feed speed for boring bar

[ken wong]

HI everyone

i need to bore a hole dia .562+/- .0002 deep 1.4 on aluminum (job on mill) i use boring bar but not luck

how do u recomment feed speed and material left for boring bar

[MotorCityMinion]

Try to find lathe turning data for that material and apply that to the boring bar s&f.

 

+ or - .0002 is fairly tight. Reaming or burnishing may be an alternative worth investigating.

[iowajim62]

spot drill, drill .531, use 1/4 2 flt dataflute endmill with .250/.375 loc and flat-bottom with G81, then helix bore with same endmill to .560 dia, now bore with 1/4" carbide bar using 2500 rpm and feed 5 ipm, don't let boring bar go 1.400 deep only go 1.399 dp.

 

do test cuts on setup part or scrap material first and adjust boring bar till just right

 

hth

[dprovost71]

This may go without saying but make sure you have a good tenth set boring head.

[iowajim62]

quote:

---

have a good tenth set boring head

---

yeah and a set of Del-Tronics pins wouldn't be a bad idea either

[crazy^millman]

Tenth Set Boring Bar most important.

 

Carbide Boring Bar 2nd thing needed.

 

Very positive cutting Insert. Kaiser make a good system this small.

 

.0001 reading internal Micrometer would be a huge help.

 

.557/.559 regrind 4 flute endmill to help you hold true position and get the hole a normal size before boring.

 

I would use Kersoene or WD40 to do the holes.

 

Probably start at about 800 to 1000 rpms and .35 feedrate per inch.

 

HTH

[robk]

What kind of problem are you having? Holding the size or chatter or both?

+/-.0002 is not all that tight.

Make sure you're not rubbing the material, but actualy taking a cut. If you have chatter then make sure you go underneath it to get rid of it.

I prefer to do 2 passes per hole that size using G75 cycle (bore in/ orientate/ rapid out) because even carbide will deflect a little bit.

I always found that 1000 rpm @ 1 IPM is pretty good area to start no matter what kind of material I'm cutting.

Also a good quality boring heads and bars make all the difference. We use Urma brand.

[Namliek_J@TheeCircle™]

Romicron Boring Heads work the best IMO.

[DavidSV]

We have an Iscar Boring head with the available attachments. With it you could just use a standard bar and insert. We consistantly hold a +.0002,-0 hole with it.

 

On our mills, its G76 for feed in, orient, shift and rapid out.

 

Oh, and don't load the boring head in backwards.

 

David

[Justin Beebe at Folsom Tool]

We hold +-.0002 with Ron's method. We use tenth set Valenite or Komet boreing heads.