CNC milling into corners

[Ian Paterson]

So I just broke a 1/8" endmill when I tried to cut a 3/16" keyway in a pulley. I decided to use climb milling in a semicircular tool path to "scoop out" the keyway in 0.1mm passes. I used a tried-and-true "feed, speed & chip thinning" formula for side milling in a straight line, but there may have been an increased chip load because I was cutting a fairly tight inside radius. 

Has anyone had a similar experience? Should plunge cuts or multiple passes while incrementing the z axis instead? I recall This Old Tony broke an endmill in a similar scenario when he was trying to cut a gear on his CNC machine.

Ian

[Larry Maas]

I'm guessing the biggest problem is usually RPM required for a small cutter. A 1/8 HSS cutter machining aluminum requires about 400 surface feet per minute, RPM needs to be over 12,000 RPM. Most home mills are limited for speed. What are you using for coolant / lubrication? Mineral oil (paint thinner) or kerosene work well. With small cutters, compressed air helps to clear chips while machining. Curious to know what a speed, feed, and chip thinning formula is, never heard of it. Climb milling is ok if you have ball screws, otherwise I'd recommend conventional. Any pics of job? 

[Ian Paterson]

Hi Larry,

I'll work on sending pics, but for now I can give some details:

• My mill uses ball screws and I tweaked the backlash compensation in Mach3 to the best of my ability before running the job. I've never had a problem with climb milling when doing straight line cuts.
• Mild steel
• No coolant or lubrication
• 4 flute, carbide 1/8" endmill with nitride coating
• 4443 rpm gives me a cutting speed of about 145 SFM
• Feed rate 400 mm/min
• Radial depth of cut 0.1mm, axial depth of cut 7mm

The following numbers came from my own homebrew formula for calculating chip thinning, but it's for straight line cutting and doesn't take into account the significantly greater chip volume and thickness when cutting an inside radius:

• 0.023mm feed per tooth
• 0.008mm max chip thickness
• 0.029mm^3 approximate chip volume
• 508 mm^3/min material removal rate

Attached is a terrible diagram and formula that I use to calculate chip thinning. It also illustrates how much more material each tooth of the cutter must remove when milling an inside radius. Imagine the orange line is the inside radius of the material being cut.

Also attached is an .ods spreadsheet which has a practical application of the chip thinning formula - it's in column N. I never figured out how to simplify the formula, so the one in the spreadsheet is horrific. Line #39 has the data for the g-code I ran that broke my endmill and the red one below it is what I'll try next with 0.1mm Z increments per pass.

Ian

[Ian Paterson]

And here's my G-code in case anyone wants to see it:

% 20211211 I'm installing a treadmill motor on the No129 lathe and I need to adapt the plastic treadmill pulley to fit the lathe countershaft
% Countershaft is 3/4" diameter with a 3/16" keyway
% I'll be using a 4 flute, 1/8" carbide endmill
% Milling with a cutting speed of 44.317m/min (145 SFM) which means I need to run the spindle at 4443 RPM

% I want a chip thickness of 0.011mm, so feedrate should be 200mm/min
% I plan to make the cut at 0.1mm Z depth increments, using slot-style milling (axial depth of cut is same as bit diameter)

#100 = 1 (this is the z height - use positive numbers for testing, actual run should be -12.7mm)
#101 = 1 (Number of times to call subroutine. For the actual run, this should be ?)

O0001 (Main program)
G21 (millimeters)
G90 (absolute positioning mode)
G17 (XY plane select)
F200 (feedrate 200mm/min)
G0Z20 (move up to a safe height)
G0X0Y0 (move to centre axis of bore)
G0Z[#100] (move down to working depth)
G1X0.79Y7.05 (move at current feed rate into position for cutting the arcs)

G91 (relative mode)
M98 P0002 L[#101] (Call subroutine L times)
G90 (absolute mode)

G0Z20 (pull up to a safe height)
G0X0Y0 (return home)
M30 (Program end)

O0002 (Subroutine for milling keyway)
G1Z-0.1 (advance the cutter 0.1mm down)
G1Y4.18 (advance in y direction into keyway slot)
G3X-1.58I-0.79 (counter-clockwise arc at top of keyway slot)
G1Y-4.18 (retract away from keyway back into pulley bore)
G1X1.58 (return to start point)
M99 (Return to main program)

[Ian Paterson]

[Ian Paterson]

I should point out the above G-code represents the new tool path that I plan to use, which decrements the Z axis by 0.1mm with each pass. It ought to be slower with a more consistent chip load.

On Wednesday, 15 December 2021 at 06:17:43 UTC-8 Ian Paterson wrote:

[Ian Paterson]

Here's a revised chip thinning diagram. Purple area shows the chip size when milling a straight line and the purple + pink areas together show the chip size when milling into an inside radius. The relative sizes of the cutter radius and material radius are not to scale, but I think it's close enough to give a general idea.

Sorry for so many posts, but the forum has been rather quiet recently and I thought some people might find this interesting :-)

Ian

On Tuesday, 14 December 2021 at 23:02:06 UTC-8 Ian Paterson wrote:

[Mat Stoeckle]

No worries Ian, it’s all jibberish to me but I’d love to learn someday. Still refurbishing my manual machines. Coming along nicely however :)

I was just about to start the “shop visit” series when Omicron happened. Guess we’ll wait a little longer to see how that pans out. 

Sent from my iPhone

--
You received this message because you are subscribed to the Google Groups "Victoria Hobby Machinists" group.
To unsubscribe from this group and stop receiving emails from it, send an email to victoria-hobby-mac...@googlegroups.com.
To view this discussion on the web visit https://groups.google.com/d/msgid/victoria-hobby-machinists/247c27f0-74ef-4874-b1d4-af73bcbd0271n%40googlegroups.com.

<Chip thinning diagram.pdf>

[Larry Maas]

Ian, small cutters need high speed, carbide needs 4 times the speed of HSS. You have enough speed for HSS on your machine, running about 100 SFM, or about 3200 RPM, possibly higher, use coolant or mister or air. Depth of axial cut might be excessive. With this small a cutter I'd suggest reducing feed per tooth to .0005" or .015 mm . Carbide needs high surface speed to cut, otherwise it just rubs and eventually breaks from side pressure. High speed is tougher, albeit slower.

I understood your drawings more or less, still unclear on what chip thinning is.

Or you could find someone with a broach or a shaper (know anyone out there Mat?) that could cut it. Another alternative is simply mount the hub in a lathe and broach it with a single point tool on a boring bar. Quick and simple.

[Alex Kunadze]

Hi Ian,

That 7mm axial depth of cut is definitely a problem. That's over 2x
the tool diameter. Also check the runout on the cutter once it's
mounted. It has much more impact as tools get smaller. Can be
corrected a little bit by gently tapping on the cutter. If you're
still having problems, plunge milling might be the best solution. It
places almost no radial load on the tool, so less chance to break it.

Cheers,
Alex.

> To view this discussion on the web visit https://groups.google.com/d/msgid/victoria-hobby-machinists/ad68494f-b17c-4795-8da2-c95d65dc9585n%40googlegroups.com.

[Ian Paterson]

Ok I got the job done. Thanks Larry and Alex for your advice.

I ended up removing most of the material with 127 "D-shaped" passes, each one 0.1mm further down than the previous. So in other words, only the bottom 0.1mm of the endmill's cutting edges were being used. After that, I was able to go back to my original plan of using the full 1/2" length of the endmill's cutting edges to clean up the sides of the keyway with a 0.1mm radial depth of cut and 400mm/min feed rate. I avoided the high chip loads by simply cutting into the keyway on one side, then moving in a straight line across to the other side without following the curved top part. After that, I found the key would fit the keyway high up, but not deep down. This suggests the sides were tapered due to tool deflection, so I ran about 5 spring passes and then the key fit nicely.

Alex, you expressed concern about the axial depth of cut being greater than 2x the tool diameter. As I understand it, that rule of thumb applies to slot milling where the radial depth of cut is the same as the bit diameter. In my case, the radial depth of cut is only 0.1mm, so I was able to use the full 12.7mm of the endmill's cutting edges. I'll be sure to check cutter runout in the future and yes, plunge milling sounds like a safe bet.

Larry, you suggested reducing the feed per tooth to 0.015mm and I think this is where chip thinning comes into play. If the radial depth of cut is equal to or greater than the bit radius, then the maximum chip thickness is the same as the feed per tooth. If on the other hand, the radial depth of cut is only a small fraction of the bit's radius, then the maximum chip thickness is reduced and you have to increase the feed rate to bring the thickness back up. I was actually quite surprised how much the feed rate had to be increased when using a shallow radial depth of cut. As a rule of thumb, I've tried to keep the maximum chip thickness in the 0.01 - 0.02mm range for small endmills. I think you made a good point about coolant, so one day I may look into getting some kind of MQL or mister.

Regarding cutting speed, my mill can only go up to 4443 rpm before it starts to time travel, so that's all I've got to work with. In my opinion, a stock Chinese Mini Mill isn't rigid enough for heavy cuts with big endmills and it's not fast enough for use with small endmills, so I tend to stick to cutters between 3 and 8mm. I suppose there are exceptions for fly cutters and stuff like that if you're taking really light cuts though. I have a feeling that maintaining a high cutting speed with carbide is more important for cutters that aren't very sharp like with cheap coarse-grain carbide turning inserts. Modern carbide endmills and router bits seem exceptionally sharp though, especially expensive ones, and I think you can get away with dropping the cutting speed if you have no other choice and you adjust feed rates to maintain an adequate chip thickness.

The following video encouraged me to incorporate some aspects of high speed machining when writing G-code:

https://youtu.be/5bjMjE4Y7e8

And this video explains chip thinning better than I did:

https://youtu.be/SjbmFywJN7Y

Ian