506,071 active members
3,693 visitors online
Register for free
Results 1 to 8 of 8
  1. #1

    Fusion slotting

    How do I remove the ramping in and out and just do a clear stepdown.?? I made my toolpath 6x as long as my hard coded program. I'm very new to fusion.

    I am the only one with a machining background. So I hard code everything the owner bought me a Haas and said buy what ever you need. Almost everything is basic drilling and milling paths so I just hardcode it. I've made fixtures and all sorts of stuff so far with no cam software. But I would like to get into more advanced fixturing and such.

    I just need to slap to 13/16 slots in .450 material 1.5 inches in and .075 step down. Full WOC. 13/16 endmill. Fusion took a 1:12 second toolpath and turned It into 6 minutes.

    I currently work in a glass manufacturer where we do all aluminum extrusions.

    I am able to draw in Inventor and AutoCAD.

    Sent from my SM-G950U using Tapatalk

  2. #2

    Re: Fusion slotting

    I think you can uncheck ramping in the operation setup. On my Haas, I would use a smaller end mill, maybe 1/2 or 5/8 inch and do a adaptive clearing pass at full depth, 6000 RPM, 120 IPM, full DOC, about 0.035 step over, aluminum cutting carbide endmill.

    Then a final profile clean up of about 0.005. 6000 RPM, 80 IPM, full DOC

    To learn Fusion 360, I would recommend https://academy.titansofcnc.com/ a free online course that takes you from 0 to machining parts in a couple of days. Uses Fusion 360 and Haas machines.
    Jim Dawson
    Sandy, Oregon, USA

  3. #3
    Join Date
    Jan 2018

    Re: Fusion slotting

    I'm not a fan of plunging straight in.
    In my program it's using the 'multiple depths' setting that slows it down a lot.
    I use 'ramping' but I increase the angle setting and that makes it quicker, still less aggressive than a straight stepdown.

  4. #4
    Join Date
    May 2015

    Re: Fusion slotting

    Don't plunge straight in, instead, change the ramp type to helix (IIRC it's the default for adaptive paths anyway) and it will ramp into the guts of the cut in a spiral, then work its way out. You can adjust the thickness of each pass. Using the full depth means even wear on the cutter, faster cutting and a cleaner finish.

  5. #5

    Re: Fusion slotting

    Surface finish isn't important where I work guys. Basically it's full send all the time because these are small hidden parts for high rise window assemblies.

    I clear the part every step down and take
    .075 passes
    at 2250 rpm
    29 ipm
    Hs Cobalt 4 flute .8125 flat

    Sounds buttery smooth. Rapid to the other side and start chewing. I was just wondering if fusion could speed this up any more a 4 part cycle is a little over 2 minutes.

    I was just trying to eliminate the ramp and have the cutter step of the side of the part half the radius of the tool + .100

    Do you think a 1/2 cutter or even a 3/8 cutter could keep up in an adaptive clear with a full WOC 13/16?

    The owner is fine with supper agressive cuts and drill cycles. We pay like 2-5 dollars for are TiCn drills some of which I've hit through holes in up to 1/2 material with no peck at almost 5k holes. The 7/16 I've had in there almost 4 months.

    and tolerances are basically non existent.

    The only time you change a tool is when it's completely shot.

    Basically I need fusion to machine more agressive than me but not snap tools off or chip weld them.

    I'm looking for a better option at this point the owner has no clue what I do and openly says what your saying is all Greek to me.

    Sent from my SM-G950U using Tapatalk

  6. #6

    Re: Fusion slotting

    You're only going 0.450 deep, so do it in 1 pass. But use a 3 flute aluminum cutting carbide rougher end mill, and pour on the coolant. I would use a 1/2 or 5/8 end mill and just do 1 profile pass since the tolerance is not important. Max out the spindle speed which I assume is 6000 on your machine. Start at about 120 IPM, and then bump it up until the spindle load is in the 95% range.

    Adaptive clearing is a little slower but easier on the tool, but you can bump up the feed to compensate. We would normally run your parts with a 5/8 rougher.

    Here is a good video illustrating adaptive clearing and feeds & speeds.

    Jim Dawson
    Sandy, Oregon, USA

  7. #7
    Join Date
    Jan 2018

    Re: Fusion slotting

    I'd prob go:
    1. Ramp unchecked,
    2. Multiple depths set the same height as your full cut depth,
    3. Plunge outside stock.

  8. #8
    Join Date
    Oct 2010

    Re: Fusion slotting

    If you have lots of these to make, why not make some sort of palletized tooling that holds 20-30 parts, and you can be loading one pallet while the other one is being run?

    Most efficient production does not always mean taking the last few seconds out of a toolpath.


Similar Threads

  1. Help slotting 304 SS.
    By AP71 in forum Machinist Hangout
    Replies: 4
    Last Post: 01-17-2015, 04:01 PM
  2. Slotting in VM 6.0 NOT
    By UniqueMachining in forum Visual Mill
    Replies: 4
    Last Post: 09-16-2013, 05:16 PM
  3. Slotting MDF
    By Me2 in forum General Material Machining Solutions
    Replies: 2
    Last Post: 07-28-2007, 05:25 AM
  4. Slotting for CNC
    By Kavanthony in forum Uncategorised MetalWorking Machines
    Replies: 3
    Last Post: 04-04-2007, 10:20 AM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts