Re: [Emc-users] milling tool life, or lack thereof.

2019-04-20 Thread John Dammeyer 
Hi Gene
I used the Machinist toolbox to figure out what sort of speed and feed I needed 
but ended up running the mill faster (thought I'd read it should be 3000 but it 
was supposed to be 2000).  Typo error.

OK. So tool bit 0.09375.  Two flutes.  HSS. Chip load 0.00551. Aluminium bar. 
SFM set at 40 which called for 2000 RPM and about 22 ipm  Max Radial 0.0375 (I 
think that means step over), and Max Axial 0.7969 (I think is depth per pass).

I ended up using all those parameters except ran the mill at 2950 RPM.   I ran 
0.025" depth of cut and 25% of tool diameter step over.So very conservative 
compared to the toolbox parameters.  And, squirts of WD-40 since I haven't set 
up the mister yet.  Parts are still on the way for that and I don’t want to run 
the flood coolant until I have it all boxed in and will use it often enough to 
prevent it going smelly.

No gumming up of the tool.  What I found with some other plate on the CNC 
router (disaster as far as gumming) is that one has to be really conservative 
to keep the heat down.  My CNC router couldn't move fast enough with the BOSCH 
Colt doing its minimum 16,000 RPM.  And I didn't want WD-40 all over the MDF.

Anyway, on the mill this is the end result.  AlibreCAM created a slot which 
meant it cut little arcs as it moved along the length of the slot.
The two switch mount holes were done with a #41 drill bit peck drilling.  No 
gumming. I like WD-40 although I suspect kerosene would work too.
http://www.autoartisans.com/mill/YAxisSwitchPlate.jpg

John

> -Original Message-
> From: Gene Heskett [mailto:ghesk...@shentel.net]
> Sent: April-20-19 5:58 PM
> To: emc-users@lists.sourceforge.net
> Subject: [Emc-users] milling tool life, or lack thereof.
> 
> Greetings all;
> 
> Having discovered the settings that control the low frequency boost in
> this VFD, and having rigged a pretty dry misting arrangement, I figured
> it was as good a time as any to cut the end panels of the box that has
> the interface cards in it.  These panels are about .035" thick, and are
> hard anodized which presents a challenge to most carbide tooling.  So I
> set it up to do the connectors holes in one panel, and the db cutouts
> for the computer cableds db 25's in the other panel. It did a beautiful
> job on the 11 holes in the first panel, but swapping panels to cut the
> db25 patterns was a disaster, the tool was obviously starting to plug
> up.  So I wound up with ragged holes with lots of metal thrown up that I
> had to sharpen up my pocket knife and clean up. Didn't break the tool
> but probably pushed my luck on that point.  Used about 4 oz of kool mist
> for the whole job, so it was wet, but not really soaking the cherry
> spoil board so bad I can't use it again after its dry.
> 
> This was an uncoated sc tool, 4mm in diameter, 3 flute with about a 45
> degree up spiral. Speeds ranged from 6000 revs to 14000. Chips thrown
> were almost dust and its obvious I need to put up some lexan splash
> guards.
> 
> The fact that it plugged up tells me that kool mist is not the magic
> bullet for this job. Safflower oil, which I used for one job years ago,
> would be better, but the cleanup needs solvent, lots of it. On
> everything it settles on. Including your lungs as I used more air
> pressure and smaller orifices. Blame it on younger and dumber as I was
> then in my mid-60's, 20 years ago?
> 
> Any suggestions as to what to concoct for misting fluid next time, that
> would prevent the sticking and plugging up while doing such sheet alu
> the next time? Or was the hard anodized brushed satin finish the real
> killer?  Add some liquid dish soap to enhance its "sticky" maybe?  IDK.
> 
> Thanks everybody.
> 
> Cheers, Gene Heskett
> --
> "There are four boxes to be used in defense of liberty:
>  soap, ballot, jury, and ammo. Please use in that order."
> -Ed Howdershelt (Author)
> Genes Web page 
> 
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread andy pugh 
On Sun, 21 Apr 2019 at 03:34, John Dammeyer  wrote:

> I used the Machinist toolbox to figure out what sort of speed and feed I 
> needed but ended up running the mill faster (thought I'd read it should be 
> 3000 but it was supposed to be 2000).  Typo error.
> OK. So tool bit 0.09375.  Two flutes.  HSS. Chip load 0.00551. Aluminium bar. 
> SFM set at 40 which called for 2000 RPM and about 22 ipm

That sounds slow at the spindle, I have been running at 8500 rpm and a
2.5mm cutter in tool steel.

FSWizard on my phone is suggesting 589 fpm (180 m/min) surface speed,
24,000 rpm and 15 in/min (388mm/min) for your <2.5mm cutter.
(So 10x the spindle speed but lower feedrate)

I suspect that Gene has the opposite problem, I am suspecting his feed
rate was too low if the swarf comes off as dust. (but he didn't
specify feed rate)

-- 
atp
"A motorcycle is a bicycle with a pandemonium attachment and is
designed for the especial use of mechanical geniuses, daredevils and
lunatics."
— George Fitch, Atlanta Constitution Newspaper, 1916


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Gene Heskett 
On Saturday 20 April 2019 22:32:21 John Dammeyer wrote:

> Hi Gene
> I used the Machinist toolbox to figure out what sort of speed and feed
> I needed but ended up running the mill faster (thought I'd read it
> should be 3000 but it was supposed to be 2000).  Typo error.
>
> OK. So tool bit 0.09375.  Two flutes.  HSS. Chip load 0.00551.
> Aluminium bar. SFM set at 40 which called for 2000 RPM and about 22
> ipm  Max Radial 0.0375 (I think that means step over), and Max Axial
> 0.7969 (I think is depth per pass).
>
> I ended up using all those parameters except ran the mill at 2950 RPM.
>   I ran 0.025" depth of cut and 25% of tool diameter step over.So
> very conservative compared to the toolbox parameters.  And, squirts of
> WD-40 since I haven't set up the mister yet.  Parts are still on the
> way for that and I don’t want to run the flood coolant until I have it
> all boxed in and will use it often enough to prevent it going smelly.
>
> No gumming up of the tool.  What I found with some other plate on the
> CNC router (disaster as far as gumming) is that one has to be really
> conservative to keep the heat down.  My CNC router couldn't move fast
> enough with the BOSCH Colt doing its minimum 16,000 RPM.  And I didn't
> want WD-40 all over the MDF.
>
> Anyway, on the mill this is the end result.  AlibreCAM created a slot
> which meant it cut little arcs as it moved along the length of the
> slot. The two switch mount holes were done with a #41 drill bit peck
> drilling.  No gumming. I like WD-40 although I suspect kerosene would
> work too. http://www.autoartisans.com/mill/YAxisSwitchPlate.jpg
>
> John
>
Thats purty, but then so was the first 11 holes it drilled, with a .0075" 
stepdown per full circle of g3. Here I found using the spiral down 
feature of g2/g3 seemed to accelerate the failure rate, so this time I 
did a straight stepdown at the starting angle of the hole. The bottom of 
the mill was starting to go by the time it had done about half the 
holes. And that stepdown was a g0 move so it would penetrate the anodic 
surface fast.

There was a 20 second cooldown pause between cutting operations, with the 
mister still energized, so I don't think the tool got hot. Maybe ran it 
too fast, probably should has slowed the spin as I believe it could have 
thrown bigger chips, not as far. But even drilling the holes, it was a 
full 4mm diameter of tool cut, eventually ejecting the center of the 
hole. Ditto the dsubs, straight plow until depth was reached and the 
center strip ejected. Obviously not ideal for max tool life. Stuff I'm 
still learning. :(

> > -Original Message-
> > From: Gene Heskett [mailto:ghesk...@shentel.net]
> > Sent: April-20-19 5:58 PM
> > To: emc-users@lists.sourceforge.net
> > Subject: [Emc-users] milling tool life, or lack thereof.
> >
> > Greetings all;
> >
> > Having discovered the settings that control the low frequency boost
> > in this VFD, and having rigged a pretty dry misting arrangement, I
> > figured it was as good a time as any to cut the end panels of the
> > box that has the interface cards in it.  These panels are about
> > .035" thick, and are hard anodized which presents a challenge to
> > most carbide tooling.  So I set it up to do the connectors holes in
> > one panel, and the db cutouts for the computer cableds db 25's in
> > the other panel. It did a beautiful job on the 11 holes in the first
> > panel, but swapping panels to cut the db25 patterns was a disaster,
> > the tool was obviously starting to plug up.  So I wound up with
> > ragged holes with lots of metal thrown up that I had to sharpen up
> > my pocket knife and clean up. Didn't break the tool but probably
> > pushed my luck on that point.  Used about 4 oz of kool mist for the
> > whole job, so it was wet, but not really soaking the cherry spoil
> > board so bad I can't use it again after its dry.
> >
> > This was an uncoated sc tool, 4mm in diameter, 3 flute with about a
> > 45 degree up spiral. Speeds ranged from 6000 revs to 14000. Chips
> > thrown were almost dust and its obvious I need to put up some lexan
> > splash guards.
> >
> > The fact that it plugged up tells me that kool mist is not the magic
> > bullet for this job. Safflower oil, which I used for one job years
> > ago, would be better, but the cleanup needs solvent, lots of it. On
> > everything it settles on. Including your lungs as I used more air
> > pressure and smaller orifices. Blame it on younger and dumber as I
> > was then in my mid-60's, 20 years ago?
> >
> > Any suggestions as to what to concoct for misting fluid next time,
> > that would prevent the sticking and plugging up while doing such
> > sheet alu the next time? Or was the hard anodized brushed satin
> > finish the real killer?  Add some liquid dish soap to enhance its
> > "sticky" maybe?  IDK.
> >
> > Thanks everybody.
> >
> > Cheers, Gene Heskett
> > --
> > "There are four boxes to be used in defense of liberty:
> >  soap, ballot, jury, and ammo. Pl

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Gene Heskett 
On Sunday 21 April 2019 03:40:08 andy pugh wrote:

> On Sun, 21 Apr 2019 at 03:34, John Dammeyer  
wrote:
> > I used the Machinist toolbox to figure out what sort of speed and
> > feed I needed but ended up running the mill faster (thought I'd read
> > it should be 3000 but it was supposed to be 2000).  Typo error. OK.
> > So tool bit 0.09375.  Two flutes.  HSS. Chip load 0.00551. Aluminium
> > bar. SFM set at 40 which called for 2000 RPM and about 22 ipm
>
> That sounds slow at the spindle, I have been running at 8500 rpm and a
> 2.5mm cutter in tool steel.
>
> FSWizard on my phone is suggesting 589 fpm (180 m/min) surface speed,
> 24,000 rpm and 15 in/min (388mm/min) for your <2.5mm cutter.
> (So 10x the spindle speed but lower feedrate)
>
> I suspect that Gene has the opposite problem, I am suspecting his feed
> rate was too low if the swarf comes off as dust. (but he didn't
> specify feed rate)

It was in retrospect too slow for the revs once I had some mist flowing, 
5 ipm to a max of 10 I think. Where can I get a copy of this machinist 
toolbox.  Sounds handy. The handbook covers this too, but in hard to 
find format since theres around 2k pages of it.

Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
Genes Web page 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread John Dammeyer 
Hi Andy,

> > I used the Machinist toolbox to figure out what sort of speed and feed I
> needed but ended up running the mill faster (thought I'd read it should be
> 3000 but it was supposed to be 2000).  Typo error.
> > OK. So tool bit 0.09375.  Two flutes.  HSS. Chip load 0.00551. Aluminium
> bar. SFM set at 40 which called for 2000 RPM and about 22 ipm
> 
> That sounds slow at the spindle, I have been running at 8500 rpm and a
> 2.5mm cutter in tool steel.
> 
> FSWizard on my phone is suggesting 589 fpm (180 m/min) surface speed,
> 24,000 rpm and 15 in/min (388mm/min) for your <2.5mm cutter.
> (So 10x the spindle speed but lower feedrate)
> 
> I suspect that Gene has the opposite problem, I am suspecting his feed
> rate was too low if the swarf comes off as dust. (but he didn't
> specify feed rate)


My mill has a top speed of 2950 so keeping the chip load per tooth  the same 
meant I had to keep tweaking the FPM until the recommended RPM dropped down to 
what my mill could do with a 2 flute HSS 3/32" cutter.  That also gave me the 
feed rate of about 22 ipm.

I guess it's like using a file on aluminium.  You can move the file quickly or 
slowly across the work.  Quickly removes more material but if it heats up it 
also gums up the file.  If it's done slowly with some WD-40 it doesn't gum up 
the file.  

BTW https://www.machinist-toolbox.com/ came included as part of my AlibreCAM 
license.  A google on FSWizad yields this: https://fswizard.com/


John



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Gene Heskett 
On Sunday 21 April 2019 12:11:11 John Dammeyer wrote:

> Hi Andy,
>
> > > I used the Machinist toolbox to figure out what sort of speed and
> > > feed I
> >
> > needed but ended up running the mill faster (thought I'd read it
> > should be 3000 but it was supposed to be 2000).  Typo error.
> >
> > > OK. So tool bit 0.09375.  Two flutes.  HSS. Chip load 0.00551.
> > > Aluminium
> >
> > bar. SFM set at 40 which called for 2000 RPM and about 22 ipm
> >
> > That sounds slow at the spindle, I have been running at 8500 rpm and
> > a 2.5mm cutter in tool steel.
> >
> > FSWizard on my phone is suggesting 589 fpm (180 m/min) surface
> > speed, 24,000 rpm and 15 in/min (388mm/min) for your <2.5mm cutter.
> > (So 10x the spindle speed but lower feedrate)
> >
> > I suspect that Gene has the opposite problem, I am suspecting his
> > feed rate was too low if the swarf comes off as dust. (but he didn't
> > specify feed rate)
>
> My mill has a top speed of 2950 so keeping the chip load per tooth 
> the same meant I had to keep tweaking the FPM until the recommended
> RPM dropped down to what my mill could do with a 2 flute HSS 3/32"
> cutter.  That also gave me the feed rate of about 22 ipm.
>
> I guess it's like using a file on aluminium.  You can move the file
> quickly or slowly across the work.  Quickly removes more material but
> if it heats up it also gums up the file.  If it's done slowly with
> some WD-40 it doesn't gum up the file.
>
> BTW https://www.machinist-toolbox.com/ came included as part of my
> AlibreCAM license.  A google on FSWizad yields this:
> https://fswizard.com/
>
>
> John
>
And I note, pricing to match, yet I doubt bobcad is paying the bills with 
that product.  I guess thats why I keep a whole zoo full of ti30x and 
ti36x calculators around. Then all I have to do is find the formula. 
lol. I've been tempted to get one of ti's modern programmables, but the 
calculators suplied with linux can do all that, except the programming 
bit.  Or maybe I haven't looked hard enough. TANSTAAFL.
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
Genes Web page 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread John Dammeyer 
HI Gene,

> > BTW https://www.machinist-toolbox.com/ came included as part of my
> > AlibreCAM license.  A google on FSWizad yields this:
> > https://fswizard.com/
> >
> >
> > John
> >
> And I note, pricing to match, yet I doubt bobcad is paying the bills with
> that product.  I guess thats why I keep a whole zoo full of ti30x and
> ti36x calculators around. Then all I have to do is find the formula.
> lol. I've been tempted to get one of ti's modern programmables, but the
> calculators supplied with linux can do all that, except the programming
> bit.  Or maybe I haven't looked hard enough. TANSTAAFL.
> >


Most of it I don't use.  But I tried the FSWizard and it doesn't appear to 
allow tweaking with different SFM to determine ipm of the axis.  There must be 
a free something out there.

John




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Roland Jollivet 
And I note, pricing to match, yet I doubt bobcad is paying the bills with

> that product.  I guess thats why I keep a whole zoo full of ti30x and
> ti36x calculators around. Then all I have to do is find the formula.
> lol. I've been tempted to get one of ti's modern programmables, but the
> calculators suplied with linux can do all that, except the programming
> bit.  Or maybe I haven't looked hard enough. TANSTAAFL.
> >
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
>
>
Hi Gene

Did you ever try out Bob Warfield's software?
https://www.cnccookbook.com/




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Jon Elson 




On Sun, 21 Apr 2019 at 03:34, John Dammeyer  wrote:


I used the Machinist toolbox to figure out what sort of speed and feed I needed 
but ended up running the mill faster (thought I'd read it should be 3000 but it 
was supposed to be 2000).  Typo error.
OK. So tool bit 0.09375.  Two flutes.  HSS. Chip load 0.00551. Aluminium bar. 
SFM set at 40 which called for 2000 RPM and about 22 ipm


.094 tool at 2000 RPM is 50 SFPM, really slow for aluminum.  
600 SFPM is recommended.
chip load for HSS end mills should be .010 * end mill 
diameter, so .010 * .094 = about .001".

At these settings, feed rate should be 4 IPM.

I have stopped using all HSS in the smaller sizes, I buy 
10-packs of 1/8" solid carbide end mills for about $3 each, 
and they last a LONG time.  Crummy "HSS" tools from China 
last about 5 minutes before dulling begins to show.  
Name-brand M42 HSS tools seem to last at least 3 times 
longer, maybe even up to 10 X better.  And, they rarely cost 
more than $1 extra over plain HSS.


One of the tricks with aluminum is to keep the cutter 
moving.  So, take a shallow cut and keep the feedrate up, 
and always do climb milling if possible.  Higher feeds keep 
the heat from being concentrated in one spot on the workpiece.


Using a 1/8" carbide end mill at about 3000 RPM (limit of my 
mill), I would plow full-width cuts at a depth of .062" 
(half diameter) at about 4 IPM, then cut the sides at 10-15 
IPM with a side step over of about 0.25 - .050, and a final 
dimension pass taking off .010 on the side at 8 - 12 IPM.
This is with a 4-flute cutter.  As long as you keep the 
cutter moving right along, you won't have a problem with 
gumming up the cutter.


And, flood coolant REALLY helps with the heating problem.  I 
have a throttle valve on my coolant system, and use the 
smallest LocLine nozzle, and throttle it down to a little 
jet pointed right at the cutter.  So, it just spreads out a 
little puddle on the top of the part.


Jon


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Ken Strauss 
If you are getting chips that are "almost dust" you have a serious problem
with your speeds/feeds. Increase your feed rate and/or reduce the tool rpm.
You should always be getting real chips. I find that ZrN (Zirconium Nitride)
coating on the cutters helps significantly to reduce chip welding in soft
aluminum.

> -Original Message-
> From: Gene Heskett [mailto:ghesk...@shentel.net]
> Sent: Saturday, April 20, 2019 8:58 PM
> To: emc-users@lists.sourceforge.net
> Subject: [Emc-users] milling tool life, or lack thereof.
>
> Greetings all;
>
> Having discovered the settings that control the low frequency boost in
> this VFD, and having rigged a pretty dry misting arrangement, I figured
> it was as good a time as any to cut the end panels of the box that has
> the interface cards in it.  These panels are about .035" thick, and are
> hard anodized which presents a challenge to most carbide tooling.  So I
> set it up to do the connectors holes in one panel, and the db cutouts
> for the computer cableds db 25's in the other panel. It did a beautiful
> job on the 11 holes in the first panel, but swapping panels to cut the
> db25 patterns was a disaster, the tool was obviously starting to plug
> up.  So I wound up with ragged holes with lots of metal thrown up that I
> had to sharpen up my pocket knife and clean up. Didn't break the tool
> but probably pushed my luck on that point.  Used about 4 oz of kool mist
> for the whole job, so it was wet, but not really soaking the cherry
> spoil board so bad I can't use it again after its dry.
>
> This was an uncoated sc tool, 4mm in diameter, 3 flute with about a 45
> degree up spiral. Speeds ranged from 6000 revs to 14000. Chips thrown
> were almost dust and its obvious I need to put up some lexan splash
> guards.
>
> The fact that it plugged up tells me that kool mist is not the magic
> bullet for this job. Safflower oil, which I used for one job years ago,
> would be better, but the cleanup needs solvent, lots of it. On
> everything it settles on. Including your lungs as I used more air
> pressure and smaller orifices. Blame it on younger and dumber as I was
> then in my mid-60's, 20 years ago?
>
> Any suggestions as to what to concoct for misting fluid next time, that
> would prevent the sticking and plugging up while doing such sheet alu
> the next time? Or was the hard anodized brushed satin finish the real
> killer?  Add some liquid dish soap to enhance its "sticky" maybe?  IDK.
>
> Thanks everybody.
>
> Cheers, Gene Heskett
> --
> "There are four boxes to be used in defense of liberty:
>  soap, ballot, jury, and ammo. Please use in that order."
> -Ed Howdershelt (Author)
> Genes Web page 
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Ken Strauss 
Consider: https://hsmadvisor.com/


> -Original Message-
> From: Gene Heskett [mailto:ghesk...@shentel.net]
> Sent: Sunday, April 21, 2019 4:09 AM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] milling tool life, or lack thereof.
>
> On Sunday 21 April 2019 03:40:08 andy pugh wrote:
>
> > On Sun, 21 Apr 2019 at 03:34, John Dammeyer 
> wrote:
> > > I used the Machinist toolbox to figure out what sort of speed and
> > > feed I needed but ended up running the mill faster (thought I'd read
> > > it should be 3000 but it was supposed to be 2000).  Typo error. OK.
> > > So tool bit 0.09375.  Two flutes.  HSS. Chip load 0.00551. Aluminium
> > > bar. SFM set at 40 which called for 2000 RPM and about 22 ipm
> >
> > That sounds slow at the spindle, I have been running at 8500 rpm and a
> > 2.5mm cutter in tool steel.
> >
> > FSWizard on my phone is suggesting 589 fpm (180 m/min) surface speed,
> > 24,000 rpm and 15 in/min (388mm/min) for your <2.5mm cutter.
> > (So 10x the spindle speed but lower feedrate)
> >
> > I suspect that Gene has the opposite problem, I am suspecting his feed
> > rate was too low if the swarf comes off as dust. (but he didn't
> > specify feed rate)
>
> It was in retrospect too slow for the revs once I had some mist flowing,
> 5 ipm to a max of 10 I think. Where can I get a copy of this machinist
> toolbox.  Sounds handy. The handbook covers this too, but in hard to
> find format since theres around 2k pages of it.
>
> Cheers, Gene Heskett
> --
> "There are four boxes to be used in defense of liberty:
>  soap, ballot, jury, and ammo. Please use in that order."
> -Ed Howdershelt (Author)
> Genes Web page <http://geneslinuxbox.net:6309/gene>
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread John Dammeyer 
Hi Jon,


> .094 tool at 2000 RPM is 50 SFPM, really slow for aluminum.
> 600 SFPM is recommended.
> chip load for HSS end mills should be .010 * end mill
> diameter, so .010 * .094 = about .001".
> At these settings, feed rate should be 4 IPM.

The Machinist toolbox with 600SFPM, carbide, 4 flute, 0.094 diameter, chip load 
0.001 comes out to 24,000 RPM and 97 ipm. 



> Using a 1/8" carbide end mill at about 3000 RPM (limit of my
> mill), I would plow full-width cuts at a depth of .062"
> (half diameter) at about 4 IPM, then cut the sides at 10-15
> IPM with a side step over of about 0.25 - .050, and a final
> dimension pass taking off .010 on the side at 8 - 12 IPM.
> This is with a 4-flute cutter.  As long as you keep the
> cutter moving right along, you won't have a problem with
> gumming up the cutter.

> 
> Jon


The trick is to not get it hot enough to melt I guess.  Watched a video the 
other day where, to make the video better he cut back the flood coolant a bit 
to better see what it was cutting and had an instant clog up of the mill.



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Gene Heskett 
On Sunday 21 April 2019 13:01:18 John Dammeyer wrote:

> HI Gene,
>
> > > BTW https://www.machinist-toolbox.com/ came included as part of my
> > > AlibreCAM license.  A google on FSWizad yields this:
> > > https://fswizard.com/
> > >
> > >
> > > John
> >
> > And I note, pricing to match, yet I doubt bobcad is paying the bills
> > with that product.  I guess thats why I keep a whole zoo full of
> > ti30x and ti36x calculators around. Then all I have to do is find
> > the formula. lol. I've been tempted to get one of ti's modern
> > programmables, but the calculators supplied with linux can do all
> > that, except the programming bit.  Or maybe I haven't looked hard
> > enough. TANSTAAFL.
>
> Most of it I don't use.  But I tried the FSWizard and it doesn't
> appear to allow tweaking with different SFM to determine ipm of the
> axis.  There must be a free something out there.
>
> John
>
Yeah, I've a nearly 40 yo ti-52, I even rebuilt it to use nmh batteries 
after the early nicads died in a year or so, but the charger connection 
is so iffy I gave up on the thing 30 years ago.  I see hp has one for 
around a 50 dollar bill that does both rpn and std algebraic, but the 
adv's never tell you how much nv program ram they have. TI's graphing 
models seem interesting, but its the same problem, nobody wants to put 
enough program memory in them so this stuff can be "canned" for future 
conversational use.  So I've not had the urge to stick the end of the 
card in the slot. And frankly, if I used such in the shop, and it got 
drowned in coolant, at its price I'd be upset.

I wonder if Big John T has some of his pythonic skills up his sleeve?

I sorta got some pix of the mess that 6040 is in Friday, now I need to 
bring the camera back in and pull them out & run them thru Wilbers 
toolbox for about a 90% shrink.  This camera, a Nikon L100, needs a new 
data socket, I can only get pix out of it by placeing it face down on 
the lens, so the weight of the cable makes a usable connection.  So if 
you hear some background muttering, you'll know why.

Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
Genes Web page 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Gene Heskett 
On Sunday 21 April 2019 13:11:01 Roland Jollivet wrote:

[...]
> Hi Gene
>
> Did you ever try out Bob Warfield's software?
> https://www.cnccookbook.com/

No, but I've heard good things about it, so when the next hour+ job turns 
up, its bookmarked.

Thanks for the link. It did not turn up in a google search earlier today, 
and it should have.
>
One year for 80 bucks would be enough to decide on a lifetime license. 
But at 84 now, one has to wonder if his name is on the call-up list for 
next week.

I take it its in python or other portable language, it gives no 
requirements to run it.

> 
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
Genes Web page 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Ken Strauss 
The one-year price buys a perpetual licence for small machines (less than
1.5HP as I recall).

> -Original Message-
> From: Gene Heskett [mailto:ghesk...@shentel.net]
> Sent: Sunday, April 21, 2019 5:01 PM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] milling tool life, or lack thereof.
>
> On Sunday 21 April 2019 13:11:01 Roland Jollivet wrote:
>
> [...]
> > Hi Gene
> >
> > Did you ever try out Bob Warfield's software?
> > https://www.cnccookbook.com/
>
> No, but I've heard good things about it, so when the next hour+ job turns
> up, its bookmarked.
>
> Thanks for the link. It did not turn up in a google search earlier today,
> and it should have.
> >
> One year for 80 bucks would be enough to decide on a lifetime license.
> But at 84 now, one has to wonder if his name is on the call-up list for
> next week.
>
> I take it its in python or other portable language, it gives no
> requirements to run it.
>
> > <https://lists.sourceforge.net/lists/listinfo/emc-users>
> >
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
>
>
> Cheers, Gene Heskett
> --
> "There are four boxes to be used in defense of liberty:
>  soap, ballot, jury, and ammo. Please use in that order."
> -Ed Howdershelt (Author)
> Genes Web page <http://geneslinuxbox.net:6309/gene>
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Gene Heskett 
On Sunday 21 April 2019 14:07:55 Jon Elson wrote:

> > On Sun, 21 Apr 2019 at 03:34, John Dammeyer  
wrote:
> >> I used the Machinist toolbox to figure out what sort of speed and
> >> feed I needed but ended up running the mill faster (thought I'd
> >> read it should be 3000 but it was supposed to be 2000).  Typo
> >> error. OK. So tool bit 0.09375.  Two flutes.  HSS. Chip load
> >> 0.00551. Aluminium bar. SFM set at 40 which called for 2000 RPM and
> >> about 22 ipm
>
> .094 tool at 2000 RPM is 50 SFPM, really slow for aluminum.
> 600 SFPM is recommended.
> chip load for HSS end mills should be .010 * end mill
> diameter, so .010 * .094 = about .001".
> At these settings, feed rate should be 4 IPM.
>
> I have stopped using all HSS in the smaller sizes, I buy
> 10-packs of 1/8" solid carbide end mills for about $3 each,
> and they last a LONG time.  Crummy "HSS" tools from China
> last about 5 minutes before dulling begins to show.
> Name-brand M42 HSS tools seem to last at least 3 times
> longer, maybe even up to 10 X better.  And, they rarely cost
> more than $1 extra over plain HSS.
>
> One of the tricks with aluminum is to keep the cutter
> moving.  So, take a shallow cut and keep the feedrate up,
> and always do climb milling if possible.  Higher feeds keep
> the heat from being concentrated in one spot on the workpiece.
>
> Using a 1/8" carbide end mill at about 3000 RPM (limit of my
> mill), I would plow full-width cuts at a depth of .062"
> (half diameter) at about 4 IPM, then cut the sides at 10-15
> IPM with a side step over of about 0.25 - .050, and a final
> dimension pass taking off .010 on the side at 8 - 12 IPM.
> This is with a 4-flute cutter.  As long as you keep the
> cutter moving right along, you won't have a problem with
> gumming up the cutter.
>
Printed for shop use, thanks Jon.
 
> And, flood coolant REALLY helps with the heating problem.  I
> have a throttle valve on my coolant system, and use the
> smallest LocLine nozzle, and throttle it down to a little
> jet pointed right at the cutter.  So, it just spreads out a
> little puddle on the top of the part.
>
> Jon
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
Genes Web page 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Gregg Eshelman via Emc-users 
Is that still requiring an internet connection in order to use it? There are 
plenty of would-be customers who've said "No way!" to that software because 
they don't have and don't want any internet connected computers in their shops.
 
On Sunday, April 21, 2019, 3:02:33 PM MDT, Gene Heskett 
 wrote:  
 On Sunday 21 April 2019 13:11:01 Roland Jollivet wrote:

[...]
> Hi Gene
>
> Did you ever try out Bob Warfield's software?
> https://www.cnccookbook.com/

No, but I've heard good things about it, so when the next hour+ job turns 
up, its bookmarked.

Thanks for the link. It did not turn up in a google search earlier today, 
and it should have.
>
One year for 80 bucks would be enough to decide on a lifetime license. 
But at 84 now, one has to wonder if his name is on the call-up list for 
next week.

I take it its in python or other portable language, it gives no 
requirements to run it.  
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread John Dammeyer 
I just tried it and it appears to want to be registered.  It says Hi johnd in 
the upper right corner but then when I try one of the menu selections it jumps 
back to the hello and set up your machine screen.  Plus already a couple of 
emails about it.

Enough annoying characteristics that I'm happy I have the Alibre sponsored 
Machinist Toolbox.  My 30 day trial will now last less than 24 hours before 
it's removed.

John


> -Original Message-
> From: Gregg Eshelman via Emc-users [mailto:emc-
> us...@lists.sourceforge.net]
> Sent: April-21-19 3:35 PM
> To: Enhanced Machine Controller (EMC)
> Cc: Gregg Eshelman
> Subject: Re: [Emc-users] milling tool life, or lack thereof.
> 
> Is that still requiring an internet connection in order to use it? There are
> plenty of would-be customers who've said "No way!" to that software
> because they don't have and don't want any internet connected computers
> in their shops.
> 
> On Sunday, April 21, 2019, 3:02:33 PM MDT, Gene Heskett
>  wrote:
>  On Sunday 21 April 2019 13:11:01 Roland Jollivet wrote:
> 
> [...]
> > Hi Gene
> >
> > Did you ever try out Bob Warfield's software?
> > https://www.cnccookbook.com/
> 
> No, but I've heard good things about it, so when the next hour+ job turns
> up, its bookmarked.
> 
> Thanks for the link. It did not turn up in a google search earlier today,
> and it should have.
> >
> One year for 80 bucks would be enough to decide on a lifetime license.
> But at 84 now, one has to wonder if his name is on the call-up list for
> next week.
> 
> I take it its in python or other portable language, it gives no
> requirements to run it.
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread John Dammeyer 
I think I just figured out why it knows me and appears to have loaded properly. 
 I must have done a trial a long time ago.  When I try and log in it tells me 
my trial is expired.  I can ask for a new trial I guess.  Or not.
John


> -Original Message-
> From: John Dammeyer [mailto:jo...@autoartisans.com]
> Sent: April-21-19 3:55 PM
> To: 'Enhanced Machine Controller (EMC)'
> Subject: Re: [Emc-users] milling tool life, or lack thereof.
> 
> I just tried it and it appears to want to be registered.  It says Hi johnd in 
> the
> upper right corner but then when I try one of the menu selections it jumps
> back to the hello and set up your machine screen.  Plus already a couple of
> emails about it.
> 
> Enough annoying characteristics that I'm happy I have the Alibre sponsored
> Machinist Toolbox.  My 30 day trial will now last less than 24 hours before 
> it's
> removed.
> 
> John
> 
> 
> > -Original Message-
> > From: Gregg Eshelman via Emc-users [mailto:emc-
> > us...@lists.sourceforge.net]
> > Sent: April-21-19 3:35 PM
> > To: Enhanced Machine Controller (EMC)
> > Cc: Gregg Eshelman
> > Subject: Re: [Emc-users] milling tool life, or lack thereof.
> >
> > Is that still requiring an internet connection in order to use it? There are
> > plenty of would-be customers who've said "No way!" to that software
> > because they don't have and don't want any internet connected
> computers
> > in their shops.
> >
> > On Sunday, April 21, 2019, 3:02:33 PM MDT, Gene Heskett
> >  wrote:
> >  On Sunday 21 April 2019 13:11:01 Roland Jollivet wrote:
> >
> > [...]
> > > Hi Gene
> > >
> > > Did you ever try out Bob Warfield's software?
> > > https://www.cnccookbook.com/
> >
> > No, but I've heard good things about it, so when the next hour+ job turns
> > up, its bookmarked.
> >
> > Thanks for the link. It did not turn up in a google search earlier today,
> > and it should have.
> > >
> > One year for 80 bucks would be enough to decide on a lifetime license.
> > But at 84 now, one has to wonder if his name is on the call-up list for
> > next week.
> >
> > I take it its in python or other portable language, it gives no
> > requirements to run it.
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
> 
> 
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Jon Elson 

On 04/21/2019 02:20 PM, John Dammeyer wrote:



The trick is to not get it hot enough to melt I guess.  Watched a video the 
other day where, to make the video better he cut back the flood coolant a bit 
to better see what it was cutting and had an instant clog up of the mill.


Yes, absolutely!  The softer the alloy, the less heat it 
takes to get it to the "gummy" state.
Coolant works wonders, the whole trick is to make sure the 
workpiece is stiff enough for the cutting edge to CUT, 
rather than MASH, through the material.  Heating some grades 
of aluminum just to about body temperature (100F - 37 C) 
will get it into that range when the cutter hits it.


Jon


___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Gene Heskett 
On Sunday 21 April 2019 14:12:36 Ken Strauss wrote:

> If you are getting chips that are "almost dust" you have a serious
> problem with your speeds/feeds. Increase your feed rate and/or reduce
> the tool rpm. You should always be getting real chips. I find that ZrN
> (Zirconium Nitride) coating on the cutters helps significantly to
> reduce chip welding in soft aluminum.

So noted Ken.  Now the trick is to get my ancient wet ram to remember 
that detail. I find over the last 2 decades, that I spend a lot of my 
time contemplating the here after. I go to get a tool, and when I get to 
where my memory says I last saw or used that tool, I have to stand there 
asking myself what am I here after. And worse yet I do not always 
succeed in recalling it.

I don't recommend getting old, too much of that stuff goes with it...

> > -Original Message-
> > From: Gene Heskett [mailto:ghesk...@shentel.net]
> > Sent: Saturday, April 20, 2019 8:58 PM
> > To: emc-users@lists.sourceforge.net
> > Subject: [Emc-users] milling tool life, or lack thereof.
> >
> > Greetings all;
> >
> > Having discovered the settings that control the low frequency boost
> > in this VFD, and having rigged a pretty dry misting arrangement, I
> > figured it was as good a time as any to cut the end panels of the
> > box that has the interface cards in it.  These panels are about
> > .035" thick, and are hard anodized which presents a challenge to
> > most carbide tooling.  So I set it up to do the connectors holes in
> > one panel, and the db cutouts for the computer cableds db 25's in
> > the other panel. It did a beautiful job on the 11 holes in the first
> > panel, but swapping panels to cut the db25 patterns was a disaster,
> > the tool was obviously starting to plug up.  So I wound up with
> > ragged holes with lots of metal thrown up that I had to sharpen up
> > my pocket knife and clean up. Didn't break the tool but probably
> > pushed my luck on that point.  Used about 4 oz of kool mist for the
> > whole job, so it was wet, but not really soaking the cherry spoil
> > board so bad I can't use it again after its dry.
> >
> > This was an uncoated sc tool, 4mm in diameter, 3 flute with about a
> > 45 degree up spiral. Speeds ranged from 6000 revs to 14000. Chips
> > thrown were almost dust and its obvious I need to put up some lexan
> > splash guards.
> >
> > The fact that it plugged up tells me that kool mist is not the magic
> > bullet for this job. Safflower oil, which I used for one job years
> > ago, would be better, but the cleanup needs solvent, lots of it. On
> > everything it settles on. Including your lungs as I used more air
> > pressure and smaller orifices. Blame it on younger and dumber as I
> > was then in my mid-60's, 20 years ago?
> >
> > Any suggestions as to what to concoct for misting fluid next time,
> > that would prevent the sticking and plugging up while doing such
> > sheet alu the next time? Or was the hard anodized brushed satin
> > finish the real killer?  Add some liquid dish soap to enhance its
> > "sticky" maybe?  IDK.
> >
> > Thanks everybody.
> >
> > Cheers, Gene Heskett
> > --
> > "There are four boxes to be used in defense of liberty:
> >  soap, ballot, jury, and ammo. Please use in that order."
> > -Ed Howdershelt (Author)
> > Genes Web page 
> >
> >
> >
> > ___
> > Emc-users mailing list
> > Emc-users@lists.sourceforge.net
> > https://lists.sourceforge.net/lists/listinfo/emc-users
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users


Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
Genes Web page 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Gene Heskett 
On Sunday 21 April 2019 14:21:24 Ken Strauss wrote:

> Consider: https://hsmadvisor.com/

Apple or android only.  Sob.

[...]

Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
Genes Web page 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Ken Strauss 
Or windows.

> -Original Message-
> From: Gene Heskett [mailto:ghesk...@shentel.net]
> Sent: Sunday, April 21, 2019 7:42 PM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] milling tool life, or lack thereof.
>
> On Sunday 21 April 2019 14:21:24 Ken Strauss wrote:
>
> > Consider: https://hsmadvisor.com/
>
> Apple or android only.  Sob.
>
> [...]
>
> Cheers, Gene Heskett
> --
> "There are four boxes to be used in defense of liberty:
>  soap, ballot, jury, and ammo. Please use in that order."
> -Ed Howdershelt (Author)
> Genes Web page <http://geneslinuxbox.net:6309/gene>
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Gene Heskett 
On Sunday 21 April 2019 17:33:36 Ken Strauss wrote:

> The one-year price buys a perpetual licence for small machines (less
> than 1.5HP as I recall).
>
I didn't see that, didn't click on the buy now button either. But 
figuratively speaking all my machines could probably qualify.  Clicked 
on the annual button, but it still doesn't show that.  So I've sent Mr 
Woodward an email.

Thank Ken.

Cheers, Gene Heskett
-- 
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author)
Genes Web page 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] milling tool life, or lack thereof.

2019-04-21 Thread Ken Strauss 
Perhaps things have changed after I purchased my copy several years ago but
I still get frequent updates.

> -Original Message-
> From: Gene Heskett [mailto:ghesk...@shentel.net]
> Sent: Sunday, April 21, 2019 8:35 PM
> To: emc-users@lists.sourceforge.net
> Subject: Re: [Emc-users] milling tool life, or lack thereof.
>
> On Sunday 21 April 2019 17:33:36 Ken Strauss wrote:
>
> > The one-year price buys a perpetual licence for small machines (less
> > than 1.5HP as I recall).
> >
> I didn't see that, didn't click on the buy now button either. But
> figuratively speaking all my machines could probably qualify.  Clicked
> on the annual button, but it still doesn't show that.  So I've sent Mr
> Woodward an email.
>
> Thank Ken.
>
> Cheers, Gene Heskett
> --
> "There are four boxes to be used in defense of liberty:
>  soap, ballot, jury, and ammo. Please use in that order."
> -Ed Howdershelt (Author)
> Genes Web page <http://geneslinuxbox.net:6309/gene>
>
>
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users