I’m trying to rotary a car model again using poplar and being mindful of the pass depth recommendations of my bit. However, my robust hogging 1/4" bit keeps breaking during the first roughing pass! Do I need bigger bits like 1/2" for roughing? I’m reluctant to reduce the pass depth as it’s already 5+ hrs of roughing for initial pass.
Give some more details on DOC, Step Over, tool path direction, Speeds & Feeds. How many flutes on the end mill?
Let’s see your material setup as well. I suspect this has to do with the Z zero/stock setup being incorrect.
Hey @Eric - here’s the material setup…
Ok, I don’t see any “smoking guns” here but a couple of things stick out:
Your feed and speed is slow… you might be cooking the bit and breaking it.
But, if it’s digging into your material more than .25" of an inch (which is what your pass depth is set at) then you have a setup problem.
With the stock removed from your rotary when you go to Z zero is the tip of the bit at the centerline of your rotary? It should be because you have it set that way in your material setup.
When you jog to 7.99 inches is the tip of the bit resting on the highest part of your stock?
What I would do is run this job without any material in it and see if you can observe what is going on here… This seems to be a mis match between how you have zeroed your work VS what is in CAM
I had a rotary project recently and discovered that if I try to take heavy passes with the bit off-center to the rotary axis (like a 2D strategy without rotating), that setup is just not rigid enough. Lots of chatter and digs, and if you’re pushing the bit’s limits, you can easily cross them.
I ended up using Fusion’s “rotary spiral” for roughing - keeping the bit top-center to the rotary (a bit off-axis so the cutting edges are on-axis) and climb cutting so the forces are always towards the chuck and not perpendicular to the rotary axis. With that setup I was able to take pretty heavy cuts with an old 3/4" straight bit I had. One side benefit - chip evacuation is easy because they’re always going the same way.
I also found that Fusion likes to plunge into the stock when roughing, and setting up your lead-in correctly is critical.
I would run .250 DOC, .063 WOC and a chip load of .006. At your 22k rpm that will put your feed rate at 396 ipm, but lighter cut, thicker chip so no rubbing and the heat from the cut will go with the chip so cutter will stay cooler. It also will increase your MMR to 6.24 in^3/min. vs 5 in^3/min with your current numbers. If that sounds like a crazy fast feed rate slow the spindle down and keep the same chip load for a slower feed rate.
Agree with Eric, run it without stock and see if you see something that looks out of place.
Hey Eric -
My bit is sitting at zero and in the center of the rotary:
However, with my project diameter of 7.99, my bit touches the top of the piece around 3.4 (probably more like 3.5 since i’ve already cut some stock off in the first pass). My machine won’t even go up to 7.99" high…it maxes out around 7".
Thoughts?
Trying to get more clarity from @djdelorie regarding speeds/feeds comment…
I’ve never really messed with chip loads before…usually I got with the stock settings when I import the tool database. Correct me if I’m wrong but essentially what you are saying is by decreasing the steopover to .063 (or roughtly 25% vs 80% before) and a faster IPM at a chip load of .006, the bit is moving faster through the stock, yet in thinner deeper passes so less chance of excessive heat buildup?
If you’re talking about my “dig” comment, consider… if you’re milling on the “side” of your stock (i.e. way off center but close to Z=0, mostly using the bit’s edge) and your recipe is for 50% depth of cut, and the bit grabs and digs in… you might for a moment be cutting at 60-70% DoC and overloading the bit.
This is made worse by the fact that both the flexibility of your stock and the “twistability” of the avid gantry means that this cut is the worst for rigidity.
Chip load is simply how big a bite each cutting edge (tooth/flute) takes every time it passes through the material or for each rpm of that cutting edge (for an end mill). With a .0015" chip load the cutting edge is taking a very thin cutting, and because of that it could very well just rub and not cut, which generates heat. Chips will and should carry heat away from the cutter and material. You want chips and not dust. Reducing the .200" WOC (width of cut or stepover) to .063" you are reducing the side loading on the cutter, which somehow you have an excessive amount now because you are breaking cutters.
It’s not the faster IPM feed, it’s the chip load that matters, which just happens to equal the faster feed rate. If the 396 IPM seems scary fast, slow the spindle down to 12k rpm and that would give you 216 IPM feed rate.
I will add that chip load is only half of the problem - you need to get those chips out of the flutes and out of the way, too. Make sure there’s an ejection path and/or air jets or good dust collection to make sure those chips don’t stay in the cut and get jammed into the bit. That would be instant breakage.
I do have dust collection, but not for the rotary. I’m reluctant to run dust collection for several hours on end. What kind of air jets would you suggest?
I bolted one of these onto my carriage:
https://www.amazon.com/dp/B07JVKBS4V
but I had an air manifold there already and still needed to 3D print a custom bracket for it. Then I took it off because I’m designing something different…
(I didn’t use the coolant part, just the loc-line and air inputs)
Also, the rotary-spiral pattern always seems to have good chip ejection. So much so I ended up putting a board there to keep them in one place.
You have your pass depth at .25" From the looks of your pictures your first pass it’s way deeper than .25" which is likely what snapped that bit. If that’s true you need to figure out why that happened
Nice! Do you have a pic of your setup?
That’s a rig! Thanks for sharing!