A286 small feature machining

[socalsurf]

I have a very small pocket I need to machine in A286, bought the material from McMaster, .625" round stock. Part measures .115" long. Pocket to be machined is circular with 2 round ears , like a slot and circle combined. I am predrilling the hole to .089 diameter, opening up to .112. Smallest radius in pocket is .020" so I am trying to use a Harvey end mill, https://www.harveytool.com/products/tool-details-886231-c6 .  Using Harvey's speed and feed guide, https://harveyperformance.widen.net/content/jno1w53rk1/pdf/SF_886200.pdf?u=1i9tm9, using Nickel alloys as the guide, I get 50SFM and .0001 per tooth. I am trying a radial and axial DOC of .008" and not having much luck, broke 3 end mills.  Any suggestions on how to make this work besides sending it out for wire EDM?

Thanks, LeoC

[JParis]

Check your run out on that tool, anything is going to hamper the tool...

A .031 e/m at 50 SFM is an RPM of 6100..

A feedrate of .0001 CPT works out to a feedrate of 1.83 IPm

50 * 3.82 = 191

191 / .031 = 6161 RPM

.0001 x 3(flutes) - .0003

6161 RPM x .0003 = 1.848 IPM

You don't list anything beyond SFM

[crazy^millman]

1 hour ago, socalsurf said:

I have a very small pocket I need to machine in A286, bought the material from McMaster, .625" round stock. Part measures .115" long. Pocket to be machined is circular with 2 round ears , like a slot and circle combined. I am predrilling the hole to .089 diameter, opening up to .112. Smallest radius in pocket is .020" so I am trying to use a Harvey end mill, https://www.harveytool.com/products/tool-details-886231-c6 .  Using Harvey's speed and feed guide, https://harveyperformance.widen.net/content/jno1w53rk1/pdf/SF_886200.pdf?u=1i9tm9, using Nickel alloys as the guide, I get 50SFM and .0001 per tooth. I am trying a radial and axial DOC of .008" and not having much luck, broke 3 end mills.  Any suggestions on how to make this work besides sending it out for wire EDM?

Thanks, LeoC

In a ER collet? Throw in a Precision Hydraulic control TIR to less than 3 microns and then you might be successful.

[#Rekd™]

In HSM advisor I ran it with a slotting (0.02" deep) application in Inconel at 50SFM and I am getting these numbers:

6164 RPM

0.58 in/min

Chip load 0.00003"

If the depth is 0.01 slotting application I am getting these numbers:

6164 RPM

0.92 in/min

Chip load 0.00005"

 

As stated by JP and Ron, runout will increase the chip load dramatically on one of the teeth. 

 

 

[socalsurf]

Thanks for the feedback, I didn't allow for the runout factor, my bad. I see MSC has Regofix tool holders on sale, I think I will pick up one of those. I was at 2.5 IPM, so also too high of a feed.

LeoC

[huskermcdoogle]

With A286 you are in the realm of needing to make a chip but not rub like any other S3 type Nickel based material.  As mentioned earlier, runout is killer with these small tools as usually runout is easily greater than your chipload...   

Just as a rule of thumb, it is pointless to run a chipload less than your runout...  I have found that chiploads under .0002" usually don't have any benefit any typically yield worse results with anything larger than .062", but given your cutter diameter, you will need to reduce some if slotting, so their recommendation of .0001" should be achievable, but you will have to have runout less than half of that likely, and you will need to find a sweet spot where you can still make a chip, but not overload the cutter and break it from bending load.

SFM likely won't matter much as you probably don't have enough spindle speed to actually burn up a cutter, and is more going to be a function of balance and how dynamically stable your spindle is.

 

 

[Matthew Hajicek - Singularity]

I manage this kind of thing in ER collets all the time, but my holders and collets are in very good shape, and I carefully clean them every single use.  Harvey's suggested parameters are for cutting in a straight line; you'll be making concave scoops in those slots, which increases the engagement angle.

[socalsurf]

Update:

Purchased and used a Regofix high precision ER16 tool holder and collet. For the small feature, I first drilled as large a hole as would fit with .010 clearance per side, then used a .040" four flute end mill to clear out the pocket leaving .002, this was run at S4900 at 5ipm with a stepover and DOC of .008. This tool lasted through all 6 parts. To finish the sidewalls, I used a Harvey 886231-C6 in the Regofix tool holder at S6160 at F .9 taking .002" radially and .008 DOC. I used 3 radial passes each at .002 to cut the required feature. I was able to cut 2 parts with one tool before I was getting a small taper which blew out the required tolerance. 

Thanks for all of the help and suggestions. I would have updated sooner but I had caught the COVID, fortunately, it was a mild case.

LeoC

[Charlie Pierson]

Check out Schunk Tendo E  hydraulic holders for those small endmills.

3 micron and under !!