What's new
What's new

Making a deep hole with good finish and accuracy

matoind

Plastic
Joined
Mar 4, 2005
Location
India
I have to make a hole of Dia 13.5mm and 68mm deep in Aluminium 6082. The finish required is 0.8 Ra max.

I am doing bigger holes on CNC lathe with carbide boring bars. But this one seems to be challenge as I will have to use a 8mm Carbide boring Bar would mean L/D ratio of 8.5 Times. This results in chattering.

I am thinking of doing this hole on a VMC. But I am not sure about the tools to use! Maybe a Drill of 13.25mm followed with a boring bar. Or maybe a PCD drill?

Wohlhaupter sales person is not confident that it is possible on their holders even with carbide boring bar and not not seem to have a solution.

So I guess it may have to be PCD Drill.
 
Use a larger boring bar or reduce the tip radius on the cutting edge to near nothing. Preferably both. :)
 
Is it a blind hole? Might want to try feeding left to right for the finish.
Do you have the budget to buy a carbide dampened bar?
 
I am lost here, it isn't even 10x diameter deep. Why not just drill and ream for the finish requirement?
 
Use a 10mm boring bar. That needs a minimum bore size of 12mm so you have plenty of clearance.


Sent from my iPhone using Tapatalk
 
That was my reaction, ......but I didn't post as the R word seems kinda dirty on the CNC forum.

You can ream faster than boring and you don't have to worry about galling in soft aluminum from chips getting packed around a boring bar. No brainer to me unless you are making a one off and you don't have a reamer in stock, but plenty of boring bars.
 
I gotta agree. It just seemed like such an obvious answer, I suspected a trap.:D

Maybe the metric numbers have baffled some of the USA contingent here. It amazes me how many machinists can't convert metric numbers to inches in their head. The last place I worked for the man almost everybody but me had either a small calculator (most people didn't have cell phones then)or a decimal equivalent chart in their pocket.
 
Maybe the metric numbers have baffled some of the USA contingent here. It amazes me how many machinists can't convert metric numbers to inches in their head. The last place I worked for the man almost everybody but me had either a small calculator (most people didn't have cell phones then)or a decimal equivalent chart in their pocket.


.03937

For rough conversions on the fly, I just use .040.
 
I would be leery of reaming the hole, IF you only have 1 shot at the part.
Reaming is a crap shoot, at best, if you have no experience with the exact same part/material/tooling/ machining strategy, etc....

Without notes or previous experience, I can foresee any/ all of the following:
Bell mouthed hole
Over/undersize issues
retract lines (scratches) from the reamer
wondering hole

I love reamers, but when I NEED absolute control over a NEW process; always the boring bar.....

To the OP, if you have some setup parts, and or some extra material, DEFINITELY try a reamer.
Drill a 33/64" and follow it up with a LH sprial, RH cut reamer. If you can get coolant through the reamer, it will be a snap!

Doug.
 
hole is .5315" depth is 2.677", microfinish 125 ra.

Buy a 13.1 drill if you're getting oversize holes. if not 13.2mm (.520) then ream it 13.5.

buy a brand new chucking reamer and lovingly dull the corner at the chamfer with a "reamer stone" or equivalent

Make sure drilled hole looks like 13.2mm

Throw some of that green tapping fluid for aluminum on the reamer with an air gun

ream it at 50 rpm and 15.25 mm/min (.012" / rev) feed

increase feed rate & speed for a little bigger hole

bore in - bore out, don't rapid out or you'll yank the part out of the vise

and if the finish comes out ugly, have a 13.5mm ball bearing ready and press it through ...

wait, is this a blind hole or thru hole?
 
Finish is 32


Is there a reason that you can't use a reamer? (BTW - that is 17/32 inche in Western civilization)

Is it blind?

Does it need to have sqr bottom?


I for one would NOT go with a LH spiral reamer unless it's a through hole. (we are in the "CNC" forum, so I'm expecting that this is not a Manuel opperation that needs the LH twist)

I also would NOT stand it up and bore it in a mill if it is blind.

If a reamer is possible, I would use a floating holder to help it stay on size and negate those nasty pull-out marks that you were warned about prior.

If you need a sqr bottom in a blind hole, I have had endmills altered with through coolant (apparently a "hole popper" is the ticket for this. Many folks with wire EDM's will have this.) The coolant through will help to flush the chips out. I have had good luck with this in 6061.


disclaimer
I have no experience (knowingly anyhow) with this flavour or alum.


------------------------

Think Snow Eh!
Ox
 








 
Back
Top