Metalworking (rec.crafts.metalworking) Discuss various aspects of working with metal, such as machining, welding, metal joining, screwing, casting, hardening/tempering, blacksmithing/forging, spinning and hammer work, sheet metal work.

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
  #1   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 1,768
Default Micro Milling 4104HT

I never thought I'd be doing this sort of work ever. I am quite content
to high speed micro mill aluminum. When I was first learning I asked a
lot of questions here and elsewhere. Eventually I put together enough
information to where I can produce satisfactory results most of the time.

When I say micro milling I mean optimizing cut rates with modestly high
speed spindles (24K RPM) and pretty small cutters. Almost no milling
job that I do gets by without a finish pass without atleast a .0625 ball
mill. Quite often I have to use .03125 ball mills to finish some
details. I even have to break out the .0156 stuff once in a while.
That's the range I am talking about when I say micro milling.

For all of that work I use uncoated square end and ball end mills with
6-8% SC520 and water with a constant flood. Cutters last a very long
time and the results are good. Jobs often last for hours. Sometimes a
single tiny little cutter has to work for hours.

Well somebody offered me enough money to tempt me to do some similar
work in 4140HT. I've milled some hardened steels and hard tool steels
before. The numbers say 4140HT should be easier. Its a sort of
compromise. My past experience shows me that a low speed and feed with
an AlTin or TiAlN coated cutter works pretty good. That's fine when you
are pushing a 1/2" 5 flute end mill, but I have to do some of that small
detail work to finish this job. I need to push the envelope with ball
mills as small as .0156 for some of the finish work. I can break it out
so I don't have to finish everything with it, but its still going to
more time than just a few hours. HSM Adviser gives some numbers that
show days instead of weeks, but I wonder if there is anything I can do
to actually get those numbers. With aluminum heat and thermal shock is
not really an issue. With Altin in steal I don't run coolant, but I
admit I do throw a little cutting oil on the part. I've just never done
small or micro milling in harder steel. Well, I have engraved some
knife blades, but that's it.

I'm hoping I can cut down the learning curve, but I am prepared to break
some cutters and ruin some work pieces if I have to. Chip clearance is
probably also going to be an issue. Maybe an air blast to blow chips
clear and see what happens. The thing is we are talking about steel.
Steel chips don't blow clear as easily as aluminum chips.

I am open to any suggestions.

Worst comes to worse I am prepared to tie up my machines for a few
weeks. I certainly figure days even in the best case.

  #2   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 2,163
Default Micro Milling 4104HT


On Fri, 8 Dec 2017 13:02:15 -0700, Bob La Londe
wrote:

I never thought I'd be doing this sort of work ever. I am quite content
to high speed micro mill aluminum. When I was first learning I asked a
lot of questions here and elsewhere. Eventually I put together enough
information to where I can produce satisfactory results most of the time.

When I say micro milling I mean optimizing cut rates with modestly high
speed spindles (24K RPM) and pretty small cutters. Almost no milling
job that I do gets by without a finish pass without atleast a .0625 ball
mill. Quite often I have to use .03125 ball mills to finish some
details. I even have to break out the .0156 stuff once in a while.
That's the range I am talking about when I say micro milling.

For all of that work I use uncoated square end and ball end mills with
6-8% SC520 and water with a constant flood. Cutters last a very long
time and the results are good. Jobs often last for hours. Sometimes a
single tiny little cutter has to work for hours.

Well somebody offered me enough money to tempt me to do some similar
work in 4140HT. I've milled some hardened steels and hard tool steels
before. The numbers say 4140HT should be easier. Its a sort of
compromise. My past experience shows me that a low speed and feed with
an AlTin or TiAlN coated cutter works pretty good. That's fine when you
are pushing a 1/2" 5 flute end mill, but I have to do some of that small
detail work to finish this job. I need to push the envelope with ball
mills as small as .0156 for some of the finish work. I can break it out
so I don't have to finish everything with it, but its still going to
more time than just a few hours. HSM Adviser gives some numbers that
show days instead of weeks, but I wonder if there is anything I can do
to actually get those numbers. With aluminum heat and thermal shock is
not really an issue. With Altin in steal I don't run coolant, but I
admit I do throw a little cutting oil on the part. I've just never done
small or micro milling in harder steel. Well, I have engraved some
knife blades, but that's it.

I'm hoping I can cut down the learning curve, but I am prepared to break
some cutters and ruin some work pieces if I have to. Chip clearance is
probably also going to be an issue. Maybe an air blast to blow chips
clear and see what happens. The thing is we are talking about steel.
Steel chips don't blow clear as easily as aluminum chips.

I am open to any suggestions.

Worst comes to worse I am prepared to tie up my machines for a few
weeks. I certainly figure days even in the best case.

Greetings Bob,
You really need to make sure to get all the chips removed so that
there is no re-cutting of the chips going on. Especially with those
tiny cutters. And the chip load needs to be the same for each flute as
well as enough of a chip load to insure that the flute cuts instead of
pushing away. So your tiny cutters need to run very true. I suggest
you contact the cutter manufacturer for chip load requirements. I
think you should also run coolant or cutting oil. If I was doing this
job I would be using about a 10% water soluble coolant concentration.
And I would try to make sure the coolant flushes away the chips. So
aiming the coolant nozzle correctly can really help.
Eric
  #3   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 1,768
Default Micro Milling 4104HT

On 12/8/2017 2:28 PM, wrote:

On Fri, 8 Dec 2017 13:02:15 -0700, Bob La Londe
wrote:

I never thought I'd be doing this sort of work ever. I am quite content
to high speed micro mill aluminum. When I was first learning I asked a
lot of questions here and elsewhere. Eventually I put together enough
information to where I can produce satisfactory results most of the time.

When I say micro milling I mean optimizing cut rates with modestly high
speed spindles (24K RPM) and pretty small cutters. Almost no milling
job that I do gets by without a finish pass without atleast a .0625 ball
mill. Quite often I have to use .03125 ball mills to finish some
details. I even have to break out the .0156 stuff once in a while.
That's the range I am talking about when I say micro milling.

For all of that work I use uncoated square end and ball end mills with
6-8% SC520 and water with a constant flood. Cutters last a very long
time and the results are good. Jobs often last for hours. Sometimes a
single tiny little cutter has to work for hours.

Well somebody offered me enough money to tempt me to do some similar
work in 4140HT. I've milled some hardened steels and hard tool steels
before. The numbers say 4140HT should be easier. Its a sort of
compromise. My past experience shows me that a low speed and feed with
an AlTin or TiAlN coated cutter works pretty good. That's fine when you
are pushing a 1/2" 5 flute end mill, but I have to do some of that small
detail work to finish this job. I need to push the envelope with ball
mills as small as .0156 for some of the finish work. I can break it out
so I don't have to finish everything with it, but its still going to
more time than just a few hours. HSM Adviser gives some numbers that
show days instead of weeks, but I wonder if there is anything I can do
to actually get those numbers. With aluminum heat and thermal shock is
not really an issue. With Altin in steal I don't run coolant, but I
admit I do throw a little cutting oil on the part. I've just never done
small or micro milling in harder steel. Well, I have engraved some
knife blades, but that's it.

I'm hoping I can cut down the learning curve, but I am prepared to break
some cutters and ruin some work pieces if I have to. Chip clearance is
probably also going to be an issue. Maybe an air blast to blow chips
clear and see what happens. The thing is we are talking about steel.
Steel chips don't blow clear as easily as aluminum chips.

I am open to any suggestions.

Worst comes to worse I am prepared to tie up my machines for a few
weeks. I certainly figure days even in the best case.

Greetings Bob,
You really need to make sure to get all the chips removed so that
there is no re-cutting of the chips going on. Especially with those
tiny cutters. And the chip load needs to be the same for each flute as
well as enough of a chip load to insure that the flute cuts instead of
pushing away. So your tiny cutters need to run very true. I suggest
you contact the cutter manufacturer for chip load requirements. I
think you should also run coolant or cutting oil. If I was doing this
job I would be using about a 10% water soluble coolant concentration.
And I would try to make sure the coolant flushes away the chips. So
aiming the coolant nozzle correctly can really help.
Eric


I've been doing some simulations and with the smallest cutters I am
still looking only 2-7 IPM depending on the cut at full 24K RPM. 7 is
only for light step over with chip thinning turned on in the calculator.
Maybe its time to invest in some 60K spindles just for this type of work.

I swear every day this gets scarier. I just got a request to cut some
graphite molds. I know less about cutting graphite than I do about
cutting steel. LOL. I may pass on that one. I have way to many jobs
on the board right now already that are outside of my comfort zone.

  #4   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 12,529
Default Micro Milling 4104HT

On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe
wrote:

On 12/8/2017 2:28 PM, wrote:

On Fri, 8 Dec 2017 13:02:15 -0700, Bob La Londe
wrote:

I never thought I'd be doing this sort of work ever. I am quite content
to high speed micro mill aluminum. When I was first learning I asked a
lot of questions here and elsewhere. Eventually I put together enough
information to where I can produce satisfactory results most of the time.

When I say micro milling I mean optimizing cut rates with modestly high
speed spindles (24K RPM) and pretty small cutters. Almost no milling
job that I do gets by without a finish pass without atleast a .0625 ball
mill. Quite often I have to use .03125 ball mills to finish some
details. I even have to break out the .0156 stuff once in a while.
That's the range I am talking about when I say micro milling.

For all of that work I use uncoated square end and ball end mills with
6-8% SC520 and water with a constant flood. Cutters last a very long
time and the results are good. Jobs often last for hours. Sometimes a
single tiny little cutter has to work for hours.

Well somebody offered me enough money to tempt me to do some similar
work in 4140HT. I've milled some hardened steels and hard tool steels
before. The numbers say 4140HT should be easier. Its a sort of
compromise. My past experience shows me that a low speed and feed with
an AlTin or TiAlN coated cutter works pretty good. That's fine when you
are pushing a 1/2" 5 flute end mill, but I have to do some of that small
detail work to finish this job. I need to push the envelope with ball
mills as small as .0156 for some of the finish work. I can break it out
so I don't have to finish everything with it, but its still going to
more time than just a few hours. HSM Adviser gives some numbers that
show days instead of weeks, but I wonder if there is anything I can do
to actually get those numbers. With aluminum heat and thermal shock is
not really an issue. With Altin in steal I don't run coolant, but I
admit I do throw a little cutting oil on the part. I've just never done
small or micro milling in harder steel. Well, I have engraved some
knife blades, but that's it.

I'm hoping I can cut down the learning curve, but I am prepared to break
some cutters and ruin some work pieces if I have to. Chip clearance is
probably also going to be an issue. Maybe an air blast to blow chips
clear and see what happens. The thing is we are talking about steel.
Steel chips don't blow clear as easily as aluminum chips.

I am open to any suggestions.

Worst comes to worse I am prepared to tie up my machines for a few
weeks. I certainly figure days even in the best case.

Greetings Bob,
You really need to make sure to get all the chips removed so that
there is no re-cutting of the chips going on. Especially with those
tiny cutters. And the chip load needs to be the same for each flute as
well as enough of a chip load to insure that the flute cuts instead of
pushing away. So your tiny cutters need to run very true. I suggest
you contact the cutter manufacturer for chip load requirements. I
think you should also run coolant or cutting oil. If I was doing this
job I would be using about a 10% water soluble coolant concentration.
And I would try to make sure the coolant flushes away the chips. So
aiming the coolant nozzle correctly can really help.
Eric


I've been doing some simulations and with the smallest cutters I am
still looking only 2-7 IPM depending on the cut at full 24K RPM. 7 is
only for light step over with chip thinning turned on in the calculator.
Maybe its time to invest in some 60K spindles just for this type of work.

I swear every day this gets scarier. I just got a request to cut some
graphite molds. I know less about cutting graphite than I do about
cutting steel. LOL. I may pass on that one. I have way to many jobs
on the board right now already that are outside of my comfort zone.


If you haven't machined it, it's a piece of cake. Do you know what
grade it is? Brand?

Most are very abrasive but you can go as fast as your spindle will
allow. It machines more easily than magnesium. I machined a lot of
thread-cutting electrodes from Poco 3 graphite a few decades ago
Easy-peasy. Don't be afraid of it.

--
Ed Huntress
  #5   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 45
Default Micro Milling 4104HT

On 12/08/2017 05:43 PM, Ed Huntress wrote:
On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe
wrote:
If you haven't machined it, it's a piece of cake. Do you know what
grade it is? Brand?

Most are very abrasive but you can go as fast as your spindle will
allow. It machines more easily than magnesium. I machined a lot of
thread-cutting electrodes from Poco 3 graphite a few decades ago
Easy-peasy. Don't be afraid of it.


Wicked messy though. Graphite dust everywhere. I bought some equipment
from a shop that did a lot of graphite machining and it was a dusty mess.


  #6   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 12,529
Default Micro Milling 4104HT

On Fri, 8 Dec 2017 20:46:47 -0700, BobH
wrote:

On 12/08/2017 05:43 PM, Ed Huntress wrote:
On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe
wrote:
If you haven't machined it, it's a piece of cake. Do you know what
grade it is? Brand?

Most are very abrasive but you can go as fast as your spindle will
allow. It machines more easily than magnesium. I machined a lot of
thread-cutting electrodes from Poco 3 graphite a few decades ago
Easy-peasy. Don't be afraid of it.


Wicked messy though. Graphite dust everywhere. I bought some equipment
from a shop that did a lot of graphite machining and it was a dusty mess.


Despite the common understanding about graphite, the synthetic
variety, used in the applications we're describing, is very abrasive.
It's coarse and gritty, rather than slippery flakes, which is the
typical structure of natural graphite.

I've been in shops that specialize in machining graphite EDM
electrodes and they replace machines every two or three years. They
often buy Fadals for that reason: they're cheap, and nothing else will
last longer, unless the machine is built for it.

I marketed Roku-Roku for a couple of years. They were pioneers in
building machining centers specifically made for machining graphite.
They have a three-part approach to keeping graphite off the ways.

First, they have special way covers. Second, the area under the covers
has pressurized air to keep graphite dust from entering. And third,
they have a built-in high-volume vacuum system to suck the dust out of
the complete machine enclosure.

As I said, I used to turn threading electrodes for an EDM company, and
I'm serious about protecting the ways on my lathe. First, I don't
machine much graphite. Second, I cover the ways with oil-soaked
(WD-40-sprayed) newspaper, taped on tightly. Third, I cover areas with
aluminum foil if I can't get newspaper around them. And fourth, I make
a vacuusm plenum out of an old plastic milk bottle, attach a vacuum
hose to it, and cut a hole in it that allows you to fit it closely
around the cutting tool and the workpiece.

If you're going to do much of it, you really have to protect your
machine. But machining it is really easy, requiring little force. It
will wear HSS pretty quickly, however.

--
Ed Huntress
  #7   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 1,768
Default Micro Milling 4104HT

On 12/9/2017 4:32 AM, Ed Huntress wrote:
On Fri, 8 Dec 2017 20:46:47 -0700, BobH
wrote:

On 12/08/2017 05:43 PM, Ed Huntress wrote:
On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe
wrote:
If you haven't machined it, it's a piece of cake. Do you know what
grade it is? Brand?

Most are very abrasive but you can go as fast as your spindle will
allow. It machines more easily than magnesium. I machined a lot of
thread-cutting electrodes from Poco 3 graphite a few decades ago
Easy-peasy. Don't be afraid of it.


Wicked messy though. Graphite dust everywhere. I bought some equipment
from a shop that did a lot of graphite machining and it was a dusty mess.


Despite the common understanding about graphite, the synthetic
variety, used in the applications we're describing, is very abrasive.
It's coarse and gritty, rather than slippery flakes, which is the
typical structure of natural graphite.

I've been in shops that specialize in machining graphite EDM
electrodes and they replace machines every two or three years. They
often buy Fadals for that reason: they're cheap, and nothing else will
last longer, unless the machine is built for it.

I marketed Roku-Roku for a couple of years. They were pioneers in
building machining centers specifically made for machining graphite.
They have a three-part approach to keeping graphite off the ways.

First, they have special way covers. Second, the area under the covers
has pressurized air to keep graphite dust from entering. And third,
they have a built-in high-volume vacuum system to suck the dust out of
the complete machine enclosure.

As I said, I used to turn threading electrodes for an EDM company, and
I'm serious about protecting the ways on my lathe. First, I don't
machine much graphite. Second, I cover the ways with oil-soaked
(WD-40-sprayed) newspaper, taped on tightly. Third, I cover areas with
aluminum foil if I can't get newspaper around them. And fourth, I make
a vacuusm plenum out of an old plastic milk bottle, attach a vacuum
hose to it, and cut a hole in it that allows you to fit it closely
around the cutting tool and the workpiece.

If you're going to do much of it, you really have to protect your
machine. But machining it is really easy, requiring little force. It
will wear HSS pretty quickly, however.



Sounds like for my shop the way to go might be to dedicate a cheap
easily rebuildable & easily discardable small CNC router for the
application. Put it in a box with light negative pressure (cheap shop
vac) and call it a day.

I don't really use any HSS except for hand ground lathe bits, drill
bits, and one specialty HSS lathe insert.

I have a little less than a small fortune in carbide mills on hand.








  #8   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 12,529
Default Micro Milling 4104HT

On Sat, 9 Dec 2017 09:45:55 -0700, Bob La Londe
wrote:

On 12/9/2017 4:32 AM, Ed Huntress wrote:
On Fri, 8 Dec 2017 20:46:47 -0700, BobH
wrote:

On 12/08/2017 05:43 PM, Ed Huntress wrote:
On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe
wrote:
If you haven't machined it, it's a piece of cake. Do you know what
grade it is? Brand?

Most are very abrasive but you can go as fast as your spindle will
allow. It machines more easily than magnesium. I machined a lot of
thread-cutting electrodes from Poco 3 graphite a few decades ago
Easy-peasy. Don't be afraid of it.


Wicked messy though. Graphite dust everywhere. I bought some equipment
from a shop that did a lot of graphite machining and it was a dusty mess.


Despite the common understanding about graphite, the synthetic
variety, used in the applications we're describing, is very abrasive.
It's coarse and gritty, rather than slippery flakes, which is the
typical structure of natural graphite.

I've been in shops that specialize in machining graphite EDM
electrodes and they replace machines every two or three years. They
often buy Fadals for that reason: they're cheap, and nothing else will
last longer, unless the machine is built for it.

I marketed Roku-Roku for a couple of years. They were pioneers in
building machining centers specifically made for machining graphite.
They have a three-part approach to keeping graphite off the ways.

First, they have special way covers. Second, the area under the covers
has pressurized air to keep graphite dust from entering. And third,
they have a built-in high-volume vacuum system to suck the dust out of
the complete machine enclosure.

As I said, I used to turn threading electrodes for an EDM company, and
I'm serious about protecting the ways on my lathe. First, I don't
machine much graphite. Second, I cover the ways with oil-soaked
(WD-40-sprayed) newspaper, taped on tightly. Third, I cover areas with
aluminum foil if I can't get newspaper around them. And fourth, I make
a vacuusm plenum out of an old plastic milk bottle, attach a vacuum
hose to it, and cut a hole in it that allows you to fit it closely
around the cutting tool and the workpiece.

If you're going to do much of it, you really have to protect your
machine. But machining it is really easy, requiring little force. It
will wear HSS pretty quickly, however.



Sounds like for my shop the way to go might be to dedicate a cheap
easily rebuildable & easily discardable small CNC router for the
application. Put it in a box with light negative pressure (cheap shop
vac) and call it a day.


'Sounds reasonable.


I don't really use any HSS except for hand ground lathe bits, drill
bits, and one specialty HSS lathe insert.

I have a little less than a small fortune in carbide mills on hand.


Non-specialists use carbide. Specialists use diamond. Most machining
of graphite today probably is done in EDM shops, where the volumes are
not really large, and I've seen mostly carbide.

I used carbide on my SB 10L, and that machine does not like carbide
for turning steel. But the forces are quite low when machining
graphite -- if you try to take too big a bite it can crack -- and
machine rigidity is not much of an issue, except for the brittleness
of the workpiece.

Speeds are, basically, whatever ya' got. Feedrates are moderate, so
the tool doesn't climb and crack the work.

If you want some tips, you can call Poco Graphite. They're very
helpful and very expert.

--
Ed Huntress
  #9   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 5,888
Default Micro Milling 4104HT

"Ed Huntress" wrote in message
...
On Sat, 9 Dec 2017 09:45:55 -0700, Bob La Londe
wrote:

On 12/9/2017 4:32 AM, Ed Huntress wrote:
On Fri, 8 Dec 2017 20:46:47 -0700, BobH
wrote:

On 12/08/2017 05:43 PM, Ed Huntress wrote:
On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe

wrote:
If you haven't machined it, it's a piece of cake. Do you know
what
grade it is? Brand?

Most are very abrasive but you can go as fast as your spindle
will
allow. It machines more easily than magnesium. I machined a lot
of
thread-cutting electrodes from Poco 3 graphite a few decades ago
Easy-peasy. Don't be afraid of it.


Wicked messy though. Graphite dust everywhere. I bought some
equipment
from a shop that did a lot of graphite machining and it was a
dusty mess.

Despite the common understanding about graphite, the synthetic
variety, used in the applications we're describing, is very
abrasive.
It's coarse and gritty, rather than slippery flakes, which is the
typical structure of natural graphite.

I've been in shops that specialize in machining graphite EDM
electrodes and they replace machines every two or three years.
They
often buy Fadals for that reason: they're cheap, and nothing else
will
last longer, unless the machine is built for it.

I marketed Roku-Roku for a couple of years. They were pioneers in
building machining centers specifically made for machining
graphite.
They have a three-part approach to keeping graphite off the ways.

First, they have special way covers. Second, the area under the
covers
has pressurized air to keep graphite dust from entering. And
third,
they have a built-in high-volume vacuum system to suck the dust
out of
the complete machine enclosure.

As I said, I used to turn threading electrodes for an EDM company,
and
I'm serious about protecting the ways on my lathe. First, I don't
machine much graphite. Second, I cover the ways with oil-soaked
(WD-40-sprayed) newspaper, taped on tightly. Third, I cover areas
with
aluminum foil if I can't get newspaper around them. And fourth, I
make
a vacuusm plenum out of an old plastic milk bottle, attach a
vacuum
hose to it, and cut a hole in it that allows you to fit it closely
around the cutting tool and the workpiece.

If you're going to do much of it, you really have to protect your
machine. But machining it is really easy, requiring little force.
It
will wear HSS pretty quickly, however.



Sounds like for my shop the way to go might be to dedicate a cheap
easily rebuildable & easily discardable small CNC router for the
application. Put it in a box with light negative pressure (cheap
shop
vac) and call it a day.


'Sounds reasonable.


I don't really use any HSS except for hand ground lathe bits, drill
bits, and one specialty HSS lathe insert.

I have a little less than a small fortune in carbide mills on hand.


Non-specialists use carbide. Specialists use diamond. Most machining
of graphite today probably is done in EDM shops, where the volumes
are
not really large, and I've seen mostly carbide.

I used carbide on my SB 10L, and that machine does not like carbide
for turning steel. But the forces are quite low when machining
graphite -- if you try to take too big a bite it can crack -- and
machine rigidity is not much of an issue, except for the brittleness
of the workpiece.

Speeds are, basically, whatever ya' got. Feedrates are moderate, so
the tool doesn't climb and crack the work.

If you want some tips, you can call Poco Graphite. They're very
helpful and very expert.

--
Ed Huntress


When I milled carbon brushes for a Variac I found that I had to always
cut into the edge,
the material would crack off very easily where the cutting edge
exited. OTOH climb milling wasn't a problem.
-jsw


  #10   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 12,529
Default Micro Milling 4104HT

On Sat, 9 Dec 2017 12:34:45 -0500, "Jim Wilkins"
wrote:

"Ed Huntress" wrote in message
.. .
On Sat, 9 Dec 2017 09:45:55 -0700, Bob La Londe
wrote:

On 12/9/2017 4:32 AM, Ed Huntress wrote:
On Fri, 8 Dec 2017 20:46:47 -0700, BobH
wrote:

On 12/08/2017 05:43 PM, Ed Huntress wrote:
On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe

wrote:
If you haven't machined it, it's a piece of cake. Do you know
what
grade it is? Brand?

Most are very abrasive but you can go as fast as your spindle
will
allow. It machines more easily than magnesium. I machined a lot
of
thread-cutting electrodes from Poco 3 graphite a few decades ago
Easy-peasy. Don't be afraid of it.


Wicked messy though. Graphite dust everywhere. I bought some
equipment
from a shop that did a lot of graphite machining and it was a
dusty mess.

Despite the common understanding about graphite, the synthetic
variety, used in the applications we're describing, is very
abrasive.
It's coarse and gritty, rather than slippery flakes, which is the
typical structure of natural graphite.

I've been in shops that specialize in machining graphite EDM
electrodes and they replace machines every two or three years.
They
often buy Fadals for that reason: they're cheap, and nothing else
will
last longer, unless the machine is built for it.

I marketed Roku-Roku for a couple of years. They were pioneers in
building machining centers specifically made for machining
graphite.
They have a three-part approach to keeping graphite off the ways.

First, they have special way covers. Second, the area under the
covers
has pressurized air to keep graphite dust from entering. And
third,
they have a built-in high-volume vacuum system to suck the dust
out of
the complete machine enclosure.

As I said, I used to turn threading electrodes for an EDM company,
and
I'm serious about protecting the ways on my lathe. First, I don't
machine much graphite. Second, I cover the ways with oil-soaked
(WD-40-sprayed) newspaper, taped on tightly. Third, I cover areas
with
aluminum foil if I can't get newspaper around them. And fourth, I
make
a vacuusm plenum out of an old plastic milk bottle, attach a
vacuum
hose to it, and cut a hole in it that allows you to fit it closely
around the cutting tool and the workpiece.

If you're going to do much of it, you really have to protect your
machine. But machining it is really easy, requiring little force.
It
will wear HSS pretty quickly, however.



Sounds like for my shop the way to go might be to dedicate a cheap
easily rebuildable & easily discardable small CNC router for the
application. Put it in a box with light negative pressure (cheap
shop
vac) and call it a day.


'Sounds reasonable.


I don't really use any HSS except for hand ground lathe bits, drill
bits, and one specialty HSS lathe insert.

I have a little less than a small fortune in carbide mills on hand.


Non-specialists use carbide. Specialists use diamond. Most machining
of graphite today probably is done in EDM shops, where the volumes
are
not really large, and I've seen mostly carbide.

I used carbide on my SB 10L, and that machine does not like carbide
for turning steel. But the forces are quite low when machining
graphite -- if you try to take too big a bite it can crack -- and
machine rigidity is not much of an issue, except for the brittleness
of the workpiece.

Speeds are, basically, whatever ya' got. Feedrates are moderate, so
the tool doesn't climb and crack the work.

If you want some tips, you can call Poco Graphite. They're very
helpful and very expert.

--
Ed Huntress


When I milled carbon brushes for a Variac I found that I had to always
cut into the edge,
the material would crack off very easily where the cutting edge
exited. OTOH climb milling wasn't a problem.
-jsw


Yeah, it can be a little tricky. A lot has to do with the quality of
graphite you're using. Poco 3 is an industry standard for high-quality
electrodes. It's more resistant to chipping and cracking than the
cheaper stuff.

--
Ed Huntress


  #11   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 12,529
Default Micro Milling 4104HT

On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe
wrote:

On 12/8/2017 2:28 PM, wrote:

On Fri, 8 Dec 2017 13:02:15 -0700, Bob La Londe
wrote:

I never thought I'd be doing this sort of work ever. I am quite content
to high speed micro mill aluminum. When I was first learning I asked a
lot of questions here and elsewhere. Eventually I put together enough
information to where I can produce satisfactory results most of the time.

When I say micro milling I mean optimizing cut rates with modestly high
speed spindles (24K RPM) and pretty small cutters. Almost no milling
job that I do gets by without a finish pass without atleast a .0625 ball
mill. Quite often I have to use .03125 ball mills to finish some
details. I even have to break out the .0156 stuff once in a while.
That's the range I am talking about when I say micro milling.

For all of that work I use uncoated square end and ball end mills with
6-8% SC520 and water with a constant flood. Cutters last a very long
time and the results are good. Jobs often last for hours. Sometimes a
single tiny little cutter has to work for hours.

Well somebody offered me enough money to tempt me to do some similar
work in 4140HT. I've milled some hardened steels and hard tool steels
before. The numbers say 4140HT should be easier. Its a sort of
compromise. My past experience shows me that a low speed and feed with
an AlTin or TiAlN coated cutter works pretty good. That's fine when you
are pushing a 1/2" 5 flute end mill, but I have to do some of that small
detail work to finish this job. I need to push the envelope with ball
mills as small as .0156 for some of the finish work. I can break it out
so I don't have to finish everything with it, but its still going to
more time than just a few hours. HSM Adviser gives some numbers that
show days instead of weeks, but I wonder if there is anything I can do
to actually get those numbers. With aluminum heat and thermal shock is
not really an issue. With Altin in steal I don't run coolant, but I
admit I do throw a little cutting oil on the part. I've just never done
small or micro milling in harder steel. Well, I have engraved some
knife blades, but that's it.

I'm hoping I can cut down the learning curve, but I am prepared to break
some cutters and ruin some work pieces if I have to. Chip clearance is
probably also going to be an issue. Maybe an air blast to blow chips
clear and see what happens. The thing is we are talking about steel.
Steel chips don't blow clear as easily as aluminum chips.

I am open to any suggestions.

Worst comes to worse I am prepared to tie up my machines for a few
weeks. I certainly figure days even in the best case.

Greetings Bob,
You really need to make sure to get all the chips removed so that
there is no re-cutting of the chips going on. Especially with those
tiny cutters. And the chip load needs to be the same for each flute as
well as enough of a chip load to insure that the flute cuts instead of
pushing away. So your tiny cutters need to run very true. I suggest
you contact the cutter manufacturer for chip load requirements. I
think you should also run coolant or cutting oil. If I was doing this
job I would be using about a 10% water soluble coolant concentration.
And I would try to make sure the coolant flushes away the chips. So
aiming the coolant nozzle correctly can really help.
Eric


I've been doing some simulations and with the smallest cutters I am
still looking only 2-7 IPM depending on the cut at full 24K RPM. 7 is
only for light step over with chip thinning turned on in the calculator.
Maybe its time to invest in some 60K spindles just for this type of work.

I swear every day this gets scarier. I just got a request to cut some
graphite molds. I know less about cutting graphite than I do about
cutting steel. LOL. I may pass on that one. I have way to many jobs
on the board right now already that are outside of my comfort zone.


I should have asked what types of molds these are. Poco has some
online articles about graphite molds.

http://poco.com/IndustriesApplications.aspx

--
Ed Huntress
  #12   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 1,768
Default Micro Milling 4104HT

On 12/9/2017 10:42 AM, Ed Huntress wrote:
On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe
wrote:

On 12/8/2017 2:28 PM, wrote:

On Fri, 8 Dec 2017 13:02:15 -0700, Bob La Londe
wrote:

I never thought I'd be doing this sort of work ever. I am quite content
to high speed micro mill aluminum. When I was first learning I asked a
lot of questions here and elsewhere. Eventually I put together enough
information to where I can produce satisfactory results most of the time.

When I say micro milling I mean optimizing cut rates with modestly high
speed spindles (24K RPM) and pretty small cutters. Almost no milling
job that I do gets by without a finish pass without atleast a .0625 ball
mill. Quite often I have to use .03125 ball mills to finish some
details. I even have to break out the .0156 stuff once in a while.
That's the range I am talking about when I say micro milling.

For all of that work I use uncoated square end and ball end mills with
6-8% SC520 and water with a constant flood. Cutters last a very long
time and the results are good. Jobs often last for hours. Sometimes a
single tiny little cutter has to work for hours.

Well somebody offered me enough money to tempt me to do some similar
work in 4140HT. I've milled some hardened steels and hard tool steels
before. The numbers say 4140HT should be easier. Its a sort of
compromise. My past experience shows me that a low speed and feed with
an AlTin or TiAlN coated cutter works pretty good. That's fine when you
are pushing a 1/2" 5 flute end mill, but I have to do some of that small
detail work to finish this job. I need to push the envelope with ball
mills as small as .0156 for some of the finish work. I can break it out
so I don't have to finish everything with it, but its still going to
more time than just a few hours. HSM Adviser gives some numbers that
show days instead of weeks, but I wonder if there is anything I can do
to actually get those numbers. With aluminum heat and thermal shock is
not really an issue. With Altin in steal I don't run coolant, but I
admit I do throw a little cutting oil on the part. I've just never done
small or micro milling in harder steel. Well, I have engraved some
knife blades, but that's it.

I'm hoping I can cut down the learning curve, but I am prepared to break
some cutters and ruin some work pieces if I have to. Chip clearance is
probably also going to be an issue. Maybe an air blast to blow chips
clear and see what happens. The thing is we are talking about steel.
Steel chips don't blow clear as easily as aluminum chips.

I am open to any suggestions.

Worst comes to worse I am prepared to tie up my machines for a few
weeks. I certainly figure days even in the best case.
Greetings Bob,
You really need to make sure to get all the chips removed so that
there is no re-cutting of the chips going on. Especially with those
tiny cutters. And the chip load needs to be the same for each flute as
well as enough of a chip load to insure that the flute cuts instead of
pushing away. So your tiny cutters need to run very true. I suggest
you contact the cutter manufacturer for chip load requirements. I
think you should also run coolant or cutting oil. If I was doing this
job I would be using about a 10% water soluble coolant concentration.
And I would try to make sure the coolant flushes away the chips. So
aiming the coolant nozzle correctly can really help.
Eric


I've been doing some simulations and with the smallest cutters I am
still looking only 2-7 IPM depending on the cut at full 24K RPM. 7 is
only for light step over with chip thinning turned on in the calculator.
Maybe its time to invest in some 60K spindles just for this type of work.

I swear every day this gets scarier. I just got a request to cut some
graphite molds. I know less about cutting graphite than I do about
cutting steel. LOL. I may pass on that one. I have way to many jobs
on the board right now already that are outside of my comfort zone.


I should have asked what types of molds these are. Poco has some
online articles about graphite molds.

http://poco.com/IndustriesApplications.aspx


I probably won't get this one with the graphite. I threw a price at
them that covered my learning curve, and they said they were going to do
some more research.


  #13   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 2,163
Default Micro Milling 4104HT

On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe
wrote:

On 12/8/2017 2:28 PM, wrote:

On Fri, 8 Dec 2017 13:02:15 -0700, Bob La Londe
wrote:

I never thought I'd be doing this sort of work ever. I am quite content
to high speed micro mill aluminum. When I was first learning I asked a
lot of questions here and elsewhere. Eventually I put together enough
information to where I can produce satisfactory results most of the time.

When I say micro milling I mean optimizing cut rates with modestly high
speed spindles (24K RPM) and pretty small cutters. Almost no milling
job that I do gets by without a finish pass without atleast a .0625 ball
mill. Quite often I have to use .03125 ball mills to finish some
details. I even have to break out the .0156 stuff once in a while.
That's the range I am talking about when I say micro milling.

For all of that work I use uncoated square end and ball end mills with
6-8% SC520 and water with a constant flood. Cutters last a very long
time and the results are good. Jobs often last for hours. Sometimes a
single tiny little cutter has to work for hours.

Well somebody offered me enough money to tempt me to do some similar
work in 4140HT. I've milled some hardened steels and hard tool steels
before. The numbers say 4140HT should be easier. Its a sort of
compromise. My past experience shows me that a low speed and feed with
an AlTin or TiAlN coated cutter works pretty good. That's fine when you
are pushing a 1/2" 5 flute end mill, but I have to do some of that small
detail work to finish this job. I need to push the envelope with ball
mills as small as .0156 for some of the finish work. I can break it out
so I don't have to finish everything with it, but its still going to
more time than just a few hours. HSM Adviser gives some numbers that
show days instead of weeks, but I wonder if there is anything I can do
to actually get those numbers. With aluminum heat and thermal shock is
not really an issue. With Altin in steal I don't run coolant, but I
admit I do throw a little cutting oil on the part. I've just never done
small or micro milling in harder steel. Well, I have engraved some
knife blades, but that's it.

I'm hoping I can cut down the learning curve, but I am prepared to break
some cutters and ruin some work pieces if I have to. Chip clearance is
probably also going to be an issue. Maybe an air blast to blow chips
clear and see what happens. The thing is we are talking about steel.
Steel chips don't blow clear as easily as aluminum chips.

I am open to any suggestions.

Worst comes to worse I am prepared to tie up my machines for a few
weeks. I certainly figure days even in the best case.

Greetings Bob,
You really need to make sure to get all the chips removed so that
there is no re-cutting of the chips going on. Especially with those
tiny cutters. And the chip load needs to be the same for each flute as
well as enough of a chip load to insure that the flute cuts instead of
pushing away. So your tiny cutters need to run very true. I suggest
you contact the cutter manufacturer for chip load requirements. I
think you should also run coolant or cutting oil. If I was doing this
job I would be using about a 10% water soluble coolant concentration.
And I would try to make sure the coolant flushes away the chips. So
aiming the coolant nozzle correctly can really help.
Eric


I've been doing some simulations and with the smallest cutters I am
still looking only 2-7 IPM depending on the cut at full 24K RPM. 7 is
only for light step over with chip thinning turned on in the calculator.
Maybe its time to invest in some 60K spindles just for this type of work.

I swear every day this gets scarier. I just got a request to cut some
graphite molds. I know less about cutting graphite than I do about
cutting steel. LOL. I may pass on that one. I have way to many jobs
on the board right now already that are outside of my comfort zone.

Yeah, more jobs can get scarier. Especially when new materials are
considered. Graphite is one material I myself would avoid because it
is so abrasive and dirty. I know this because I have machined it
before.
Because you are machining with small cutters at high speeds you
might be interested in this web site:
http://www.precisebits.com/ .
Then again you may already know about it. If you don't then if you
visit the site you will discover a good source of knowledge regarding
high rpm cutting with tiny tools. I called them once with a question
and had a quite informative discussion and so learned some good stuff.
Cheers,
Eric
  #14   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 1,768
Default Micro Milling 4104HT

On 12/10/2017 12:19 PM, wrote:
On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe
wrote:

On 12/8/2017 2:28 PM,
wrote:

On Fri, 8 Dec 2017 13:02:15 -0700, Bob La Londe
wrote:

I never thought I'd be doing this sort of work ever. I am quite content
to high speed micro mill aluminum. When I was first learning I asked a
lot of questions here and elsewhere. Eventually I put together enough
information to where I can produce satisfactory results most of the time.

When I say micro milling I mean optimizing cut rates with modestly high
speed spindles (24K RPM) and pretty small cutters. Almost no milling
job that I do gets by without a finish pass without atleast a .0625 ball
mill. Quite often I have to use .03125 ball mills to finish some
details. I even have to break out the .0156 stuff once in a while.
That's the range I am talking about when I say micro milling.

For all of that work I use uncoated square end and ball end mills with
6-8% SC520 and water with a constant flood. Cutters last a very long
time and the results are good. Jobs often last for hours. Sometimes a
single tiny little cutter has to work for hours.

Well somebody offered me enough money to tempt me to do some similar
work in 4140HT. I've milled some hardened steels and hard tool steels
before. The numbers say 4140HT should be easier. Its a sort of
compromise. My past experience shows me that a low speed and feed with
an AlTin or TiAlN coated cutter works pretty good. That's fine when you
are pushing a 1/2" 5 flute end mill, but I have to do some of that small
detail work to finish this job. I need to push the envelope with ball
mills as small as .0156 for some of the finish work. I can break it out
so I don't have to finish everything with it, but its still going to
more time than just a few hours. HSM Adviser gives some numbers that
show days instead of weeks, but I wonder if there is anything I can do
to actually get those numbers. With aluminum heat and thermal shock is
not really an issue. With Altin in steal I don't run coolant, but I
admit I do throw a little cutting oil on the part. I've just never done
small or micro milling in harder steel. Well, I have engraved some
knife blades, but that's it.

I'm hoping I can cut down the learning curve, but I am prepared to break
some cutters and ruin some work pieces if I have to. Chip clearance is
probably also going to be an issue. Maybe an air blast to blow chips
clear and see what happens. The thing is we are talking about steel.
Steel chips don't blow clear as easily as aluminum chips.

I am open to any suggestions.

Worst comes to worse I am prepared to tie up my machines for a few
weeks. I certainly figure days even in the best case.
Greetings Bob,
You really need to make sure to get all the chips removed so that
there is no re-cutting of the chips going on. Especially with those
tiny cutters. And the chip load needs to be the same for each flute as
well as enough of a chip load to insure that the flute cuts instead of
pushing away. So your tiny cutters need to run very true. I suggest
you contact the cutter manufacturer for chip load requirements. I
think you should also run coolant or cutting oil. If I was doing this
job I would be using about a 10% water soluble coolant concentration.
And I would try to make sure the coolant flushes away the chips. So
aiming the coolant nozzle correctly can really help.
Eric


I've been doing some simulations and with the smallest cutters I am
still looking only 2-7 IPM depending on the cut at full 24K RPM. 7 is
only for light step over with chip thinning turned on in the calculator.
Maybe its time to invest in some 60K spindles just for this type of work.

I swear every day this gets scarier. I just got a request to cut some
graphite molds. I know less about cutting graphite than I do about
cutting steel. LOL. I may pass on that one. I have way to many jobs
on the board right now already that are outside of my comfort zone.

Yeah, more jobs can get scarier. Especially when new materials are
considered. Graphite is one material I myself would avoid because it
is so abrasive and dirty. I know this because I have machined it
before.
Because you are machining with small cutters at high speeds you
might be interested in this web site:
http://www.precisebits.com/ .
Then again you may already know about it. If you don't then if you
visit the site you will discover a good source of knowledge regarding
high rpm cutting with tiny tools. I called them once with a question
and had a quite informative discussion and so learned some good stuff.
Cheers,
Eric


Yeah, Ron is a really good guy and pretyt knowledgable about small
cutters. Ages ago was using his collets in a Bosch Colt trim router
for milling aluminum. I burned a few of those routers. Still have one
mounted on my little CNC router.

As far as graphite, as I mentioned in another post, my plan if I had
gotten that job was to use my little (almost throw away) Chinese noodle
(limp like a noddle) router. If I ate the whole thing up a decent size
job would pay for another one. On my short list of plans is to make a
little better frame and move what's good on that router over to the new
frame. I'd lay the machine out on my surface plate and I'd be able to
replace any of the cheap parts even faster and easier than it is now. I
already have it in a box. I could slap some doors on it, and put some
vacuum in there with a shop vac to keep the graphite out of the shop. I
had doors on the box before, and they are laying around somewhere.

Only part that would not be super cheap to replace quickly and easily is
the YZ motors. The X can actually be outside of the box when I rebuild
it.


  #15   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 10,399
Default Micro Milling 4104HT

On Fri, 8 Dec 2017 20:46:47 -0700, BobH
wrote:

On 12/08/2017 05:43 PM, Ed Huntress wrote:
On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe
wrote:
If you haven't machined it, it's a piece of cake. Do you know what
grade it is? Brand?

Most are very abrasive but you can go as fast as your spindle will
allow. It machines more easily than magnesium. I machined a lot of
thread-cutting electrodes from Poco 3 graphite a few decades ago
Easy-peasy. Don't be afraid of it.


Wicked messy though. Graphite dust everywhere. I bought some equipment
from a shop that did a lot of graphite machining and it was a dusty mess.


If you are going to cut graphite...first thing you need is a fully
enclosed work space on your table. Second thing you need is a HEPA
filter on the vac system you install to get the dust OUT of your shop.

Third thing..is a separate room to do the work in..preferably one not
attached to the rest of your shop. That **** tracks like the plague.


---
This email has been checked for viruses by Avast antivirus software.
https://www.avast.com/antivirus



  #16   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 1,768
Default Micro Milling 4104HT

On 12/8/2017 1:02 PM, Bob La Londe wrote:
I never thought I'd be doing this sort of work ever.Â* I am quite content
to high speed micro mill aluminum.Â* When I was first learning I asked a
lot of questions here and elsewhere.Â* Eventually I put together enough
information to where I can produce satisfactory results most of the time.

When I say micro milling I mean optimizing cut rates with modestly high
speed spindles (24K RPM) and pretty small cutters.Â* Almost no milling
job that I do gets by without a finish pass without atleast a .0625 ball
mill.Â* Quite often I have to use .03125 ball mills to finish some
details.Â* I even have to break out the .0156 stuff once in a while.
That's the range I am talking about when I say micro milling.

For all of that work I use uncoated square end and ball end mills with
6-8% SC520 and water with a constant flood.Â* Cutters last a very long
time and the results are good.Â* Jobs often last for hours.Â* Sometimes a
single tiny little cutter has to work for hours.

Well somebody offered me enough money to tempt me to do some similar
work in 4140HT.Â* I've milled some hardened steels and hard tool steels
before.Â* The numbers say 4140HT should be easier.Â* Its a sort of
compromise.Â* My past experience shows me that a low speed and feed with
an AlTin or TiAlN coated cutter works pretty good.Â* That's fine when you
are pushing a 1/2" 5 flute end mill, but I have to do some of that small
detail work to finish this job.Â* I need to push the envelope with ball
mills as small as .0156 for some of the finish work.Â* I can break it out
so I don't have to finish everything with it, but its still going to
more time than just a few hours.Â* HSM Adviser gives some numbers that
show days instead of weeks, but I wonder if there is anything I can do
to actually get those numbers.Â* With aluminum heat and thermal shock is
not really an issue.Â* With Altin in steal I don't run coolant, but I
admit I do throw a little cutting oil on the part.Â* I've just never done
small or micro milling in harder steel.Â* Well, I have engraved some
knife blades, but that's it.

I'm hoping I can cut down the learning curve, but I am prepared to break
some cutters and ruin some work pieces if I have to.Â* Chip clearance is
probably also going to be an issue.Â* Maybe an air blast to blow chips
clear and see what happens.Â* The thing is we are talking about steel.
Steel chips don't blow clear as easily as aluminum chips.

I am open to any suggestions.

Worst comes to worse I am prepared to tie up my machines for a few
weeks.Â* I certainly figure days even in the best case.


Well I just started breaking down stock for this job. I don't know how
its going to micro machines, but regular machining should go just fine
based on the way it saw cuts.


  #17   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 1,768
Default Micro Milling 4104HT

I spent most of Thursday and Friday setting up roller tables so I could
run the large pieces of bar stock into my bandsaw, and roughing out
blanks. I liked the way it saw cut.

Today I am truing up blanks on the Hurco mill for further machining.
Cut starts sound a little hard on my face mill, but the surface finish
on the final pass is really nice.

Higher RPM with the same feed reduced the pounding, and of course
improved the finish even on the roughing passes. Flood coolant seems to
work about the same as cutting oil, so I went with flood coolant since I
don't have to stand there with a brush. The face mill does not have
only has TiN coated inserts. They definitely did not work well dry. It
cut, but the sound made the hair on the back of my neck stand on end.

I am not looking forward to the sound of the detailed machining of the
embossing portions on the smaller mills at "high" speed, but the stuff
machines really nicely at lower RPMs on the big mill. My finish pass
isn't mirror smooth, but its close enough I know I could make it that
way if I needed to.


  #18   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 2,163
Default Micro Milling 4104HT

On Mon, 18 Dec 2017 10:59:34 -0700, Bob La Londe
wrote:

I spent most of Thursday and Friday setting up roller tables so I could
run the large pieces of bar stock into my bandsaw, and roughing out
blanks. I liked the way it saw cut.

Today I am truing up blanks on the Hurco mill for further machining.
Cut starts sound a little hard on my face mill, but the surface finish
on the final pass is really nice.

Higher RPM with the same feed reduced the pounding, and of course
improved the finish even on the roughing passes. Flood coolant seems to
work about the same as cutting oil, so I went with flood coolant since I
don't have to stand there with a brush. The face mill does not have
only has TiN coated inserts. They definitely did not work well dry. It
cut, but the sound made the hair on the back of my neck stand on end.

I am not looking forward to the sound of the detailed machining of the
embossing portions on the smaller mills at "high" speed, but the stuff
machines really nicely at lower RPMs on the big mill. My finish pass
isn't mirror smooth, but its close enough I know I could make it that
way if I needed to.

I like machining both 4140HT and 4340HT. Nice chips and the hot chips
smell sweet. You will need to make sure the chip load is high enough
to get under the surface hardened slightly by the previous pass. I
used to turn lots of both metals and roughing passes using negative
rake inserts worked well to break the chip and to keep most of the
heat of the metal removal in the chip. When turning to final
dimensions where I had to hold a couple tenths and of course get the
finish required by the close tolerances I used very sharp positive
rake carbide tools. Usually inserts modified by hand grinding with
diamond wheels and brass laps charged with diamond. But sometimes
brazed carbide tools too, also hand ground. I used high sulfur cutting
oil for the final high tolerance, low material removal cuts. I know
milling is different because of the interrupted cuts and the way the
chip changes thickness during the cut. But really sharp cutters are
important as is getting the chips away from the cut so as to avoid
re-cutting of the chips.
Eric
  #19   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 10,399
Default Micro Milling 4104HT

On Mon, 18 Dec 2017 11:08:59 -0800, wrote:

On Mon, 18 Dec 2017 10:59:34 -0700, Bob La Londe
wrote:

I spent most of Thursday and Friday setting up roller tables so I could
run the large pieces of bar stock into my bandsaw, and roughing out
blanks. I liked the way it saw cut.

Today I am truing up blanks on the Hurco mill for further machining.
Cut starts sound a little hard on my face mill, but the surface finish
on the final pass is really nice.

Higher RPM with the same feed reduced the pounding, and of course
improved the finish even on the roughing passes. Flood coolant seems to
work about the same as cutting oil, so I went with flood coolant since I
don't have to stand there with a brush. The face mill does not have
only has TiN coated inserts. They definitely did not work well dry. It
cut, but the sound made the hair on the back of my neck stand on end.

I am not looking forward to the sound of the detailed machining of the
embossing portions on the smaller mills at "high" speed, but the stuff
machines really nicely at lower RPMs on the big mill. My finish pass
isn't mirror smooth, but its close enough I know I could make it that
way if I needed to.

I like machining both 4140HT and 4340HT. Nice chips and the hot chips
smell sweet. You will need to make sure the chip load is high enough
to get under the surface hardened slightly by the previous pass. I
used to turn lots of both metals and roughing passes using negative
rake inserts worked well to break the chip and to keep most of the
heat of the metal removal in the chip. When turning to final
dimensions where I had to hold a couple tenths and of course get the
finish required by the close tolerances I used very sharp positive
rake carbide tools. Usually inserts modified by hand grinding with
diamond wheels and brass laps charged with diamond. But sometimes
brazed carbide tools too, also hand ground. I used high sulfur cutting
oil for the final high tolerance, low material removal cuts. I know
milling is different because of the interrupted cuts and the way the
chip changes thickness during the cut. But really sharp cutters are
important as is getting the chips away from the cut so as to avoid
re-cutting of the chips.
Eric



And the chips are what carries the heat wasy from the cut as well.


---
This email has been checked for viruses by Avast antivirus software.
https://www.avast.com/antivirus

  #20   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 524
Default Micro Milling 4104HT

On Friday, December 8, 2017 at 10:47:12 PM UTC-5, BobH wrote:
On 12/08/2017 05:43 PM, Ed Huntress wrote:
On Fri, 8 Dec 2017 17:30:50 -0700, Bob La Londe
wrote:
If you haven't machined it, it's a piece of cake. Do you know what
grade it is? Brand?

Most are very abrasive but you can go as fast as your spindle will
allow. It machines more easily than magnesium. I machined a lot of
thread-cutting electrodes from Poco 3 graphite a few decades ago
Easy-peasy. Don't be afraid of it.


Wicked messy though. Graphite dust everywhere. I bought some equipment
from a shop that did a lot of graphite machining and it was a dusty mess.


How much can you get capturing and reselling the stuff?


  #22   Report Post  
Posted to rec.crafts.metalworking
external usenet poster
 
Posts: 1,768
Default Micro Milling 4104HT

On 12/8/2017 1:02 PM, Bob La Londe wrote:
I never thought I'd be doing this sort of work ever.Â* I am quite content
to high speed micro mill aluminum.Â* When I was first learning I asked a
lot of questions here and elsewhere.Â* Eventually I put together enough
information to where I can produce satisfactory results most of the time.

When I say micro milling I mean optimizing cut rates with modestly high
speed spindles (24K RPM) and pretty small cutters.Â* Almost no milling
job that I do gets by without a finish pass without atleast a .0625 ball
mill.Â* Quite often I have to use .03125 ball mills to finish some
details.Â* I even have to break out the .0156 stuff once in a while.
That's the range I am talking about when I say micro milling.

For all of that work I use uncoated square end and ball end mills with
6-8% SC520 and water with a constant flood.Â* Cutters last a very long
time and the results are good.Â* Jobs often last for hours.Â* Sometimes a
single tiny little cutter has to work for hours.

Well somebody offered me enough money to tempt me to do some similar
work in 4140HT.Â* I've milled some hardened steels and hard tool steels
before.Â* The numbers say 4140HT should be easier.Â* Its a sort of
compromise.Â* My past experience shows me that a low speed and feed with
an AlTin or TiAlN coated cutter works pretty good.Â* That's fine when you
are pushing a 1/2" 5 flute end mill, but I have to do some of that small
detail work to finish this job.Â* I need to push the envelope with ball
mills as small as .0156 for some of the finish work.Â* I can break it out
so I don't have to finish everything with it, but its still going to
more time than just a few hours.Â* HSM Adviser gives some numbers that
show days instead of weeks, but I wonder if there is anything I can do
to actually get those numbers.Â* With aluminum heat and thermal shock is
not really an issue.Â* With Altin in steal I don't run coolant, but I
admit I do throw a little cutting oil on the part.Â* I've just never done
small or micro milling in harder steel.Â* Well, I have engraved some
knife blades, but that's it.

I'm hoping I can cut down the learning curve, but I am prepared to break
some cutters and ruin some work pieces if I have to.Â* Chip clearance is
probably also going to be an issue.Â* Maybe an air blast to blow chips
clear and see what happens.Â* The thing is we are talking about steel.
Steel chips don't blow clear as easily as aluminum chips.

I am open to any suggestions.

Worst comes to worse I am prepared to tie up my machines for a few
weeks.Â* I certainly figure days even in the best case.


Ok, roughing now with a 1/2" 6 Flute and its going as good as I can
expect with my "not as rigid as it once was" KMB1. 0.8" DOC, 5% Step
over, conservative trochoidal approach. Its barking a little bit, but
the wall looks pretty good, and this is the roughing pass. I did the
math at 10% full depth stepover, and got to much deflection. Right now
its only at about 1HP load, but its removing a lot of material. I think
I could feed a lot faster, but at the risk of having to leave room for
two finish passes. The flood is really doing the trick. If it wasn't
for deflection I would rough faster. The chips are just brown. Not
even close to blue.

I am starting to like this material. Not sure what I was afraid of. I
may be done in a week. I was planning three. Well I may be done in a
week if the pieces I ordered for the largest die arrive soon.

Nah. I don't want to curse it. Three weeks it is. Maybe four. LOL.
I still don't know how the fine details of the embossing portion of the
dies will machine.


Reply
Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules

Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
PCB Micro drills and micro end mills" Ignoramus10035 Metalworking 11 September 27th 10 02:07 AM
Micro-Rel Badge - Micro-Rel-Badge.jpg Jim Thompson Electronic Schematics 17 December 22nd 08 07:25 AM
Milling on the lathe Vertical tslot table or vertical milling vise? Brent Philion Metalworking 25 April 1st 06 08:55 PM
Musing about up milling, down milling, shearing and scraping. Arch Woodturning 10 February 6th 05 09:11 PM
FA 'A treatsie on milling and milling machines' larry g Metalworking 0 November 9th 03 07:44 PM


All times are GMT +1. The time now is 05:25 PM.

Powered by vBulletin® Copyright ©2000 - 2024, Jelsoft Enterprises Ltd.
Copyright ©2004-2024 DIYbanter.
The comments are property of their posters.
 

About Us

"It's about DIY & home improvement"