Subject: Cutting speeds and Depths

From: [email-masked] (John Dammeyer)
Date: Tue, 23 Jul 1996 07:19:43 GMT

hi,

Just received (finally) my end mill holders and now I can play with my
Drill press conversion.  I should have my drawbar installed in a day
or so and then I can safely do some milling in steel.  Not to say that
I haven't tried it using the 5/8" chuck to hold the end mill and
taking light cuts.  Works peachy in Al. and yesterday I even tried a
bit of steel.  Not much chatter.

So... for the question.  Given that I am following a chart for end
mill speeds ie; x RPM for d Diameter mill and that my drill press is
equivelent to an inexpensive far east Mill/Drill how big a pass should
I be able to make with this.

Lets say, for example I want to make a slot in mild steel 3/8" wide
and 1/2" deep.  On a huge Bridgeport can it be done in one pass or how
many passes should it take on:  (Give Mill RPM and number of passes) 

Sherline mill ??

Lathe (4.5" and 18" between centers) c/w Milling Vise ??

Lathe (8" and 36" between centers)   c/w Milling Vise  ??

Myford Mill ??

Taiwan type MILL/Drill (Sells for about $2000)

Gingery Mill ??

Is this purely a function of Motor horsepower or is size and mass a
portion of the formula?

Thanks

John.

Pioneers are the ones, face down in the mud,
with arrows in their backs.
Automation Artisans Inc.      Ph. 604-544-4950
6468 Loganberry Place         Fax 604-544-4954
Victoria BC CANADA V8Z 7E6

---

From: [email-masked] (Randolph Lee)
Date: Tue, 23 Jul 1996 10:06:09 -0400

In article <[email-masked]>, [email-masked] (John
Dammeyer) wrote:

snip

> many passes should it take on:  (Give Mill RPM and number of passes) 

snip

you have to take into account that with a slot drill (center cutting endmill)
that:

1. depth of cut when sloting should never be more than 1/2 the diam. of
the cutter... so to cut a slot 1/2" deep (easy on bridgeport in mild steel
even an old 1 HP Bridgeport like mine can make chips of 3/4 of a cubic
inch of steel a min and that is the old rule of thumb 3/4 to 1 Cu Inch of
MS per HP per Min) you would need a 1" dia cutter... with a 3/8 slot
(disreguarding that for 'nice' work you would use a 5/16 dia cutter and
then finish the slot exactly to size as your 3/8" slot drill will cut a
few thou over size) you would make multi passes 3/16 deep.

 Speeds on a light setup such as yours with a HSS slot drill would be 
about 450rpm don't bother with the info in industrial books... they are
for machines far more stiff than your set up... and they are concerned
with max econ life of a cutter in heavy use... you care about kepping your
cutter as sharp as you can as long as you can... for feed... feed it fast
enought so it does not rub (death to a sharp edge) and not so fast that
you get chatter or dig in. on  a light set up like yours 

get a copy of:
Vertical Milling in the home workshop by A. Thorpe ISBN 0-85242-843-X

one of the Nexus press (used to be Argus) Workshop practice series.(# 2 in
fact) see the FAQ for ordering details... I think Blue Ridge also used to
stock the WP series of books (all highly recomended for the budding HSM)

Good luck... my first 'mill' was an X/Y table on my Old Delta 18" drill
press... I retired it to cordinate drilling as soon as I found an old
Atlas MF horz bench top mill... now that I have the B-port I am looking to
sell the Atlas MF to get a Horz attachment for the B-port (matter of floor
space in the shop) the point is that even the smallest old bench top horz
mill is far more useful for milling than a drill press with an X/Y table
will ever be... but you can learn some useful things about milling with
it.

~R

---

From: [email-masked] (Randolph Lee)
Date: Tue, 23 Jul 1996 10:30:47 -0400

In article <[email-masked]>,
[email-masked] (Randolph Lee) wrote:

snip
> few thou over size) you would make multi passes  max 3/16 deep.
snip

I should have looked at Thorp before I replyed... the above is normal Ind.
practice for milling with a med sized machine like a Bridgeport with
cooling fluid and is how I do it today...(though I use a MicroDrop system
rather than a flood system to cool and clear chips)

A.Throp recomends for light HSM tools the following:
For HSS spiral flute endmills... Depth of cut up to 1/8 of cutter Diam. up
to 3/16" diam cutters... then up to 1/4 of cutter Diam. if milling a step
then the width of the step up to 1/4 the diam for the cutter.

so based on this you would make those passes 3/32 deep for each pass for
normal endmilling... if slot drilling though Throp says that about .070
per pass is a deep as you should go (450 rpm was his speed for a 3/8 HSS
cutter though)

~R

---

From: [email-masked] (John Dammeyer)
Date: Tue, 23 Jul 1996 15:48:08 GMT

Silly me!  I've read through Throp a few times and have always
considered it a bit superficial rather than a really good book about
'how to mill' and so forgot that there was a table in the back.  Well,
I have warmed up the photocopier and pinned the copy of the tables up
beside the drill press.

What the book doesn't quite say if I am cutting a step:

________
        |
        |
        |__
           |
___________|

Do I still follow the same speeds and depth of cut 'as if' I was
drilling a slot?

One point however.  A Bridgeport it ain't but my 20" drill press is
certainly as robust as a Sherline and much bigger than the
Dore-Westbury.  Once I pull the original spindle out to replace it
with my drawbar capable spindle I'll see if I can preload the bearings
somehow.

[email-masked] (Randolph Lee) wrote:

>snip
>I should have looked at Thorp before I replied... the above is normal Ind.

---

From: [email-masked] (Randolph Lee)
Date: Tue, 23 Jul 1996 16:45:46 -0400

In article <[email-masked]>, [email-masked] (John

> I have warmed up the photocopier and pinned the copy of the tables up

Well Throp is no Tubal Cain thats for sure....

snip

In the case above I go in sidways 1/4 diam of cutter and depth down 
Well the speeds and feeds I use on my B-port as starting points (note
these are just starting points... I adjust feeds by 'feel' from them) are
as below:
for HSS; Cribbed and modified and simplified for the need of my own shop
>from  the chart by Tubal Cain in "Milling opperations in the lathe" ISBN
0-85242-840-5 # 5 in the workshop practice series:
 from page 27:
In the case above I go in sidways 1/4 diam of cutter and depth down = to
cutter Diam. 
I slot at a depth of 1/2 cutter Diam and with a roughing cutter Slot at a
depth = to the cutter diameter.

now speeds and feeds I hope I have avoided too many typos in this but I
expect the real experts here will let me know If it is messed up too
badly.

>from  Page 118 with a bit of mod. to make it touch simpler; note that these
are Speeds and feeds for use when a cutter is to be pushed closer to it's
industrial rating... and the cutters must be resharpend "as soon as
distress is evident" as T.C. Says.

An '*' in a slot means "Cutter speed, Max available up to the speed given
with a tooth load = cutter dia/100; 
Feed rate is then = tooth load * RPM * Number of teeth

for 4 cutter HSS endmills in Cast steel, Malleable Iron, Monel metal, 18-8
S-Steel, HS steel (annealed), Steel Drill rod, And Phospher Bronze

Cutter Dia     RPM      Feed "/min
1/16           2000        0.19
1/8            1000        0.38
3/16            700        0.63
1/4             500        0.88
3/8             350        1.13
1/2             250        1.31
5/8             200        1.38
3/4             150        1.50
 1              130        1.63

for 4 cutter HSS endmills in Bronze, Cast Iron, Hard Copper, Gunmetal
Nickel Silver, and Mild Steel

Cutter Dia     RPM      Feed "/min
1/16           3800        0.50
1/8            1920        1.00
3/16           1280        1.38
1/4             960        1.75
3/8             640        2.63
1/2             480        3.00
5/8             385        3.13
3/4             320        3.50
 1              240        3.88

for 4 cutter HSS endmills in Aluminium, Brass, Muntz Metal, Duralumin

Cutter Dia     RPM      Feed "/min
1/16             *            *
1/8           *8100          4*
3/16          *5350        5.5*
1/4           *4000          8*
3/8            2700          11
1/2            2000          13
5/8            1600          14
3/4            1350          14
 1             1000          12

for 2 cutter HSS endmills (Slotdrills) in Cast steel, Malleable Iron,
Monel metal, 18-8 S-Steel, HS steel (annealed), Steel Drill rod, And
Phospher Bronze

Cutter Dia     RPM      Feed "/min
1/16           2000        0.25
1/8            1200        0.50
3/16            800        0.75
1/4             600        1.00
3/8             480        1.25
1/2             400        1.25
5/8             350        1.50
3/4             300        1.50
 1              240        1.50

for 2 cutter HSS endmills (Slotdrills) in Bronze, Cast Iron, Hard Copper,
Gunmetal
Nickel Silver, and Mild Steel

Cutter Dia     RPM      Feed "/min
1/16           3800        0.50
1/8            3200        1.63
3/16           2100        2.13
1/4            1600        3.00
3/8            1200        4.00
1/2            1000        4.00
5/8             900        4.50
3/4             800        5.25
 1              600        5.25

for 2 cutter HSS endmills (Slotdrills) in Aluminium, Brass, Muntz Metal,
Duralumin

Cutter Dia     RPM      Feed "/min
1/16             *            *
1/8           *9170        4.5*
3/16          *6110          6*
1/4           *4590          6*
3/8            3055          12
1/2            2295          15
5/8            1835          15
3/4            1525          12
 1             1145         9.5

---

From: [email-masked] (John Dammeyer)
Date: Tue, 23 Jul 1996 22:26:48 GMT

snip

>these are just starting points... 

<Giant Humongous snip>

Wow!  Thanks.

John.

---

From: [email-masked] (Randolph Lee)
Date: Wed, 24 Jul 1996 10:10:10 -0400

In article <[email-masked]>, [email-masked] (John

> >these are just starting points... 

Glad I could help John,

 We Islanders Have to stick together (G) I fell in love with your lovely
island when I visited it for a month back in the early 70s... one of the
nicest places in north america...

one other tip and it is the major one with milling... beware of 'cutter
rub' it will kill an edge so quickly and one of the things that cause it
'just feels right' to someone just starting out.... that is the tendanccy
to reduce feed when things are going badly... that will ofton cause rub...
what is normaly needed is to reduce  the depth of cut and keep up the feed
rate... try to keep 2 flutes of your cutter on the work at all times if
the depth of cut needed is not deep enough to allow that... then select a
smaller endmill

the thing that I still have the hardest time with on the mill vrs the
lathe is getting off the last 'odd thou' it is very hard (for me) to mill
less than 3 to 5 thou off a part with good surface finish... I try to
leave a last cut of say 10 thou for this reason.

good luck and keep us posted on your progress

~R
Windshadow Enginering
Nantucket Island MA USA

---

From: Mike Rehmus <[email-masked]>
Date: 29 Jul 1996 03:35:58 GMT

>leave a last cut of say 10 thou for this reason.

Sometimes I have good luck by flooding the surface with coolant and
running the speed up a lot.  The odd thou comes right off and the
surface looks like a mirror.  Course my shirt looks funny with a
horizontal line across the chest.

Best regards,

Mike Rehmus