3D surfacing input/suggestion - Page 2
Close
Login to Your Account
Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 44
  1. #21
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    1,311
    Post Thanks / Like
    Likes (Given)
    552
    Likes (Received)
    761

    Default

    A quick click of "contact areas only" turns this

    screenshot-205-.jpg

    into this

    screenshot-204-.jpg

    I seem to remember fusion having a similar option. A direct link at an increased feed rate would likely save a lot of time as it looks to me like around 50% of that is air.

    While I agree sometimes cutting air is faster, I've found it rarely is when taking fine stepovers surfacing. Besides it's good practice for when you need to program that way.

  2. Likes mhajicek liked this post
  3. #22
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    1,381
    Post Thanks / Like
    Likes (Given)
    1791
    Likes (Received)
    924

    Default

    Quote Originally Posted by Mike1974 View Post
    Maybe, maybe not. Sometimes saving programming time can justify the air cutting. Or depending on processing power of machine and cam, could take longer/the same even though less cutting moves if the machine is jerking around "dodging" () the pocket areas.
    If you're using a proper CAM system, just put a flowline or parallel on the top surface of the model; easy peasy. It would take longer to program to waste time over the holes.

  4. #23
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,067
    Post Thanks / Like
    Likes (Given)
    255
    Likes (Received)
    709

    Default

    When I cut this part (for those that don't know this is one of the Titan building blocks lessons) I tried it with a ball and a corner radius end mill and the difference was night and day. The high SFM using the outside of the bullnose tool gave MUCH better surface finish.

    Also play with smoothing in your software.

  5. Likes hanermo, Djstorm100 liked this post
  6. #24
    Join Date
    Jul 2014
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    316
    Post Thanks / Like
    Likes (Given)
    120
    Likes (Received)
    31

    Default

    Quote Originally Posted by Rick Finsta View Post
    When I cut this part (for those that don't know this is one of the Titan building blocks lessons) I tried it with a ball and a corner radius end mill and the difference was night and day. The high SFM using the outside of the bullnose tool gave MUCH better surface finish.

    Also play with smoothing in your software.
    Rick, What speed and feeds did you use for the 3d portion I'm curious if my F&S are in line with yours.

  7. #25
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,067
    Post Thanks / Like
    Likes (Given)
    255
    Likes (Received)
    709

    Default

    I cut it on my old mill, so I would have been running a maximum of 8000rpm and I used a 1/2" bull nose with a 0.030" corner radius. I had to limit chipload only because of the block processing speed of the machine, and even then I got some dwell marks and over/under cutting. I honestly don't recall the feed rate but I know that machine couldn't handle more than about 120IPM before it started to run into serious accel/decel problems.

    With my new Okuma I'd run a Helical 1/2" 3-flute 0.030-0.060" radius bull nose with their ZrN coating at 15000 rpm and around 0.003"-0.005" chip per tooth and I'd semi-finish then finish leaving around 0.002-0.005" radial/axial for the finish pass. I use that same tool family for some 3D surfacing of some Subaru fuel rails I'm developing for a local company in areas where a 3/8" ball can't get into small radii.

    Hope that helps.

  8. Likes TeachMePlease liked this post
  9. #26
    Join Date
    Nov 2017
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    33
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    20

    Default

    My 2 cents: I make Aluminum Injection Molds, So I surface 7075 all the time.
    for this Titan part I would use the largest tool I can with a large corner radius, not a ball end mill
    In my arsenal I would run my 1.5" index-able 3 flute with .125 radii inserts
    So I could get it done, and because it is aluminum, max rpm for me that is only 10k
    feed 60-100 ipm if you want a mirror 40ipm
    with a cutter this big doesnt matter if .008-.001 rest material
    sub .01 step over for a mirror
    if this was a mold surface and I had to blend other wall areas so I had to use a ball endmill use the largest one you can use, fastest rpm I have available
    and 40ipm feed
    rest material .001-.003
    step over .003
    choice in ball end mill, a 2 flute ball end mill has a full radius, a 4 flute ball has a full radius on 2 flutes, so effectively at the tip still only 2 flutes,
    a 3 flute usually has only 1 flute past center, avoid these for surfacing, they are weaker.

    dont retract over the holes or any where possible, stay down, try to never retract during surfacing.

    here is one of my Aluminum Molds with surfacing.

    https://p.widencdn.net/bfkgfw/Harvey...tions_MoldTool

  10. #27
    Join Date
    Nov 2017
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    33
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    20

    Default

    Actually just for kicks, and because Op is learning, with the Titan part, here is a little machining analysis.
    if this is a one off, you use what you have.
    if this is a production part, that will return, and you make a few $$ from it, so you can buy tooling for optimum speed, then you start looking at selection of cutter.
    you want to get it done as fast as possible, but with the surface ridge height at or below the customers requirement.
    cutter parameters:
    -the larger the radii on the corners of the cutter the faster you can feed it.
    -the larger the diameter of the cutter the larger you can step over.
    -the larger the diameter of the cutter the higher SFM you can achieve for a given rpm
    -the more cutting edges you have the faster you can feed it.
    -the part is aluminum so it has to have non-ferrous cutter geometry, or at least a fairly sharp geometry cutter

    with all this I would say the fastest tool that would leave the lowest ridge height would be a toroid face mill with button inserts
    and the larger the diameter and the larger the insert, the better.

    Dapra has some toroid button cutter from 3"-8" Diameters and inserts from 3/8"-3/4"
    In a VF2SS a 3" toroid button cutter with 3/4" inserts would make quick work.

    Single-Sided Toroid Cutters & Inserts Page 1

  11. Likes aarongough liked this post
  12. #28
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    58
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    12

    Default

    3/8 ball 2 flute, 700-750 sfm .0045 step over for starters with .005-.007 cpt.

  13. #29
    Join Date
    Jul 2014
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    316
    Post Thanks / Like
    Likes (Given)
    120
    Likes (Received)
    31

    Default

    Thanks guys. I ran the part with 1/2 diam, 3 flute, 0.125 CR at 0.01 step over. 8,000 rpm at 183ipm. I made two other parts to try other speed and feeds.

    comparing ball nose and bull.



    img_0534.jpg

    img_0533.jpg

  14. Likes aarongough liked this post
  15. #30
    Join Date
    Oct 2014
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1,523
    Post Thanks / Like
    Likes (Given)
    1095
    Likes (Received)
    1279

    Default

    Big improvement! Looks great!

  16. Likes Djstorm100 liked this post
  17. #31
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    1,311
    Post Thanks / Like
    Likes (Given)
    552
    Likes (Received)
    761

    Default

    Looks like your chamfers need some attention

  18. Likes aarongough liked this post
  19. #32
    Join Date
    Apr 2006
    Location
    Ga.
    Posts
    138
    Post Thanks / Like
    Likes (Given)
    16
    Likes (Received)
    13

    Default

    Can you fixture them so you can use a long endmill to just side cut those surfaces? 2-3 finish passes and they would look like glass.

  20. #33
    Join Date
    Jul 2014
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    316
    Post Thanks / Like
    Likes (Given)
    120
    Likes (Received)
    31

    Default

    Quote Originally Posted by Hardplates View Post
    Looks like your chamfers need some attention
    Finish pass for the triangle needs slowed down.


    Sent from my iPhone using Tapatalk

  21. #34
    Join Date
    Jul 2014
    Country
    UNITED STATES
    State/Province
    Virginia
    Posts
    316
    Post Thanks / Like
    Likes (Given)
    120
    Likes (Received)
    31

    Default

    Quote Originally Posted by aarongough View Post
    Big improvement! Looks great!
    Thanks!!


    Sent from my iPhone using Tapatalk

  22. #35
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    1,311
    Post Thanks / Like
    Likes (Given)
    552
    Likes (Received)
    761

    Default

    Quote Originally Posted by Djstorm100 View Post
    Finish pass for the triangle needs slowed down.


    Sent from my iPhone using Tapatalk
    Have you tried playing around with G187? I think that is Haas's version of G8, G5 exc

  23. #36
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    780
    Post Thanks / Like
    Likes (Given)
    182
    Likes (Received)
    902

    Default

    A couple opinions to throw out there:

    I generally don't retract over pockets when I am surfacing. On my machines, it takes longer to come up, go over and feed back down than to just feed across. Additionally, I feel that I get an artifact in the surface finish everywhere it Z moves. Not a big deal if you can cheat the edgebreak up a bit. Even so, I generally create a model that has no pockets and create my code off of that.

    As mentioned above, there are some "new" circle segment cutters available for just this type of part. A lense shaped cutter is basically a very large diameter ball endmill that has been ground to leave the ball and reduce the diameter to a manageable size. For instance, a 1/2" diameter cutter with a 3" diameter ball radius. These work very well on large low angle surfaces. [A barrel shaped cutter is analogous in that the circle segment is on the side of the endmill... these work very well for steep walled surfacing, like a tapered wall on a mold). These overcome some of the limitations of a ball endmill.

    That being said, on a onesy twosy part like this I would just grab a generous radius bull nose endmill and let her rip. Speed is only limited by the processing power and ACC_DEC characteristics of your machine. That can range from 50 IPM to several hundred IPM. I also run surfaced parts differently depending on the lifecycle of the part. For instance, a part that is going to get tumbled and then anodized gets machined differently than an injection mold that goes straight to the customer with minimal or no polishing... I'm in this to make money, not to make the shiniest part

  24. #37
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    5,541
    Post Thanks / Like
    Likes (Given)
    2198
    Likes (Received)
    2747

    Default

    Quote Originally Posted by Hardplates View Post
    Have you tried playing around with G187? I think that is Haas's version of G8, G5 exc
    Good idea! It can be changed at the control, but I would add it into the code

    G187 P3 E.005 (or whatever, experiment for best compromise of speed/quality)

    It will run slower, but *should* be more accurate, better finish. At the end of the surfacing, just add a G187 to reset to factory specs (ours all default to medium with E of .015 I think).

  25. #38
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,067
    Post Thanks / Like
    Likes (Given)
    255
    Likes (Received)
    709

    Default

    Quote Originally Posted by G00 Proto View Post
    A couple opinions to throw out there:

    I generally don't retract over pockets when I am surfacing. On my machines, it takes longer to come up, go over and feed back down than to just feed across. Additionally, I feel that I get an artifact in the surface finish everywhere it Z moves. Not a big deal if you can cheat the edgebreak up a bit. Even so, I generally create a model that has no pockets and create my code off of that.
    IIRC this is how the Titan Academy teaches it. Fusion 360 has a surface workspace with a patch command. This places surface patches over the holes that the 3D toolpaths will "see" when calculating and not violate. So in the model being cut, it should be a flat plane with the curves on the ends.

  26. #39
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    1,311
    Post Thanks / Like
    Likes (Given)
    552
    Likes (Received)
    761

    Default

    I would not retract either but I would feed as fast as I could on a point to point linking move. I'd program something like 1600 ipm and let G8, G5 blah blah blah determine just how fast the machine can link. I have my contour control set to complete decel on the preceding block as well as programing in a couple thousands feed before reengagement.

    There is absolutely ZERO difference in surface finish vs running engagement feed over patches. But there is a large time difference.
    Attached Thumbnails Attached Thumbnails screenshot-216-.jpg  

  27. Likes mhajicek liked this post
  28. #40
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    1,067
    Post Thanks / Like
    Likes (Given)
    255
    Likes (Received)
    709

    Default

    I bet in a Speedio you'd see a huge difference on something like this with an ISOgrid if you could use high linking feeds across the hole features. I'm not sure other machines (other than linear motor) would have the accel/decel to make much difference versus just staying at the feed rate.


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
  •