Calculating surface feet ball nose tooling
Close
Login to Your Account
Results 1 to 8 of 8
  1. #1
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    0

    Default Calculating surface feet ball nose tooling

    Hello. I am a programmer at a forge plant. Our dies are made out of Finkel grade 2(fx2) material. We have been using the same F.R. and rpms for 6-7 years now. My boss is wanting me to optimize our cutting parameters. Do you guys/gals have any suggestions on calculating surface feet and recommended doc/stepover for die steels? Any good resources?

  2. #2
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    530
    Post Thanks / Like
    Likes (Given)
    107
    Likes (Received)
    592

    Default

    Basically your surface feet per minute decreases to zero at the cutting tip. In other words, use the standard formula RPM/3.82 X Cutter Diameter, but instead of the actual cutter diameter, you can approximate the diameter at the actual point of contact of the tool. If you are using the absolute tip, the diameter approaches zero and that is why you will see rubbing and tip degradation. There are some ways around this. First, if you have the opportunity, approach the surface from the bottom rather than the top. This will move the point of contact out from the tip, increasing the SFM. Second, most shops that are doing a bunch of surfacing, use tools other than traditional ball endmills. For instance, any sort of bull endmill. There is also a growing trend to use barrel tools for steep surface and large radius lense tools for shallow surface. These have a twofold advantage of increasing the SFM and increasing the effective radius to produce a finer surface finish with a larger stepover. Mastercam (and I'm sure others) has done a good job of using these new tools in their multiaxis surfacing routines.

    Lastly, when the opportunity presents itself, I like to rotate the part being machined in the A axis by a couple of degrees. This prevents me from machining with the actual tip of the cutter, and pushes the point of contact out towards the major diameter increasing the SFM even on low angle surface. This is free, but only applicable in 4 and 5 axis mill work. On my 3 Axis machines, I tend to use bull endmills. As far as actual feeds and speeds, I can't help you with that material, and stepover is very dependent on the type of toolpath you are running in the cam system (scallop, waterline, parallel....)

  3. Likes mhajicek, primeholy, kazlx liked this post
  4. #3
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    530
    Post Thanks / Like
    Likes (Given)
    107
    Likes (Received)
    592

    Default

    Bad form to respond to my own post, but after I walked away, I got to wondering why the CAM development people have not come up with a way to manipulate the RPMs of the cutter on the fly depending on what portion of a cutter is being used while surfacing. Very similar to how a lathe alters the RPM while facing. It wouldn't be a simple calculation, but it could be done. Especially for applications where you are surfacing hard materials (low SFM) with a high potential RPM spindle... shower thoughts.

  5. Likes primeholy liked this post
  6. #4
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    658
    Post Thanks / Like
    Likes (Given)
    544
    Likes (Received)
    342

    Default

    Quote Originally Posted by G00 Proto View Post
    Bad form to respond to my own post, but after I walked away, I got to wondering why the CAM development people have not come up with a way to manipulate the RPMs of the cutter on the fly depending on what portion of a cutter is being used while surfacing.
    Probably because most surface finishing routines are not stock aware. Might not hurt to send a feature request to Vericut for their toolpath optimization suite; if anyone can do it they can.

  7. #5
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,106
    Post Thanks / Like
    Likes (Given)
    1126
    Likes (Received)
    2259

    Default

    Quote Originally Posted by G00 Proto View Post
    Bad form to respond to my own post, but after I walked away, I got to wondering why the CAM development people have not come up with a way to manipulate the RPMs of the cutter on the fly depending on what portion of a cutter is being used while surfacing. Very similar to how a lathe alters the RPM while facing. It wouldn't be a simple calculation, but it could be done. Especially for applications where you are surfacing hard materials (low SFM) with a high potential RPM spindle... shower thoughts.
    It's not a question for the CAM developers. It's motion control, ladder logic, spindle mechanics. There's a lot more to it than just a code.

    R

  8. #6
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    530
    Post Thanks / Like
    Likes (Given)
    107
    Likes (Received)
    592

    Default

    Quote Originally Posted by litlerob1 View Post
    It's not a question for the CAM developers. It's motion control, ladder logic, spindle mechanics. There's a lot more to it than just a code.

    R
    I'm not sure that I agree (not trying to be argumentative since this is largely an academic question at this point). I think that the spindle speed optimization could be controlled at the cam level based on the SFM at the calculated effective radius of a ball nose endmill. The question that you nailed is could the change in spindle speed keep up with the programmed change in spindle speed. It would be pretty easy on a waterline toolpath, but very difficult on a parallel toolpath where the z (and effective cutter diameter) is constantly changing. I think that it is something that could be done on certain toolpaths. Like I said, "shower thoughts" I gotta admit, I am always amazed by how my turning center alters the RPM based on the effective diameter of the stock, pretty cool if it could do the same thing on mill toolpaths. Then again, I'm pretty simple and a lot of things amaze me... probably as a result of sniffing burnt coolant for too many years>

  9. #7
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,106
    Post Thanks / Like
    Likes (Given)
    1126
    Likes (Received)
    2259

    Default

    I guess you might be right, someone who is not talking out of their ass will chime in on the possibility of CSS on a Milling Operation.

    Theoretically you could do it manually in the program, by doing all the maths and changing the RPM at every elevation change. Line for line, it wouldn't be a huge leap for a CAM developer to add that into the Macro/Variable in the Post Processor. But it would be a huge amount of Data. Even doing it as per the Tool diamter wouldn't be too hard, you wouldn't need to Map the Surface for Elevation. The Toolpath itself would need to be off a Surface or a Net. So the software knew what diameter it would be using. Shit maybe.

    R

  10. #8
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    1,475
    Post Thanks / Like
    Likes (Given)
    50
    Likes (Received)
    535

    Default

    If the magical gremlins know a .02cr tool is using the top of the radius at the top of generating a 1/2” radius and the bottom of the radius at the bottom, I don’t know why the couldn’t say, 12k rpm at the bottom and 10k at the top?

    Disclaimer: those are all completely random numbers


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
  •