Surface finish

[CNC-ERIC]

Hi, there,

 

I have a job which has a flat bottom hole of 8.500mm (0.3346)" with depth of 44.5mm (1.750)", tolerance is 0.001", the internal surface finish is 1.6um, Can anyone give suggestions on tooling,RPM,feed,depth cut? the material is Al6061 T6.

 

thanks very much.

 

Eric

[Colin Gilchrist]

For those kinds of features you will have to EDM it... Anything else is majorly cost prohibitive. Especially if the flat bottom has that finish requirement

[Matthew Hajicek - Singularity]

Yah, that finish is the killer. No flat bottom drill is gonna do that.

[GoetzInd]

I would try a nice micro100 boring bar in a little boring head. Its worth a shot.

[CNC-ERIC]

thanks for your inputs.

 

Eric

[crazy^millman]

If that finish is a metric call out then it is a 63 finish in English.

 

Here is a link: Metric to English Surface Finish Chart

 

HTH

[mold100]

if that is the case I would helix bore with multipasses on using a .250 2 flute data flute a 63 is not that bad to achive even that deep. They have these cutters with 2" LOC. I cut pocects with .130 rads 1 3/4 deep with them. just keep the rpms down below 5000 they can squawk alot going deep.

 

[ 09-18-2008, 06:31 PM: Message edited by: mold100 ]

[Colin Gilchrist]

Yep, if that finish is a 64, any standard carbide endmill should be able to hold those tolerances. I would cuse cutter comp. of some kind and helix bore it like mold100 mentioned.

 

Good luck...

[MotorCityMinion]

Don't think so.

 

"A micrometre (American spelling: micrometer; symbol µm) is one millionth of a metre, or equivalently one thousandth of a millimetre. It is also commonly known as a micron. It can be written in scientific notation as 1×10−6 m, meaning 1/1 000 000 m."

 

He said UM, thats incredably fine. I wasn't aware that sinker edm's could achive such a fine finish.

 

Some spotfaceing tools can achive relatively fine finishes, rigidity being a must. I might try fine boring for the sides, radiused nose of course, and a 2 flute e-mill ground .002 under dia. Knock 1 of the flutes off, then grind the remaining flute flat, with a 3 deg. primary relief, followed by a 7 deg. secondary relief, making sure that the remaining flute barely comes across centerline, thus avoiding a xxxx in the center of the spotface. SLOW speed and light feed with a dwell should do the trick. Leave the bottom of the bore heavy, and mess with it untill you achive the finish your after.

[David Perron]

1.6 micrometers does approximately equal 64 micro inches. Here is why.

 

1 mm = 1000 um

1 mm = .03937 in

 

setup the conversion like this

 

1.6 um X in

------ = ---- ---> solve for X

1000 um .03937 in

 

X =.000062992 and multiply by 10^6 to get back to micro inches

 

X = 62.992 microinches or 63 Ra

 

This kind of stuff can mistakenly make a $100 job into a $1000 pretty quick.

[CNC-ERIC]

THANKS ALL YOU GUYS,

 

LEANT LOTS

[FP1]

I used to turn brake drums for a Japanese forklift company. The finish requirement for the braking surface was 2.5 um which came out to a surface fininsh of 98 in inches. The formula I used was a little easier (maybe not totally accurate) but it was 2.5/.0254 = 98.4

[Dracbus]

I agree with mold100. ive done several holes just like what he discribed and using a 1/4" flat bottom endmill and rotoring out the hole and finishing with a nice carbide endmill should do the trick. Have a gauge pin handy that is the size you want and do your final pass with a 2d with cutter comp until the pin fits. Carbides tend to be a thou or 2 off so dont forget to take that into account.