Fusion360 settings for rouging and finishing passes...

Discussion in 'Luthier's Corner' started by fretman_2, Mar 8, 2018.

  1. fretman_2

    fretman_2 Senior Member

    Messages:
    915
    Likes Received:
    558
    Joined:
    Apr 7, 2013
    I could have probably PM'd a couple of folks about this, but I chose to put it in a thread so it could be searched later by someone seeking the same info.

    I plan to use a 1/4" ball nose bit to profile a test neck in pine. I've hacked at producing a neck in Fusion360 and this is the result.

    [​IMG]

    Any guidance or suggested settings for roughing and finishing passes in Fusion360?
     
  2. pshupe

    pshupe Senior Member

    Messages:
    3,385
    Likes Received:
    2,201
    Joined:
    Jan 19, 2012
    I would use a 1/2" ballnose, unless your machine cannot take that width of a bit. The though is that the larger radius gets closer to the shape. The step over would be similar though, but quite small for that size bit. It may take about the same size as the 1/4" bit but should be a smoother final product. roughing would be 1/2" bit with a much larger step down and step over then finishing with a 1/2" with about a 10% stepover. Let me know if you want the exact numbers. With this type of machining I still revert back to my old 3d cutting software, so I have not cut a neck with Fusion yet. I have to kick myself in the butt soon though and switch everything to Fusion 360. Good luck.

    Cheers Peter.
     
    stonedmoses likes this.
  3. fretman_2

    fretman_2 Senior Member

    Messages:
    915
    Likes Received:
    558
    Joined:
    Apr 7, 2013
    Yea...that's the issue Peter...I can only accommodate 1/4" shanks in my spindle.

    Please give me your exact numbers...maybe I can extrapolate from a 1/2" bit.

     
  4. stonedmoses

    stonedmoses Member

    Messages:
    32
    Likes Received:
    13
    Joined:
    Apr 22, 2011
    I'm working with Fusion at the moment.
    I'm focused on carving a top for a LP-esque guitar but I gave my neck-skills also a try with not that much success yet...

    I would also take a 1/2 ballnose for both the roughing and the finishing... 1/4" should also work but the result takes a bit longer and the setting for stepover etc is a bit different...

    Another thing I'd try to smooth is the neck-headstock transition. Don't know if that is your final transition but I think the end result would be pretty edgy... hope that makes sense...
     

    Attached Files:

  5. fretman_2

    fretman_2 Senior Member

    Messages:
    915
    Likes Received:
    558
    Joined:
    Apr 7, 2013
    Yea...it's edgy. I'll make another stab at having a better transition. If nothing else, I can take care of the transitions with a scraper. I'm primarily interested in the profile.

     
    stonedmoses likes this.
  6. pshupe

    pshupe Senior Member

    Messages:
    3,385
    Likes Received:
    2,201
    Joined:
    Jan 19, 2012
    There’s not much to it, if you are using a 1/4” bit just use the standard cutting parameters you normally use for that bit. I get my bits from tools today and they send me speeds and feeds for their bits. I can check speeds, feeds and doc for my 1/4” bits when I get home.

    I usually doc at 1/2 the bit diameter. Rule of thumb for size vs speed and feed is the larger the bit the slower the speed (rpm) and faster feed (ipm). So a 1/4” bit I’d run about 1/8” doc per pass, 80 - 100 ipm, and 18,000rpm or so.

    I max out my tiny bits on rpm at 24k and run them slow 30 - 40 ipm. My 1/2” I can run at 10k and 120 ipm.

    There is a formula that relates to chip load to get these numbers. The numbers above are for 2 flute bits. Because it relates to chip load if I use a 3 flute, I would increase my feed rate by 50%. You want to cut fast enough, feed, through the wood to not burn and heat the bit but slow enough not to put too much lateral pressure on the bit to break it. Tools today suggest a medium high rpm for all there bits and adjust feed rate to suit the chip load calculations.

    I’m no expert. This is just my understanding. I’ve only broken two or three bits and every one of them was from user error. I jogged two into something and pushing something into a bit the other time.

    Regards Peter.
     
  7. cmjohnson

    cmjohnson Senior Member

    Messages:
    1,632
    Likes Received:
    1,084
    Joined:
    Dec 13, 2012
    It is definitely possible to obtain a 1/2" ball nose bit with a 1/4" shank. You just have to do a little searching to find it.
     
  8. fretman_2

    fretman_2 Senior Member

    Messages:
    915
    Likes Received:
    558
    Joined:
    Apr 7, 2013
    Definitely something to look into...thanks!

     
  9. fretman_2

    fretman_2 Senior Member

    Messages:
    915
    Likes Received:
    558
    Joined:
    Apr 7, 2013
    What percent stepover do you use for the finishing pass based on your 1/2" bit?

     
  10. pshupe

    pshupe Senior Member

    Messages:
    3,385
    Likes Received:
    2,201
    Joined:
    Jan 19, 2012
    10%
     
  11. Tweaker

    Tweaker Senior Member

    Messages:
    2,491
    Likes Received:
    1,572
    Joined:
    Jan 18, 2012
    I've done a lot of work with Fusion 360...lots of uke necks. My machine isn't that great...stalls out on occasion, quite a bit of slop in the machine itself, etc, so I've experimented with the finishing stepover just to see what works. Everything from 50% to less than 5%. You're always going to have to sand the neck once it's off the machine, so to be completely honest, I'd choose a stepover that gives you a machining time you like. If you can sand quickly and accurately, a higher stepover is fine. To some it might defeat the purpose of using CNC, but I use CNC to more or less do the rough shaping and I fine tune by hand.

    If you're honed in on doing as little sanding as possible, also try messing around with the finishing angle. Certain angles provide less machined ridges in certain spots on the neck. For example, I just cut a neck with a heel for a uke a couple days ago. Oriented the neck longways in the Y direction. When I did my finish op in the same direction, I had huge ridges on the heel. Would have been a good candidate for a 90* pass angle. The difficulty there is that if your neck is one body, you won't be able to pull that off. You'd have to split the body and then do a separate finish op with the desired pass angle.

    Feel free to PM me any time if you'd like.

    EDIT: For what it's worth, I have a ball cutter and a flat cutter, both 1/2" with a 1/4" shank. They work wonderfully. My spindle bearings complain horribly if I cut at an RPM below 16k, and my feedrate is around 80ipm. 0.8kw spindle...definitely has it's limitations.
     
  12. pshupe

    pshupe Senior Member

    Messages:
    3,385
    Likes Received:
    2,201
    Joined:
    Jan 19, 2012
    Here is the feeds and speeds recommendation from Tools Today for their 1/4" bit -

    46250: 1/4” diameter – 1 1/8” DOC – solid wood – up cut – 2 flute
    100" IPM @ 18,000 RPM
    Chip Load Per Tooth: 0.0028"
    Depth Per Pass: 1/4"

    Note: - I usually do not cut full width of bit. I would normally cut 1/8". Now having said that if you use Fusion 360 you can do full DOC cutting using a "scalloping method", which means it spirals down into the material and then cuts scallops at the step over for the whole depth of the cutter. I have yet to try this but I think this is the way to go as it uses the full length of the cutter and not always just the last 1/8", as in the depth per pass as noted.

    Here is the speeds and feeds chart that I use if I deviate from the above recommendation. Also this is what I went by before getting the Tools Today recommendation. The formulas are helpful if you want to run at different feeds and feed rates.

    chipload.JPG ]

    Cheers Peter
     
    Tweaker likes this.
  13. Tweaker

    Tweaker Senior Member

    Messages:
    2,491
    Likes Received:
    1,572
    Joined:
    Jan 18, 2012
    Adaptive Clearing will do that "scalloping" method. I've done it full depth on some pockets with a very small step over and it works well. Guys who machine aluminum and steel use it very frequently.
     
    stonedmoses and pshupe like this.
  14. pshupe

    pshupe Senior Member

    Messages:
    3,385
    Likes Received:
    2,201
    Joined:
    Jan 19, 2012
    That's the term I was trying to think of when replying. I have yet to try it but will try and use it soon.

    Cheers Peter.
     
    Tweaker likes this.
  15. fretman_2

    fretman_2 Senior Member

    Messages:
    915
    Likes Received:
    558
    Joined:
    Apr 7, 2013
    Awesome info all...thanks very much! I'm going to dig back into F360 this week and ponder all of the above.
     
  16. Tweaker

    Tweaker Senior Member

    Messages:
    2,491
    Likes Received:
    1,572
    Joined:
    Jan 18, 2012
    It takes forever on my machine because it isn't very robust and the spindle is weak so my step over is tint...0.5mm or less. On a machine like yours, I would think you could get away with a bit bigger step over (maybe 2-3mm depending on wood species?) and it would be a much faster operation.
     
  17. fretman_2

    fretman_2 Senior Member

    Messages:
    915
    Likes Received:
    558
    Joined:
    Apr 7, 2013
    OK...that's good to know. It's like Peter said...I won't ever get it to the point of not needing sanding, but I want to get it as close as possible.

     
  18. pshupe

    pshupe Senior Member

    Messages:
    3,385
    Likes Received:
    2,201
    Joined:
    Jan 19, 2012
    I just did a 25' radius sanding dish that was 22"x22" and I had a 10% stepover on a 1/2" ballnose and I do not need sanding but it took over 1 hr to finish. You can get it so you do not need sanding but it would take so much longer it's not worth the time. Probably a 10% rule. It may take me 5 minutes to sand out something that would take me an extra 50 minutes with the CNC.

    Cheers Peter.
     
  19. fretman_2

    fretman_2 Senior Member

    Messages:
    915
    Likes Received:
    558
    Joined:
    Apr 7, 2013
    It's difficult to know when to CNC and when to sand until you've done a few projects. Some of these aluminum projects take me an hour or more because I have such a conservative feed and depth of cut. But I don't mind really as the last thing I want to do is break a bit. Cool on the 10% stepover on the 1/2" ball nose bit. I'm going to do just a portion of the profile and see how that comes out. Much quicker than doing a whole test neck.

     
    Tweaker likes this.
  20. Tweaker

    Tweaker Senior Member

    Messages:
    2,491
    Likes Received:
    1,572
    Joined:
    Jan 18, 2012
    My rule of thumb for CNC vs sanding is...if I have another job to do that the CNC can't do (hammering frets, drilling holes on angled headstock, etc.) that I know will take a while, I'll program the CNC to do a finer stepover, since I have time to kill anyways. If I just want to get it off the machine because I don't have any other pressing tasks, I'll use a bigger stepover and do more sanding.

    I used to sand by hand, no orbital sander...I definitely had the CNC do more of the work! Then I finally bought a cheap Ryobi random orbital palm sander...I can knock off the ridges left from the machine and sand up through 400 in about 5-10 minutes. Love that sander.
     

Share This Page