What's new
What's new

How to Purposely Leave Grooves Using Face Mill/Fly Cutter

sdinzy

Aluminum
Joined
Dec 21, 2019
Hi Guys,

This is for a golf putter application. I've got a Kennametal Mill 1-10, 90* inserts with a 0.007" corner radius. Been playing around with different feeds and speeds, trying to leave grooves in the 0.005"-0.010" deep range, about 0.020" apart. I'm currently testing with only one insert on the face mill to make things simpler. I've tried various spindle speeds from 450-900, with corresponding feed rates of 12.3975ipm to 24.795ipm, with DOC's from 0.005" to 0.050". The best I can do is leave visible marks in the pattern I want, but nothing deep enough to feel. Effectively, the face mill is doing exactly what it's supposed to, just not what I want it to do. Currently testing on 6061 with MQL, but end application will be 316 and 11L17 (leaded low-carbon steel). Any advice from experience would be greatly appreciated! I've attached a picture of the desired end result, plus the insert specs. I haven't gone the fly cutter route yet, as these inserts seem to be pretty dang close to what I'd make for a fly cutter anyways (which would be totally new territory for me).

IMG_9243.jpginsert specs.jpg33105.jpg
 
Is the face mill large enough diameter to make it across the full face with the "leading edge" before the trailing edge comes across and wipes away your work?
 
Use an engraving tool.
Personally I don't understand the fascination with this new fad of leaving machine marks on golf clubs.
 
Hi Guys,

This is for a golf putter application. I've got a Kennametal Mill 1-10, 90* inserts with a 0.007" corner radius. Been playing around with different feeds and speeds, trying to leave grooves in the 0.005"-0.010" deep range, about 0.020" apart. I'm currently testing with only one insert on the face mill to make things simpler. I've tried various spindle speeds from 450-900, with corresponding feed rates of 12.3975ipm to 24.795ipm, with DOC's from 0.005" to 0.050". The best I can do is leave visible marks in the pattern I want, but nothing deep enough to feel. Effectively, the face mill is doing exactly what it's supposed to, just not what I want it to do. Currently testing on 6061 with MQL, but end application will be 316 and 11L17 (leaded low-carbon steel). Any advice from experience would be greatly appreciated! I've attached a picture of the desired end result, plus the insert specs. I haven't gone the fly cutter route yet, as these inserts seem to be pretty dang close to what I'd make for a fly cutter anyways (which would be totally new territory for me).

View attachment 283755View attachment 283753View attachment 283754

I've done it before but not intentionally. Just forget to put a G01 after a G00 and you'll have your pretty little swirly marks. To make it easier take all but 1 insert out after facing.
 
Use an engraving tool.
Personally I don't understand the fascination with this new?? fad of leaving machine marks on golf clubs.

I have a scotty cameron putter ca. 2000's that has very much what OP shows in the pick, not exactly the same, but you want some roughness on the face.

OP, you will not get what you want with a face mill (the large/deep grooves), but if you run the feed fast and rpm slow you will get some roughness on the face.
 
I don’t believe there will be a way to make a consistent pattern (as in your example photo) with a face mill unless you can synchronize the spindle with table travel/position.

Is machining in the pattern with a ball end mill out of the question?

PM
 
Fly cutter set to diameter...

Locate-plunge,retract.

relocate- plunge, retract
relocate- plunge, retract
relocate- plunge, retract
relocate- plunge, retract
relocate- plunge, retract


New flycutter, new profile with new diameter

Locate-plunge,retract.

relocate- plunge, retract
relocate- plunge, retract
relocate- plunge, retract
relocate- plunge, retract
relocate- plunge, retract



The reason for the fad is its new...and a fad.
Ask a golfer, they'll offer up some reason...but as long as they are buying, ask me if I care.
 
I've done it with an engraving tool, it's just not as authentic as the real thing, which is indeed done with a fly cutter. The circles that are spaced farther apart are definitely done with a ball mill. Looks like I may have to get a fly cutter. Thanks BALLNH!
 
One might use a single point fly cutter with the shape of a 60 (or a 30*)included thread form with a .020 radius. Mill across .020 deep with a .040 feed-per-revolution to make the close marks as this would leave tool marks..…then with .040-.050 deep travel across with a 1"‘ feed per revolution. going right , then going left.
Yes few mills would not have such a high feed rate, so moving across above the part and then plunge down at each 1” going right , then the same going left. Plunge at each 1" spot,long travel free/above between each plunge..

Yes the cut arc would the diameter the fiy-cutter is set.

Once you git the feel for this it would go very fast.

Yes likely play with feed and depth until you get the look you like.

Back in the 60s I did a few like that with using a diamond cup wheel using a tool and cutter grinder for carbide golf club pads. Yes that took more time than it was worth so I only did a few. Nowadays with a CNC machine it would be quick work.
 
That insert will not make the grooves you want due to it's trailing flat. You would have to notch the trailing flat leaving only the radius.
A TPG cutter with a small radius might. Something that uses a VPxx might be better yet.
As said above the plunge and move method is going to be best for the deeper circles.
You need a pointy tool.
Bob
 
Wait...you started the thread about the chopped-up aluminum finish.

Just put the old TPG tool back in the machine and start a NEW FAD!!! :)
 
I think the OP does not want a scattered or by luck finish.
This in the domain of controlled, measurable and repeatable.
One should be able to run SPC on this face and hold it day in and day out.
Bob
 
Haha yep! I know right, to bad I literally threw it away *facepalm*. I was just thinking that that tool with some different inserts would have been perfect, ugh.
 
Why buy a fly cutter. Get a piece of stock and mill a slot with one edge on center for a tool bit. HSS carbide or insert, couple set screws and your done.

Or buy the 3 piece fly cut set...think its about $20. But then you have to wait...
 
The fine marks were probably done with[or could easily be done with] a fly cutter.

The heavy marks are engraved. I really cannot see doing the plunge move repeat with the head tilted or whatever, be easier to interpolate it
 
The problem with a flycutter on a well squared VMC is that you will bet bidirectional toolmarks.

However ...
put the same tool on a Bridgeport, cock the head by a 1/2deg .... Voila!
With power feed, it will be consistant and repeatable.
 
The fine marks are feed per rev and done with head nod or running uphill on square VMC (Z+ feed). One can see that in the edge to center widths.
Both methods leave only the leading edge.
The deep grooves are plunge circles. Note how they line up.
Bob
 








 
Back
Top