    Likes (Received)
    6699

    Default

    Quote Originally Posted by mhajicek View Post
    Depends entirely on the work. If your stock is $20/part, don't worry to much about it, most of what you're losing is time. I know folks however who work on projects with $50,000 per part stock, with a six month lead time on that stock. You do not want to mess that up no matter what.
    Yes and no, assuming your then selling that part for 70K, and for simplicities sake your just tapping 1 hole. You make 20K a part, Now if you so long as you don't scrap any more than 1 part in any 3 your making money. To hit the magic 1% scrap rate, you get to make 2 million profit, but to totally eliminate any chance of scrapping that 50K part how much of that 20K profit do you spend. At what point does the profit become so small its not worth bothering with equally at what point does the profit become so small the risk even though infinitesimally small of scrapping one means you never make a profit?

    Tomb's castings are probably a lot more realistically in a few thousand range, hence like it or not, you have a lot less you can afford to spend on not scrapping one before you make no money. Its all risk and reward, yeah you want to minimise the risk, but holding back 50% on production to run a more steady pace may be killing your competitive edge far more than having that 1% scrap rate hit say 3%.

    But this all comes back to how fast, you don't know how fast you can go till you have exceeded 100% For high speed tool paths hes unquestionably leaving a fair bit of speed untapped, problem is like tomb rightly says your machines, your cutters and your process all reflect what those numbers really are.

    IMHO he needs to also look at what a typical machining movement is and what his machine accelerates at, there's no use baseing step overs on 10% radial engagement and 10Krpm if the moves are only long enough for his machine to hit 50% of the programmed feed rate. If hes got that issue, bumping up the radial depth of cut to regain the chip thickness and the material removal rate becomes a firm winner. The above post - video on youtube of the heavier cutting being faster is also valid, its no good hauling ass with HSM if your spending half the day rapiding back to a starting point. You need to look at the big picture to truly gain speed and beat your competition.

  11. #27
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    653
    Post Thanks / Like
    Likes (Given)
    132
    Likes (Received)
    706

    Default

    Quote Originally Posted by Finegrain View Post
    Not to be private investigator or anything, but, you are running very conservatively assuming you have fairly modern machines. Your 12,000 RPM parameters shown above give 12 in^3 per minute MRR. I'm running 40-60 in^3 per minute on my relatively lightweight 30-taper Brother, every day. I have essentially 0 scrap rate due to running too hard. About the only time scrap happens is when I make a programming mistake. Higher priced cutting tools? Yes, but they can pay for themselves within the first day of high-efficiency cutting, and then they last a long time after that. Rough guess is I can put a couple 1000 # of chips into the bin with a single Destiny Diamondback. Actually I have no idea what the wear life of a Diamondback is, as they usually suffer some other, more abrupt fate (usually programming error) before they wear out.

    I will grant you that if you have a 20-year old machine that wasn't designed for high feed rates, you are probably asking too much. But, the OP says he works in an "aerospace shop" so I can only assume they have decent machines.

    Regards.

    Mike

    Yes, I agree. 99% of what I run is low volume, high value products. It is not unusual for me to write and set-up ten operations per day, that might run 10 parts. I rarely have time to do elaborate (and rigid) fixturing, nor can I afford to have the first part not be right. As a result, I have a tendency to be pretty conservative. That being said, the feeds and speed suggested by the OP seem pretty good for getting good parts, every time. Could they be more aggressive, absolutely. If he was running high volume production, the cycle times could be probably be cut in half. When I setup for volume production, my feeds and speeds are more aggressive, but day in day out, the numbers he suggested make a good part every time.

  12. #28
    Join Date
    Feb 2009
    Location
    Midwestern MN/Wi USA
    Posts
    1,333
    Post Thanks / Like
    Likes (Given)
    74
    Likes (Received)
    366

    Default

    Max your spindle RPM, take a .013 chip load on tools larger than .374 and give yourself a 12-20% step over on cuts deeper than .75.

  13. Likes wheelieking71 liked this post
  14. #29
    Join Date
    Feb 2009
    Location
    Midwestern MN/Wi USA
    Posts
    1,333
    Post Thanks / Like
    Likes (Given)
    74
    Likes (Received)
    366

    Default

    Dont feed back zig zag that cut

  15. Likes wheelieking71 liked this post
  16. #30
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    5,752
    Post Thanks / Like
    Likes (Given)
    7180
    Likes (Received)
    7306

    Default

    Quote Originally Posted by Speedie View Post
    Dont feed back zig zag that cut
    Been waiting two days for that! LOL

  17. Likes Speedie liked this post
  18. #31
    Join Date
    Jan 2013
    Location
    Gilbert, AZ
    Posts
    5,752
    Post Thanks / Like
    Likes (Given)
    7180
    Likes (Received)
    7306

    Default

    Quote Originally Posted by adama View Post
    Now if you so long as you don't scrap any more than 1 part in any 3 your making money.
    No, your not. Because that customer is freaking gone.

    You guys are getting waaaaay to deep for the OP's simple question.

    Bye-the-way, Tom, GTFO of here, you have no dog in this fight. All you did was plow it off course.

    Here is a relevant response the OP can use to his adavantage:
    I run a 3/8" SGS S-carb, 1" deep, .075" stepover, 12,000rpm, 250ipm (straight line) in a HAAS.
    I speed up 50% around an outside corner. Slow down 20% in an inside corner. And, this is machine acceleration limited.
    I run 250ipm because the HAAS cant think any faster in anything less than 3-4" straight line.
    In an Okuma GENOS? I bet 300-350ipm would fly.

    I been watching this for two days. Some great responses. Some freakin' stupid ones as well.

  19. Likes litlerob1, Mtndew, gkoenig, mhajicek liked this post
  20. #32
    Join Date
    May 2002
    Location
    South Central PA
    Posts
    13,440
    Post Thanks / Like
    Likes (Given)
    2169
    Likes (Received)
    3364

    Default

    Quote Originally Posted by Finegrain View Post
    I will grant you that if you have a 20-year old machine that wasn't designed for high feed rates, you are probably asking too much.
    That would be me.
    We just started experimenting with a Korloy Ripper from Exkenna. Applied it to a 6061 part we normally did with an Iscar 2 flute 2" dia E90AL tool. With a previous machine we were maxed at 4000 rpm and 150 Ipm, the machine was happy at .125 DOC. So we ran it in a newer machine at the same parameters, the roughing toolpath took about 10 minutes out of 25-30 for the entire part. Received the 4 flute 2" tool from Curtis a week or two ago. Korloy says run a max of 8K rpm so we tried that at .250 DOC, 80% WOC where possible. Started at 250 IPM and ramped up to 300+ using feed override. Over 180 IPM the cutter started to gouge the part on outside arcs due to the heavy machine and old control. So we tried .400 DOC and 150 IPM and it's a lot happier. It looks like we can push the DOC deeper but we saved 5 minutes on roughing already and decided to just run the parts and experiment with parameters and toolpath strategy later.

    This Korloy tool runs way quieter than the Iscar at twice the speed. My impression is it would be more forgiving on part retention, it sounds like a router running compared to a wood chipper.

    We haven't tried waveform/trochoidal toolpaths. I have the CAM but I doubt it would be the best plan for this machine. It will cut at 400 IPM but I doubt the Acc/Dec parameters will reach that on short moves, It's rated for 5000 lb workpiece and the table and saddle probably weighs what a whole Brother does.

  21. Likes wheelieking71 liked this post
  22. #33
    Join Date
    Feb 2009
    Location
    Midwestern MN/Wi USA
    Posts
    1,333
    Post Thanks / Like
    Likes (Given)
    74
    Likes (Received)
    366

    Default

    That is using some meat behind it for sure.

  23. #34
    Join Date
    Feb 2005
    Location
    Akron, OH
    Posts
    1,824
    Post Thanks / Like
    Likes (Given)
    277
    Likes (Received)
    1368

    Default

    Be careful with the ripper mills: you can push them absurdly hard and spin them scary fast, but if a part pulls out of the workholding you're buying a new body, not just new inserts.

  24. Likes Mud, LostFab liked this post
  25. #35
    Join Date
    May 2002
    Location
    South Central PA
    Posts
    13,440
    Post Thanks / Like
    Likes (Given)
    2169
    Likes (Received)
    3364

    Default

    Quote Originally Posted by Comatose View Post
    Be careful with the ripper mills: you can push them absurdly hard and spin them scary fast, but if a part pulls out of the workholding you're buying a new body, not just new inserts.
    We broke some Iscar tools in the previous machine, snapped the body at the retention screw hole.

  26. #36
    Join Date
    Dec 2017
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    56
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    15

    Default

    My new tool of choice for aluminum is a kennametal 1" dia with (2) 1-18 inserts. There are plenty of different options with those inserts, but this is an integrated Cat40 shank. It's great for running vertical walls because of a reduced shank size. Anyway, I am running it at .7 DOC (max) with .15 step over, 300 IPM at 12k on my Hurco VM10i. I can probably push it more but I am mostly doing 1 or 2 off prototype work and don't have that much to gain with a little cycle time.

  27. Likes thesidetalker liked this post
  28. #37
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,366
    Post Thanks / Like
    Likes (Given)
    1169
    Likes (Received)
    2395

    Default

    Quote Originally Posted by TonyStark View Post
    My new tool of choice for aluminum is a kennametal 1" dia with (2) 1-18 inserts. There are plenty of different options with those inserts, but this is an integrated Cat40 shank. It's great for running vertical walls because of a reduced shank size. Anyway, I am running it at .7 DOC (max) with .15 step over, 300 IPM at 12k on my Hurco VM10i. I can probably push it more but I am mostly doing 1 or 2 off prototype work and don't have that much to gain with a little cycle time.
    I din't know you had a Hurco, in the movie you have a green Mori lathe, late 80's, single spindle with a Fanuc 3-T. Shouldn't have stepped down to the Hurco.

    R

    It would be either funnier or less funny, if that were your real name.

  29. #38
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    695
    Post Thanks / Like
    Likes (Given)
    103
    Likes (Received)
    361

    Default

    Quote Originally Posted by TonyStark View Post
    My new tool of choice for aluminum is a kennametal 1" dia with (2) 1-18 inserts. There are plenty of different options with those inserts, but this is an integrated Cat40 shank. It's great for running vertical walls because of a reduced shank size. Anyway, I am running it at .7 DOC (max) with .15 step over, 300 IPM at 12k on my Hurco VM10i. I can probably push it more but I am mostly doing 1 or 2 off prototype work and don't have that much to gain with a little cycle time.
    I have the 3 flute Ø1.25" x 3" long version. Awesome tool.

  30. #39
    Join Date
    Dec 2017
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    56
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    15

    Default

    Quote Originally Posted by thesidetalker View Post
    I have the 3 flute Ø1.25" x 3" long version. Awesome tool.
    And at $300ish they a really a deal when you consider how much a quality cat40 toolholder and large/long carbide tooling costs. I may get the straight shank version of the 1.25 because I need a little more reach for a project, but I haven't found a really solid way to hold that doesn't stick out 8 or 9 inches

  31. #40
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,032
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2609

    Default

    just saying at high feeds many cnc cannot mill a true circle to .005" and corners are not precise when it turns direction. i have seen older machines where at high feeds tolerances get worse. all you got to do is measure parts coming off a rougher
    .
    theirs a reason .010 to .020" is left from roughing for finishing


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
  •