What's new
What's new

What is the best way to mill the inside of a cone ?

jakefreese

Hot Rolled
Joined
Aug 4, 2012
Location
TEXAS
I have a funnel that I am cutting, 2" at the top, down to 3/8" bore at the bottom, 45 degree angle.

I tried with a 1/4" ball mill, but material has to flow down the funnel and surface finish has waves even with 0.020" step down.

I thought about running a 45 deg insert chamfer mill down it, single insert Iscar with a .25" center. I just have not figured out how to set the boundaries in Fusion360 as it wants to make a flat spot in the bottom. Its granular material that has very small light grains.

Any recommendations or ideas?

Drill 3/8 all the way through
1/4 Rougher
45 degree chamfer mill
1/4 ball mill to round off the transition down the hole
 
Kind of sounds like "what's the best way to mill a pocket in a lathe?"

Sure sounds like this is a job that would turn (out) faster and with better surface finish on a lathe, or on a 4th axis if the cone is in some awkwardly large part??
 
No CNC lathe yet.... I'll try the smaller steps. Hopefully lube line parts will be here soon, I went to fixing a leak and the fitting is cracked. I may run this operation on the manual lathe if the smaller steps don't smooth out, then run the outside on the mill.

The part is 2" diameter at the top.

Thanks!

Sent from my XT1254 using Tapatalk
 
Try using the 1/4 ballnose milling from top to bottom of the cone, up and down all the way around.
Of course you want to rough first.

I've used this technique and able to achieve a nice finish.
 
Thanks! Looks like I need to refine my step down and speeds to get it right. It will be nice to have a bunch of these in a fixture and let it have at it

Sent from my XT1254 using Tapatalk
 
I don't see the issue with using a chamfer mill. Of course there is a flat spot on the bottom (a chamfer mill does not have a zero diameter point) but then you said the bottom is 3/8" diameter, so that could be a 'flat spot' but that would be harmless.
 
I have a funnel that I am cutting, 2" at the top, down to 3/8" bore at the bottom, 45 degree angle.

I tried with a 1/4" ball mill, but material has to flow down the funnel and surface finish has waves even with 0.020" step down.

I thought about running a 45 deg insert chamfer mill down it, single insert Iscar with a .25" center. I just have not figured out how to set the boundaries in Fusion360 as it wants to make a flat spot in the bottom. Its granular material that has very small light grains.

Any recommendations or ideas?

Drill 3/8 all the way through
1/4 Rougher
45 degree chamfer mill
1/4 ball mill to round off the transition down the hole

JAKE its like this...for a 8 finish a feed of .0007 is needed....for a 16 finish a .0015 feed per rev or per tooth....for a 32 finish .003 feed is needed...for a 64 finish a .005 feed is needed and so on...I believe I have that correct and to double check me get a comparator finish guage and pick a finish with mill or lathe and mic the pitch of the finish cuts on the guage....so with that in mind I would use a 5/16 ball endmill on the entire thing...one tool....super smooth of whatever finish I pick....for instance if I have a 4 flute endmill and run 1000 rpms that's 1000 X 4 flutes X .0015 = 6.0 inches a minute gonna leave about a 20 finish...run part again and take out deflection and it will come out a 16 finish....I then let it run overnite and in the morn.....WALLA
 
What is the material?

You can not use a chamfer mill because the angle is not exactly 45.0000
You will have steps down the wall at every stepdown.

Rough it down
Semi finish it 5/16 ball .020 steps with .008 stock
Finish with 5/16 ball and use a continous spiral 3d path down so there arent stepover lines .008 would be ideal.
 
JAKE its like this...for a 8 finish a feed of .0007 is needed....for a 16 finish a .0015 feed per rev or per tooth....for a 32 finish .003 feed is needed...for a 64 finish a .005 feed is needed and so on...I believe I have that correct and to double check me get a comparator finish guage and pick a finish with mill or lathe and mic the pitch of the finish cuts on the guage....so with that in mind I would use a 5/16 ball endmill on the entire thing...one tool....super smooth of whatever finish I pick....for instance if I have a 4 flute endmill and run 1000 rpms that's 1000 X 4 flutes X .0015 = 6.0 inches a minute gonna leave about a 20 finish...run part again and take out deflection and it will come out a 16 finish....I then let it run overnite and in the morn.....WALLA

6 inches per minute? LOL
Is the part inconel?
 
What is the material?

You can not use a chamfer mill because the angle is not exactly 45.0000
You will have steps down the wall at every stepdown.

Using a spiral helical path, with about .020" per turn, and the chamfer mill would blend at least as good as the ball mill at a much finer step. I think so anyway.
 
JAKE its like this...for a 8 finish a feed of .0007 is needed....for a 16 finish a .0015 feed per rev or per tooth....for a 32 finish .003 feed is needed...for a 64 finish a .005 feed is needed and so on...I believe I have that correct and to double check me get a comparator finish guage and pick a finish with mill or lathe and mic the pitch of the finish cuts on the guage....so with that in mind I would use a 5/16 ball endmill on the entire thing...one tool....super smooth of whatever finish I pick....for instance if I have a 4 flute endmill and run 1000 rpms that's 1000 X 4 flutes X .0015 = 6.0 inches a minute gonna leave about a 20 finish...run part again and take out deflection and it will come out a 16 finish....I then let it run overnite and in the morn.....WALLA

So says the Jon Banquer of machining.
 
I run some graphite parts with an ID taper that need a smooth finish for glass work; when I can't use the lathe I have a couple of endmills ground to match the taper angle. I do pretty much as Dennis said, rough, then contour/spiral down. Customer seems to always be changing up the sizes and taper angles so I usually run a .02" stepover semi finish on the first one and then adjust the stepover based on that finish to what seems appropriate for that particular taper, and endmill grind.
 
If anyone here can take multiple passes in Z with a chamfer mill and get surface finish that doesn't have lines, I'll buy them lunch. I spent some quality time trying on a certain part and was never successful... it should work, it's simple math :)

If I really had to do it on a mill, I would use a helical flow line surface with a .00015 scallop height. Bottom to top. Roughing with a .020" scallop height. It's going to take some time. If I needed to do a couple and I didn't have a lathe, I would rough as above, then turn the funnel over and chuck it in a cat40 tool holder. Clamp a boring bar in the vise and write a bone simple tool path to turn my cnc mill into a lathe. Two tool holders and I could do that op just about as fast as a cnc lathe.
 
Sorry, thought I had the material in there 6061 T6.

That is a heck of idea Proto with turning it into a lathe

I have 1/4 end mills, and no 5/16 right now. I'll get some ordered tomorrow.

Sent from my XT1254 using Tapatalk
 
A while back, I did a part similar to what you describe, slightly trickier though. Around a 20-degree angle, 3-1/2" deep or so, with a 6mm hole at the bottom of the cone... had to use a 1/2"-dia extension chuck stuck out 3", with a 3/16" ball nose out 1" from the extension! LOL

Anyway! I ran 12000 RPM and either 45 or 60 IPM. Drilled just under the through-hole size from the top of the cone, then roughed with a 3/8" and 3/4" drill from the back (large I.D.) side of the cone, then roughed further with an end mill to rough in the angle as much as I could...

Worked out quite well with a step down of about .005. Took about 20 minutes or so for the surfacing toolpath. I wish I would have run it twice, a rough and finish pass with the ball nose. I think the tool had gotten some build-up on it, it was taking a fairly wide cut towards the bottom of the taper.

Anyway! Try something like that. Drill through with the finish diameter if your size is not crucial, rough it with a normal or bull end mill, then finish surfacing with a ball or fresh bull nose. Typically when surfacing your chipload can be a bit higher than normal cutting. I don't go too high, as going too high does give a sort of grainy feel. Start out around .0015 per tooth, max RPM, .005 stepdown.
 
As there doesn't seem to be an issue with roughing I'll throw something out for thought.
After roughing ( to the point near size but just doesn't look good)machine a male cone to fit the "funnel"
Using contact cement or your favorite removable glue attach a piece of 600 wet sandpaper to the entire surface
As slow as your mill will go with coolant wash, you may be looking at a mirror when done
If possible load the "cone" on a spring loaded holder

I did something similar with a pocket that had a 3/4" radius at the bottom
 








 
Back
Top