3d surfacing challenges, your best guess at this prob
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 23
  1. #1
    Join Date
    Jul 2021
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Question 3d surfacing challenges, your best guess at this prob

    So, I have successfully surfaced this with a 1/16th ball mill a couple times. All the other times is comes out like this photo attached. Really fuzzy and raspy on the flats.

    I am running it at MAX rpm for the mill (11,500. I know 20k or 30k would be better but aint got it.) and at about .0005 IPT chipload and .0035" stepover, attempted with both scallop and raster(parallel) toolpaths. Tried with both 2 and 4 flute endmills and only had success a couple times.

    A few questions I have are, given the 3d shapes, how much should I leave for the ball? I've been trying .003 before the final pass but should I do more? .010 or .012? Im stumped... Tried everything.. Maybe more chipload?
    surf-finish.jpg

  2. #2
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3,890
    Post Thanks / Like
    Likes (Given)
    2850
    Likes (Received)
    2493

    Default

    hard to tell from the pic.
    tool could be way out of balance or maybe youre recutting the chips.
    what doess your coolant setup look like? relative to how much material to leave for finish....what material are you cutting? are you able to cock the tool or work piece over on and angle so that you aren't using the zero velocity portion of the tool?

  3. #3
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    868
    Post Thanks / Like
    Likes (Given)
    251
    Likes (Received)
    668

    Default

    Looks like a broken tool (or really bad grind on center) from here. Some of the shiny spots appear to be where it changes tangency and cuts on a different part of the ball.

    If that happened here, I would say with certainty it's a broken tool. Sometimes tools that appear to be good start leaving fuzzy finishes, and we toss 'em. Like allout says though, there are so many variables it's hard to tell for sure.

    Also, I've never had a ball want more chipload for surfacing. The folks who get really nice finishes running 40k spindles are rarely feeding fast enough to keep the chipload high.

  4. #4
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    10,394
    Post Thanks / Like
    Likes (Given)
    1420
    Likes (Received)
    3814

    Default

    Are you roughing this with the equivalent sized ball mill prior to the finishing pass? It appears to me that the tool plugged up, as would happen if it had to clear those deeper details with too much stock remaining from the previous toolpath.

  5. #5
    Join Date
    Jul 2021
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    The previous "semi finish" tool is a .250 ball mill, leaving like .003 stock everywhere... I am using a brand new ball mill every time to try and finish and it keeps looking like that...

    its 1018 steel.

  6. #6
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    8,871
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    4299

    Default

    I don't s'pose you could tilt the part a little so it's not trying to cut with the center of the ball ? If you look at the photo, on areas that are steeper you don't have that problem ...

  7. Likes mkd, lumley32 liked this post
  8. #7
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    2,009
    Post Thanks / Like
    Likes (Given)
    2740
    Likes (Received)
    1403

    Default

    Do it in prehard 4140, it'll cut cleaner.

  9. Likes mkd liked this post
  10. #8
    Join Date
    Sep 2015
    Country
    CANADA
    State/Province
    Ontario
    Posts
    122
    Post Thanks / Like
    Likes (Given)
    65
    Likes (Received)
    53

    Default

    Rough it a bit closer, .001" should work better and increase the chipload a bit, maybe .002" to start

  11. #9
    Join Date
    Jan 2003
    Location
    Posts
    617
    Post Thanks / Like
    Likes (Given)
    137
    Likes (Received)
    202

    Default

    Quote Originally Posted by 007Rob View Post
    Rough it a bit closer, .001" should work better and increase the chipload a bit, maybe .002" to start
    Id try going close like this too. Roughing with a 1/4 tool is probably leaving a lot in tight corners. I would rough it really close with the 1/16 tool, then do a final finish pass with a brand new 1/16th tool.

  12. #10
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    1,288
    Post Thanks / Like
    Likes (Given)
    1337
    Likes (Received)
    825

    Default

    I agree on upping the chip load. I'd start at .001" ipt and bump it up from there

  13. #11
    Join Date
    Sep 2018
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,378
    Post Thanks / Like
    Likes (Given)
    2149
    Likes (Received)
    754

    Default

    pretty obvious IMO whats going on here. you dont have enough SFM, or chipload is too high for cutting so close to, or on the bottom of the ball. the fact that it only looks bad where its near the center is a dead giveaway.
    drop your feed, look into a ball mill with one flute going past the center.
    also if you're using a larger than 2 flute endmill, your chipload is not accurate when you get close to the center since the geometry only allows for max of 2 flutes on a ball mill.

  14. #12
    Join Date
    Aug 2014
    Location
    Indiana
    Posts
    172
    Post Thanks / Like
    Likes (Given)
    109
    Likes (Received)
    275

    Default

    Quote Originally Posted by LouGold View Post
    The previous "semi finish" tool is a .250 ball mill,
    Could it be gouging? It seems to me that there is a lot of work for a 1/16 ball nose to clean up from a 1/4 ball nose. If it was me I would probably put an 1/8" ball nose as my semi finish after the 1/4 and then follow up with a 1/16 after that.

  15. #13
    Join Date
    Jun 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    1,274
    Post Thanks / Like
    Likes (Given)
    989
    Likes (Received)
    593

    Default

    Ball endmill is clearly chipped/broken.
    fixes have already been listed.
    I favor prehard material for cutting consistency sake.

  16. #14
    Join Date
    Jul 2006
    Location
    Hillsboro, New Hampshire
    Posts
    13,943
    Post Thanks / Like
    Likes (Given)
    3056
    Likes (Received)
    9237

    Default

    As some have said, the 1/4" rougher is too big to go right to the 1/16" finisher, use a 1/8" for semi-finishing. I'd leave a nominal .003", that feels about right.

    What are you using for coolant, if any? What machine are you using, is this a proper VMC, or a router? What brand, coating, flute count and length cutters are you using?

    Can you post close-up pics of a used cutter? It would be interesting to see its condition.

    Agree with those saying tilt the plate and recode, but more than ~5-10 degrees may cause issues with some features depending on depth.

  17. #15
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    14,049
    Post Thanks / Like
    Likes (Given)
    4788
    Likes (Received)
    5067

    Default

    You might get a 10x loop and inspect your cutter bits, perhaps one bet vendor/name is better than another.

    Failure to make a good end on a radius bit is a common error.
    I used to know a fellow who finished ground carbide bits. He ground them by hand under a magnifying glass.

  18. #16
    Join Date
    Jul 2021
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by Milland View Post
    As some have said, the 1/4" rougher is too big to go right to the 1/16" finisher, use a 1/8" for semi-finishing. I'd leave a nominal .003", that feels about right.

    What are you using for coolant, if any? What machine are you using, is this a proper VMC, or a router? What brand, coating, flute count and length cutters are you using?

    Can you post close-up pics of a used cutter? It would be interesting to see its condition.

    Agree with those saying tilt the plate and recode, but more than ~5-10 degrees may cause issues with some features depending on depth.

    Milland:

    the coolant is a full synthetic (Called synergy I believe)

    The 1/16 finishing cutter is always brand new before we start the finishing on a plate. I have tried 1/16" HARVEY 2FL balls, 4 flute balls, lakeshore carbide brand, redline tooling brand.

    It is a proper VMC.. Its a Smart SM1165 (made by samsung) 12K spindle, but we're trying not to pin it at 12K for hours and running around 11,500RPM.

    Milland, given your previous recommendations, What would you run for chipload on a 2FL ball, leaving about .003" stock to finish?

    Thanks a bunch to everyone for your input!

  19. #17
    Join Date
    Aug 2006
    Location
    Wisconsin
    Posts
    1,767
    Post Thanks / Like
    Likes (Given)
    806
    Likes (Received)
    818

    Default

    2 flute PREMIUM endmills for finishing only. If you must go economical, OSG has a new series to compete with the "cheaper" tooling offered, and it works pretty good. Air-oil mist preferred, .001 stock to leave at MOST, .003 is way too much to leave for a .062 ball, I leave that much for .25 dia balls.

  20. Likes charlie gary liked this post
  21. #18
    Join Date
    Oct 2007
    Country
    UNITED STATES
    State/Province
    California
    Posts
    77
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    23

    Default

    To add to what others have said earlier in this thread, I will suggest adding a re-roughing or rest machining operation(s) with a ball nose tool of the same size-or even slightly smaller-as your finisher. It can be difficult to visualize if you're unfamiliar with this sort of thing, but you can sometimes *think* that you have roughed/semi-finished your part to within the oversize value specified in these operations, but if you are using a larger tool, there is likely quite a bit more stock left in certain areas, and when your finisher sees this it can damage/break your tool quite easily.

    Another thought: some (most?) CAM programs will have toolpath strategies that will automagically employ different strategies for surfaces depending on differences of geometry (constant Z for steep stuff, parallel plane or constant stepover for shallow, etc). In TopSolid this is called their "superfinishing" strategy; I have heard that Fusion has something called "steep and shallow" or something like that. I've gotta think that this is fairly commonplace these days, but what do I know? This might be worth a look, as it can save some programming work. YMMV as they say....

    Good luck & have fun.............Brian

  22. #19
    Join Date
    Oct 2009
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    1,527
    Post Thanks / Like
    Likes (Given)
    1052
    Likes (Received)
    849

    Default

    Some pretty good advice so far related to leave less stock for finish. No more than .001" when using a small cutter like a .0625" ball, light chip load of about .0005" per tooth, a stepover somewhere between .002"-.004", and always climb cut. Going back and forth (climb/conventional) is okay in something like aluminum where the geometry is handwork friendly, but if you don't want to spend time sanding and polishing the extra time spent ensuring every cut is a climb cut is recouped in handwork time. And make sure your coolant flow is more than adequate to flush chips and your concentration is high enough to lubricate things.

  23. #20
    Join Date
    Dec 2004
    Location
    San Antonio, Texas
    Posts
    239
    Post Thanks / Like
    Likes (Given)
    42
    Likes (Received)
    270

    Default

    Quote Originally Posted by EmanuelGoldstein View Post
    I don't s'pose you could tilt the part a little so it's not trying to cut with the center of the ball ? If you look at the photo, on areas that are steeper you don't have that problem ...
    This. If you're perpendicular to the surface the tip of the ballnose will leave marks. Tilt the tool axis so that the cut is taking place further up the ball, not the tip.


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
  •