Hey guys, Ive had my MR1 for about a year now and have milled around 500 knife bevels with it using coated 6 flute bullnose end mills. This is a relatively basic thing to mill and doesn’t take much off and Ive had a lot of success with this setup.
Now I am starting to mill out putters and it is a whole different ball game. I am milling 1.5" 1018 square stock and Im fairly inexperienced with hogging off a lot in a project. First thing I learned was a 6 flute was a bad idea for this. It just rubs the hell out of it until starts squealing on only the second putter. So now I have two 4 flutes that came in the mail. I will run the mill to match the feed and speeds they recommend… but what about stepover and stepdown. Ive read stepdown is more of a testament to how much power a spindle has but Im not sure how that translates to our machines compared to a traditional mill. Right now I have it programmed for .005 stepover and .375 stepdown. Takes about 2.5" hours mill out the body of the putter minus the face (including a flow toolpath to clean things up)
Does this seem like its in the right ballpark?
Here is a pic of the one I just finished for reference.
If it were me doing this production work, I would rough the whole thing with a roughing end mill (corn cob) either 1/4” diameter or 3/8”. Any bigger than that on a steel and you start losing roughing efficiency. Then swap in a good sharp finisher for all the finish passes.
For a 1/4 end mill I would run that at 8000 rpm, .150 depth, .03 step over, and 30-50 inches per minute.
.005 stepover is really small, what is your feed per tooth? I think you are still going to be rubbing endmills with that shallow of a cut (but I can’t compute that without knowing feed rate and spindle RPM). There are places for fine cuts like that, but it is on finish passes and not roughing.
Lakeshores chart says .002 so thats where I have it set. I am running 7200rpm and 57ipm. on a fun not it seems my spindle bearings just ate shit so I need to get ahold of Langmuir
This is a decent article explaining how all of it fits together:
FSWizard is a free tool that can help you figure out starting points and see how the pieces fit together. Their defaults are tuned more for higher power and more rigid machines, so I normally back off on Fz and spindle speed a little bit (about 70% of their recommendations). Don’t forget that Langmuir also publishes recommended settings.
No i understand the feed per tooth. My setup is running .002 feed per tooth. I just didnt think a bigger bite like .015 stepover at a stepdown like 3/8" would be okay for these machines.
I have tried a stepover at .015 and it seemed to struggle. Granted my spindle bearings just went out so Im not sure if that has anything to do with it.
I just looked at the langmuir chart you mentioned. Pretty cut and dry there lol. Now that Im thinking about it I know I have this damn chart in the toolbox🤦🏼♂️
I notice that a 1/4" is about the max stepdown but its a a pretty signifcant difference in stepover.
Off topic in terms of fixing your problem, but I’m looking to make my own putter too. (You mentioned “putters” - are you making a business out of them? Gotta give you credit if you are. Seems like a ton of work for the return.)
At any rate, how are you fixturing the stock to be able to get the bottom rocker and backside pockets too?
Did you add slots or pockets for tungsten inserts so you can play with different weighting?
Yeah I’ll be building a business from it. So, like most putter makers I am milling them face down. Adaptive clearing for almost all of it and flow with a ball nose for finishing. I go ahead and engrave the logo in the pocket at this point as well. Then i just flip the stock over and face mill what was left, followed by a parallel to do the 3-4 degree loft and I will mill in whatever texture on the face.
Its less work than what my actual job is. Ive owned and ran a production knife company for going on 10 years.
I think the hardest part of putters is the artistic side.
I didn’t add the pockets for weights on this one but I do have a couple other designs coming up that will them
Off the top of my head, I believe you could develop a strategy that would successfully cut that runtime down to 1 hour or less compared to the 2.5 hour time mentioned previously.
Is your adaptive clearing toolpath all one operation inside fusion? In my experience, you can shave off a lot more time than you’d think by creating 3 or 4 different toolpaths that isolate certain features. 90% of the results are just keeping the tool focused in each particular area as it cuts. Apologies if I’m just stating the obvious here.
If you go with a 3/8 endmill, you may check out a .03" or .015" corner radius bullnose. 4 flutes should be just fine- just try to get your length of cut as close to your deepest Z dimension on the part. I wouldnt run anything less than a .03" stepover for 3/8" diameter. You ought to be able to run that tool across half a dozen parts at 3600 rpm and 45 ipm no problem.
Hope I managed to help somewhere in there. Good luck!
I forgot to mention step down. At .03" stepover, you should be able to keep up those speeds and feeds even at a 1"-1.25" length of cut. I wouldn’t do multiple depths on your roughing unless you have deeper cuts than 1.25".
Holy crap. I didnt think it could do that. I will give it a go. Right now Im trying to figure out how to install everything on top the new spindle version.
This morning I am going to give your feed and speeds a go. As for the toolpathing I shouldve been more clear. Im running a 2d adaptive to get the contour. Then using a 3d adaptive to all the inner roughing of the putter. Followed by a flow path with a ball nose to clean up a couple curved parts.
Though I am certain my toolpathing could be done much better. I am self taught over years of cnc routing knife handles. So real metal milling is pretty foreign to me.
Also my old spindle must have been very bad from the get go because if I ever tried to take a bite as big as what you are saying it can do, it would sound like the mill was going to self detonate. It s also I would guess 3 times quieter during the spindle break in program.
I have to be doing something wrong cause it just just starts screaming at those settings. Really high pitched squealing with a brand new end mill.
EDIT
it was apparently how I had it in the vice, cause i took a piece of cork and stuck in between the parallels under the steel block and it shut up immediately.
All seems in order now, though a .02 stepover at .25 deep seems to be a comfortable spot for it. Much more than that either way and it sounds like its really straining the machine.
At some point I need to bring in a real machinist to optimize my designs and figure out finishing passes so im not doing so much work after milling.
