Deep Pocket Milling Stainless Steel

[Matthew Ensor]

Hi All,

Just hoping to get peoples thoughts on how to go about this maching problem.

I have a pocket to mill in 316L forged stainless steel 146mm x 146mm x
142.5mm deep with R20mm corner rads. The pocket has been pre-roughed on a
lathe to 136mm dia x 140mm deep
There is a rectangular thro pocket 20mm wide x 120mm long thro at the bottom
of the pocket which is machined in from the opposite side at a previous
operation.

The ideas so far:

1. Use Iscar's SHRED MILL cutter on an arbor to rough out the pocket
2. Use a HI FEED TRIWORX type design cutter to rough out pocket, utilising
approx 0.7mm DOC with 0.8mm per tooth / per rev feed.
3. Use convential type ripper and finisher cutting tools, multi staging with
diffrent lengths, or via a shell mills on arbors.
4. SUB IT


Spindle is a 40 Taper,10K rpm, T/Coolant, machine new Mikron VCE600

The Shred mill looks a cool idea but it utilises button inserts with the
ripper style knuckle ground into them, so am not sure about the loading on
this. The hi feed cutter (SECO TOOLS) has the right lengths / geometries but
have no experience of these either.
The covential method is possible if not slllllooooowwww and costly.

I have 7 off parts to manufacture approx evey six months, these are very
high value. Billets alone are close to £1000 each. So I need to be confident
on a solution

All of your thoughts and advice very much appreciated


thanks

Matt

[Matthew Ensor]

OOPS


The pocket is 164mm x 164mm x 142,5mm deep with R20mm corners.

Matt

Post by Matthew Ensor
Hi All,
Just hoping to get peoples thoughts on how to go about this maching problem.
I have a pocket to mill in 316L forged stainless steel 146mm x 146mm x
142.5mm deep with R20mm corner rads. The pocket has been pre-roughed on a
lathe to 136mm dia x 140mm deep
There is a rectangular thro pocket 20mm wide x 120mm long thro at the bottom
of the pocket which is machined in from the opposite side at a previous
operation.
1. Use Iscar's SHRED MILL cutter on an arbor to rough out the pocket
2. Use a HI FEED TRIWORX type design cutter to rough out pocket, utilising
approx 0.7mm DOC with 0.8mm per tooth / per rev feed.
3. Use convential type ripper and finisher cutting tools, multi staging with
diffrent lengths, or via a shell mills on arbors.
4. SUB IT
Spindle is a 40 Taper,10K rpm, T/Coolant, machine new Mikron VCE600
The Shred mill looks a cool idea but it utilises button inserts with the
ripper style knuckle ground into them, so am not sure about the loading on
this. The hi feed cutter (SECO TOOLS) has the right lengths / geometries but
have no experience of these either.
The covential method is possible if not slllllooooowwww and costly.
I have 7 off parts to manufacture approx evey six months, these are very
high value. Billets alone are close to £1000 each. So I need to be confident
on a solution
All of your thoughts and advice very much appreciated
thanks
Matt

[Anthony]

Post by Matthew Ensor
All of your thoughts and advice very much appreciated

Have you considered plunge milling it for roughing?

Also, how do you like the Mikron?

[Garlicdude]

Post by Matthew Ensor
Hi All,
Just hoping to get peoples thoughts on how to go about this maching problem.
I have a pocket to mill in 316L forged stainless steel 146mm x 146mm x
142.5mm deep with R20mm corner rads. The pocket has been pre-roughed on a
lathe to 136mm dia x 140mm deep
There is a rectangular thro pocket 20mm wide x 120mm long thro at the bottom
of the pocket which is machined in from the opposite side at a previous
operation.
1. Use Iscar's SHRED MILL cutter on an arbor to rough out the pocket
2. Use a HI FEED TRIWORX type design cutter to rough out pocket, utilising
approx 0.7mm DOC with 0.8mm per tooth / per rev feed.
3. Use convential type ripper and finisher cutting tools, multi staging with
diffrent lengths, or via a shell mills on arbors.
4. SUB IT
Spindle is a 40 Taper,10K rpm, T/Coolant, machine new Mikron VCE600
The Shred mill looks a cool idea but it utilises button inserts with the
ripper style knuckle ground into them, so am not sure about the loading on
this. The hi feed cutter (SECO TOOLS) has the right lengths / geometries but
have no experience of these either.
The covential method is possible if not slllllooooowwww and costly.
I have 7 off parts to manufacture approx evey six months, these are very
high value. Billets alone are close to £1000 each. So I need to be confident
on a solution
All of your thoughts and advice very much appreciated
thanks
Matt

Matt, How about drilling with an insert drill and leaving a
thin web between each hole. Then going in and mill with a
rough and finish endmill?

Just a thought.

Best,
Steve

[DanL]

Post by Matthew Ensor
Hi All,
Just hoping to get peoples thoughts on how to go about this maching problem.
I have a pocket to mill in 316L forged stainless steel 146mm x 146mm x
142.5mm deep with R20mm corner rads. The pocket has been pre-roughed on a
lathe to 136mm dia x 140mm deep
There is a rectangular thro pocket 20mm wide x 120mm long thro at the bottom
of the pocket which is machined in from the opposite side at a previous
operation.
1. Use Iscar's SHRED MILL cutter on an arbor to rough out the pocket
2. Use a HI FEED TRIWORX type design cutter to rough out pocket, utilising
approx 0.7mm DOC with 0.8mm per tooth / per rev feed.
3. Use convential type ripper and finisher cutting tools, multi staging with
diffrent lengths, or via a shell mills on arbors.
4. SUB IT
Spindle is a 40 Taper,10K rpm, T/Coolant, machine new Mikron VCE600
The Shred mill looks a cool idea but it utilises button inserts with the
ripper style knuckle ground into them, so am not sure about the loading on
this. The hi feed cutter (SECO TOOLS) has the right lengths / geometries but
have no experience of these either.
The covential method is possible if not slllllooooowwww and costly.
I have 7 off parts to manufacture approx evey six months, these are very
high value. Billets alone are close to £1000 each. So I need to be confident
on a solution
All of your thoughts and advice very much appreciated
thanks
Matt

Matt,

A couple of thoughts:

I don't know how rigid your machine is, but we run an Iscar Feedmill in
316ss pretty regularly. It's a one inch 2 flute cutter that we run dry at
1500 rpms, .030" doc and 90 inches per minute (.030" inch per tooth). We
get better life out of the inserts than we did with any other indexable and
we get 3 indexes per insert as well. The chips are beautiful little amber
colored sixes and nines and with the external air blow chip management is a
non-issue. This job is run on a 40 taper OKK vertical. Cycle time was just
a bit shorter than our previous method using a 1" diam 3 flute indexable
pocketing with a .26" doc.

You've got a pretty deep pocket there so I'd be concerned about chip
management for sure. Re-cutting of chips is going to kill your inserts.
I've never seen the Millshred run, but I'd be wondering what kind of chips
it will produce. I don't think a 20mm wide slot in the bottom will be
enough room for chips to flow out consistently.

If the Seco cutter is anything like the Iscar, which it appears to be by
their website, it should be worth a try. Iscar has the Click-fit line that
allows you to build the cutter to different lengths without losing too much
rigidity. Either way, the radial chip thinning concept truly does work.

Call the Seco or Iscar rep and tell them that you want them to drop off a
cutter body and a couple of inserts to try on guaranteed test. If they know
what they're doing they should want to hang with you and help you dial in
the process.

As previously mentioned, plunge rough might be another idea, but you'll
definitely need high pressure through coolant to get the chips out. We have
done some plunge roughing with Iscars' plunge rougher. I was actually
surprised at how hard our mill was working during the roughing process. Our
OKK is a strong 40 taper so I'm thinking that a steady diet of plunge
roughing 316ss for your brandy-new machine will take it's toll.

But then again, what do I know....


Good luck and keep us posted.

DanL

[Matthew Ensor]

Hi All,

Thanks for all your replies, there all appreciated. I'm going to go with the
SECO tool,as this gives me the advantage of plunging or high feed milling,
or a commbination of both. Ive run some simulations on the CAM, and even by
plunging with a 2.5mm step over, then roughing the bottom of the pocket off
with 0.6mm DOC the cycle time is quick, especially when compared with the
"convential" method.
I've got the tools coming on a sale or return basis so if theres any
problems I'll just send them back.

With reference to the Mikrons we have (Anthony), I rate them highly, we have
four VCE600 pro which is there budget machine but they work all day with
little problems and are very accurate, they easily hold 0.01 dowel hole
pitches.
Service could be better, but so could all the OEM machine manufacturers.

We have recently purchased a Mikron 5 axis machine, which is there new
HPM1000U machine with 20K spindle, 215 tool, all the bells, whistles and
even a kettle I think for making coffee. This a beast of a machine, and have
seen it bieng built in Switzerland.
The main work for this is large aluminium housings machined from solid, and
from the demo's I had in Switzerland its pretty impressive.

You need any more info, email me

Post by DanL

Post by Matthew Ensor
Hi All,
Just hoping to get peoples thoughts on how to go about this maching problem.
I have a pocket to mill in 316L forged stainless steel 146mm x 146mm x
142.5mm deep with R20mm corner rads. The pocket has been pre-roughed on a
lathe to 136mm dia x 140mm deep
There is a rectangular thro pocket 20mm wide x 120mm long thro at the bottom
of the pocket which is machined in from the opposite side at a previous
operation.
1. Use Iscar's SHRED MILL cutter on an arbor to rough out the pocket
2. Use a HI FEED TRIWORX type design cutter to rough out pocket, utilising
approx 0.7mm DOC with 0.8mm per tooth / per rev feed.
3. Use convential type ripper and finisher cutting tools, multi staging with
diffrent lengths, or via a shell mills on arbors.
4. SUB IT
Spindle is a 40 Taper,10K rpm, T/Coolant, machine new Mikron VCE600
The Shred mill looks a cool idea but it utilises button inserts with the
ripper style knuckle ground into them, so am not sure about the loading on
this. The hi feed cutter (SECO TOOLS) has the right lengths / geometries but
have no experience of these either.
The covential method is possible if not slllllooooowwww and costly.
I have 7 off parts to manufacture approx evey six months, these are very
high value. Billets alone are close to £1000 each. So I need to be confident
on a solution
All of your thoughts and advice very much appreciated
thanks
Matt

Matt,
I don't know how rigid your machine is, but we run an Iscar Feedmill in
316ss pretty regularly. It's a one inch 2 flute cutter that we run dry at
1500 rpms, .030" doc and 90 inches per minute (.030" inch per tooth). We
get better life out of the inserts than we did with any other indexable and
we get 3 indexes per insert as well. The chips are beautiful little amber
colored sixes and nines and with the external air blow chip management is a
non-issue. This job is run on a 40 taper OKK vertical. Cycle time was just
a bit shorter than our previous method using a 1" diam 3 flute indexable
pocketing with a .26" doc.
You've got a pretty deep pocket there so I'd be concerned about chip
management for sure. Re-cutting of chips is going to kill your inserts.
I've never seen the Millshred run, but I'd be wondering what kind of chips
it will produce. I don't think a 20mm wide slot in the bottom will be
enough room for chips to flow out consistently.
If the Seco cutter is anything like the Iscar, which it appears to be by
their website, it should be worth a try. Iscar has the Click-fit line that
allows you to build the cutter to different lengths without losing too much
rigidity. Either way, the radial chip thinning concept truly does work.
Call the Seco or Iscar rep and tell them that you want them to drop off a
cutter body and a couple of inserts to try on guaranteed test. If they know
what they're doing they should want to hang with you and help you dial in
the process.
As previously mentioned, plunge rough might be another idea, but you'll
definitely need high pressure through coolant to get the chips out. We have
done some plunge roughing with Iscars' plunge rougher. I was actually
surprised at how hard our mill was working during the roughing process.

Our

Post by DanL
OKK is a strong 40 taper so I'm thinking that a steady diet of plunge
roughing 316ss for your brandy-new machine will take it's toll.
But then again, what do I know....
Good luck and keep us posted.
DanL

[Anthony]

Post by Matthew Ensor
With reference to the Mikrons we have (Anthony), I rate them highly,
we have four VCE600 pro which is there budget machine but they work
all day with little problems and are very accurate, they easily hold
0.01 dowel hole pitches.
Service could be better, but so could all the OEM machine
manufacturers.
We have recently purchased a Mikron 5 axis machine, which is there new
HPM1000U machine with 20K spindle, 215 tool, all the bells, whistles
and even a kettle I think for making coffee. This a beast of a
machine, and have seen it bieng built in Switzerland.
The main work for this is large aluminium housings machined from
solid, and from the demo's I had in Switzerland its pretty impressive.
You need any more info, email me

Matthew,
If it is ok, I am going to have one of the guys who is over this machine
procurement deal to email you. We had them do a demonstration using our
tools and it looked really good. The big question is service and how
often it's needed. We have had extremely bad experiences with DMG.
Also, does the 'at' belong in your email username, or is that a spam
stopper?

[jimz]

Sub it to China.
3 guys with hand drills will drill holes around the premiter
of the pocket, punch it out with a sledge hammer, and
file in the sides. At least 1 person will die in the process.

Guess what ?
It will still be cheaper than
doing it here.

Commie Rats.

[Matthew Ensor]

Hi Guys,


Thanks for all you help, decided to go with the SECO tool. it allows me to
plunge as well as mill with high feed and dmall depth of cut. Will let you
all know how well / bad it goes.
Any more ideas??

China is such a good idea, problem is they will melt the billets down and
reuse for something else no doubt.

Matt

Post by Matthew Ensor
Hi All,
Just hoping to get peoples thoughts on how to go about this maching problem.
I have a pocket to mill in 316L forged stainless steel 146mm x 146mm x
142.5mm deep with R20mm corner rads. The pocket has been pre-roughed on a
lathe to 136mm dia x 140mm deep
There is a rectangular thro pocket 20mm wide x 120mm long thro at the bottom
of the pocket which is machined in from the opposite side at a previous
operation.
1. Use Iscar's SHRED MILL cutter on an arbor to rough out the pocket
2. Use a HI FEED TRIWORX type design cutter to rough out pocket, utilising
approx 0.7mm DOC with 0.8mm per tooth / per rev feed.
3. Use convential type ripper and finisher cutting tools, multi staging with
diffrent lengths, or via a shell mills on arbors.
4. SUB IT
Spindle is a 40 Taper,10K rpm, T/Coolant, machine new Mikron VCE600
The Shred mill looks a cool idea but it utilises button inserts with the
ripper style knuckle ground into them, so am not sure about the loading on
this. The hi feed cutter (SECO TOOLS) has the right lengths / geometries but
have no experience of these either.
The covential method is possible if not slllllooooowwww and costly.
I have 7 off parts to manufacture approx evey six months, these are very
high value. Billets alone are close to £1000 each. So I need to be confident
on a solution
All of your thoughts and advice very much appreciated
thanks
Matt

[Anthony]

Post by Matthew Ensor
Hi Guys,
Thanks for all you help, decided to go with the SECO tool. it allows
me to plunge as well as mill with high feed and dmall depth of cut.
Will let you all know how well / bad it goes.
Any more ideas??
China is such a good idea, problem is they will melt the billets down
and reuse for something else no doubt.

I'd say most (except John, he likes those big, hard stainless jobs) are
just glad it's you and not them with this job. :)