On 04/13/2017 02:24 PM, Erik Friesen wrote:
> Free use terms = <$100,000 per year.
>
> Non Free = you should be able to afford it.
>
> On Thu, Apr 13, 2017 at 5:16 PM, Gregg Eshelman wrote:
>
>> Do test runs in wood or machinable wax or plastic. Could try spraying a
>> dry graphite film on the c
On Fri, Apr 14, 2017, at 11:37 AM, John Kasunich wrote:
>
>
> On Thu, Apr 13, 2017, at 08:59 PM, Jon Elson wrote:
> > On 04/13/2017 12:44 PM, Todd Zuercher wrote:
> > >
> > > But I'm cutting out a 2ft x 3ft window. It would be silly to pocket fill
> > > that entire thing.
> > Yes, that is som
On Thu, Apr 13, 2017, at 08:59 PM, Jon Elson wrote:
> On 04/13/2017 12:44 PM, Todd Zuercher wrote:
> >
> > But I'm cutting out a 2ft x 3ft window. It would be silly to pocket fill
> > that entire thing.
> Yes, that is something I do all the time. I call it
> trepanning, and I have programs to
On 04/13/2017 12:44 PM, Todd Zuercher wrote:
>
> But I'm cutting out a 2ft x 3ft window. It would be silly to pocket fill
> that entire thing.
Yes, that is something I do all the time. I call it
trepanning, and I have programs to do that, also. However,
there's no way to avoid the first cut a
Free use terms = <$100,000 per year.
Non Free = you should be able to afford it.
On Thu, Apr 13, 2017 at 5:16 PM, Gregg Eshelman wrote:
> Do test runs in wood or machinable wax or plastic. Could try spraying a
> dry graphite film on the cutter. NAPA auto parts has spray cans of that.
> Don't mi
Do test runs in wood or machinable wax or plastic. Could try spraying a dry
graphite film on the cutter. NAPA auto parts has spray cans of that. Don't mill
the crappy aluminum alloy.
On Thursday, April 13, 2017, 8:46:03 AM MDT, Todd Zuercher
wrote:Here I go again. Unfortunately, the aluminum
, 2017 3:28:24 PM
Subject: Re: [Emc-users] Milling Aluminum.
On 13 April 2017 at 20:01, Todd Zuercher wrote:
>> Maybe an excuse to buy a plasma cutter?
> But it seems to be working decently now using a Vortex 5630 tool and a
> trochoidlal cut path.
You aren't very good at this
On 13 April 2017 at 20:01, Todd Zuercher wrote:
>> Maybe an excuse to buy a plasma cutter?
> But it seems to be working decently now using a Vortex 5630 tool and a
> trochoidlal cut path.
You aren't very good at this are you :-)
--
atp
"A motorcycle is a bicycle with a pandemonium attachmen
- Original Message -
> From: "andy pugh"
> To: "Enhanced Machine Controller (EMC)"
> Sent: Thursday, April 13, 2017 2:16:06 PM
> Subject: Re: [Emc-users] Milling Aluminum.
>
> On 13 April 2017 at 18:44, Todd Zuercher
> w
On 13 April 2017 at 18:44, Todd Zuercher
wrote:
> But I'm cutting out a 2ft x 3ft window.
Maybe an excuse to buy a plasma cutter? (Google just told me that
plasma is good for aluminium)
--
atp
"A motorcycle is a bicycle with a pandemonium attachment and is
designed for the
- Original Message -
> From: "Jon Elson"
> To: "Enhanced Machine Controller (EMC)"
> Sent: Thursday, April 13, 2017 1:22:32 PM
> Subject: Re: [Emc-users] Milling Aluminum.
>
> On 04/13/2017 09:41 AM, Todd Zuercher wrote:
> > Here I go again
On 04/13/2017 10:19 AM, Kirk Wallace wrote:
> On 04/13/2017 08:04 AM, andy pugh wrote:
>> On 13 April 2017 at 15:41, Todd Zuercher
>> wrote:
>>> Suggestions on where I should go from here?
>> Download Fusion360 and get a real trochoidal milling path.
>>
> It should not be terr
On 04/13/2017 09:41 AM, Todd Zuercher wrote:
> Here I go again. Unfortunately, the aluminum jig was a big hit, and now they
> want more. So I thought I'd take a crack at a trochoirdal milling path. My
> first try gave mixed results. Looking for advice.
> My CAM software still doesn't have a t
0.002" already.
>
> Next, I'll try pulling back the RPM to get a higher chipload. Aiming for
> about 0.005" this time so I'll run 8000rpm.
> Then I'm going to try a single flute O-flute cutter (with a alight up cut).
>
> - Original Message -
> Fro
k the RPM to get a higher chipload. Aiming for
> about 0.005" this time so I'll run 8000rpm.
> Then I'm going to try a single flute O-flute cutter (with a alight up cut).
>
> - Original Message -
> From: "Jim Craig"
> To: "Enhanced Machine Co
: Thursday, April 13, 2017 11:45:00 AM
Subject: Re: [Emc-users] Milling Aluminum.
On 13 April 2017 at 16:19, Todd Zuercher
wrote:
> Is what I did really all that different from a "real" trochoidal path?
> https://pastebin.com/nbQ1AKia.
Well, the "real&quo
- Original Message -
From: "Jim Craig"
To: "Enhanced Machine Controller (EMC)"
Sent: Thursday, April 13, 2017 11:27:42 AM
Subject: Re: [Emc-users] Milling Aluminum.
Lube is your friend. I try not to do any aluminum cutting without
lubrication. I think your air blast an
On 13 April 2017 at 16:19, Todd Zuercher
wrote:
> Is what I did really all that different from a "real" trochoidal path?
> https://pastebin.com/nbQ1AKia.
Well, the "real" paths move at a higher speed during the non-engagement moves.
--
atp
"A motorcycle is a bicycle with a
rom the Mic-6 scrap left over from the
> last one.
>
>
> - Original Message -
> From: "Jon Elson"
> To: "Enhanced Machine Controller (EMC)"
> Sent: Thursday, February 23, 2017 12:54:14 PM
> Subject: Re: [Emc-users] Milling Aluminum.
>
> O
Ideally,
you should not be able to see the oil blowing away, but your finger
should come away with oil on it if held downwind of the tool for a
couple seconds.
> - Original Message -
> From: "Jon Elson"
> To: "Enhanced Machine Controller (EMC)"
> Sent
om: "andy pugh"
To: "Enhanced Machine Controller (EMC)"
Sent: Thursday, April 13, 2017 11:04:11 AM
Subject: Re: [Emc-users] Milling Aluminum.
On 13 April 2017 at 15:41, Todd Zuercher
wrote:
> Suggestions on where I should go from here?
Download Fusion36
On 04/13/2017 08:04 AM, andy pugh wrote:
> On 13 April 2017 at 15:41, Todd Zuercher
> wrote:
>> Suggestions on where I should go from here?
>
> Download Fusion360 and get a real trochoidal milling path.
>
It should not be terribly hard to write a g-code loop to do a slot.
Th
On 13 April 2017 at 15:41, Todd Zuercher
wrote:
> Suggestions on where I should go from here?
Download Fusion360 and get a real trochoidal milling path.
--
atp
"A motorcycle is a bicycle with a pandemonium attachment and is
designed for the especial use of mechanical genius
Mic-6 scrap left over from the last one.
- Original Message -
From: "Jon Elson"
To: "Enhanced Machine Controller (EMC)"
Sent: Thursday, February 23, 2017 12:54:14 PM
Subject: Re: [Emc-users] Milling Aluminum.
On 02/23/2017 09:35 AM, Jim Craig wrote:
> Yep, you sho
Elson"
To: "Enhanced Machine Controller (EMC)"
Sent: Thursday, February 23, 2017 12:58:57 PM
Subject: Re: [Emc-users] Milling Aluminum.
On 02/23/2017 10:03 AM, Todd Zuercher wrote:
> There is also the fact that our CAM doesn't do HSM tool pathing as it is
>
On 02/23/2017 10:03 AM, Todd Zuercher wrote:
> There is also the fact that our CAM doesn't do HSM tool pathing as it is
> geared more towards wood working and sign making.
> http://enroutesoftware.com/
>
> What would the g-code look like for an HSM millout of something like the
> attached dxf. (
On 02/23/2017 09:35 AM, Jim Craig wrote:
> Yep, you should have done a HSM slot about 3/8" wide with the 1/4"
> cutter and you would have had little trouble. I try to avoid a
> conventional full width slot in aluminum where possible. lube definitely
> helps or is required.
>
>
Yes, the hardest part
ust slot milling everything, didn't want to
> make more mess milling bigger grooves than I had to.
>
> - Original Message -
> From: "Chris Albertson"
> To: "Enhanced Machine Controller (EMC)"
> Sent: Thursday, February 23, 2017 12:45:05 AM
&g
Albertson"
To: "Enhanced Machine Controller (EMC)"
Sent: Thursday, February 23, 2017 12:45:05 AM
Subject: Re: [Emc-users] Milling Aluminum.
Yes, WD40 works well on aluminum. I'm betting your wood mill is not
nearly rigid enough to cut metal.
What most people did early
What I'd do is have the holes rough cut on a CNC plasma table (they can cut
aluminum, with the right setup) then do full depth profile cuts with the wood
router gantry.
A lot of those cuts, just past the point of chip thinning.
http://www.mmsonline.com/articles/the-high-feed-high-reliability-pro
On 23 Feb 2017, at 05:46, Jon Elson wrote:
> On 02/22/2017 10:08 PM, Todd Zuercher wrote:
>> Yuck, if I don't ever have to mill that crap again it will be too soon.
>> Started out dry and trying to mill .12 deep per pass. 1st try (1" long ramp
>> in) tool ramped in to full depth nicely and the
ng up badly. Half a
> dozen bits later, having some success with a .06" cut depth @120imp and
> soaking it with WD-40.
>
> - Original Message -
> From: "Roland Jollivet"
> To: "Enhanced Machine Controller (EMC)"
> Sent: Tuesday, February 21, 20
On 02/22/2017 10:08 PM, Todd Zuercher wrote:
> Yuck, if I don't ever have to mill that crap again it will be too soon.
> Started out dry and trying to mill .12 deep per pass. 1st try (1" long ramp
> in) tool ramped in to full depth nicely and then promptly snapped, 400imp
> @18krpm is too fast.
g up badly. Half a dozen bits
later, having some success with a .06" cut depth @120imp and soaking it with
WD-40.
- Original Message -
From: "Roland Jollivet"
To: "Enhanced Machine Controller (EMC)"
Sent: Tuesday, February 21, 2017 3:17:27 PM
Subject: [Emc-users] Mi
Why don't you just get someone to water-jet cut, and carry on cutting wood?
On 21 February 2017 at 17:34, Todd Zuercher wrote:
> I am a wood worker in a large wood working CNC shop. But I need to mill
> some aluminum for a project (a jig for another process in our company) but
> I know next to
Are you cutting discrete parts out of the plate? IOW, will you end up with
multiple parts?
Is the support surface flat? Can you cut almost all the way through and
leave a .004/.006 membrane holding all the parts together?
I would use a reverse helix end mill to have the cutting force push the
mater
I got a bunch of scrap pieces of MIC-6 from a local scrap dealer for
pretty cheap so I have been making chips and widgets out of it for a
while now. It is dimensionaly stable but it does like to chip weld even
more than 6061.
Another little note about MIC-6 is that if you are cutting the last
Jim,
Good to know this I have a pice of MIC-6 arriving today I need to cut up
and machine it. I usually use 6061 and 7075.
JT
On 2/21/2017 11:37 AM, Jim Craig wrote:
> MIC-6 is particularly gummy when machining. I always use coolant and I
> still get a little bit of chip weld if things aren't
On 21 February 2017 at 15:34, Todd Zuercher
wrote:
> But I need to mill some aluminum for a project (a jig for another process in
> our company)
What CAM software will you be using? With the spindle speed you have I
suspect that a trochoidal path would work best.
(Fusion360
On 02/21/2017 11:37 AM, Jim Craig wrote:
> MIC-6 is particularly gummy when machining. I always use coolant and I
> still get a little bit of chip weld if things aren't just right.
>
>
Oh, and make the cuts with CLIMB milling direction, it will
make a HUGE difference, especially in the gummy mater
On 02/21/2017 09:34 AM, Todd Zuercher wrote:
> I am a wood worker in a large wood working CNC shop. But I need to mill some
> aluminum for a project (a jig for another process in our company) but I know
> next to nothing about milling such material. What I need is to cut a large
> grid out of a
On Tue, 2017-02-21 at 11:37 -0600, Jim Craig wrote:
> MIC-6 is particularly gummy when machining. I always use coolant and I
> still get a little bit of chip weld if things aren't just right.
I have a machine which comes without air blast nor coolant, I use spray
coolant WD-40
and I use a tool
On 21 Feb 2017, at 15:34, Todd Zuercher wrote:
> I am a wood worker in a large wood working CNC shop. But I need to mill some
> aluminum for a project (a jig for another process in our company) but I know
> next to nothing about milling such material. What I need is to cut a large
> grid out o
And I recommend 0.025" - 0.050" depth of cut.
N. Christopher Perry
> On Feb 21, 2017, at 11:53 AM, John Thornton wrote:
>
> The key to milling aluminum dry is cutting a chip big enough to pull the
> heat out with the chip. So big chips mean the part stays cool, and small
> chips means the too
MIC-6 is particularly gummy when machining. I always use coolant and I
still get a little bit of chip weld if things aren't just right.
Getting the chips out of the slot you are milling is also critical. I
would keep using the compressed air blast and i would probably use a HSM
slot instead of
On Tuesday 21 February 2017 10:34:30 Todd Zuercher wrote:
> I am a wood worker in a large wood working CNC shop. But I need to
> mill some aluminum for a project (a jig for another process in our
> company) but I know next to nothing about milling such material. What
> I need is to cut a large gri
The key to milling aluminum dry is cutting a chip big enough to pull the
heat out with the chip. So big chips mean the part stays cool, and small
chips means the tool will gum up and stick the aluminum. I like 2 flute
carbide from Lakeshore Carbide. They make end mills for steel and
aluminum th
I am a wood worker in a large wood working CNC shop. But I need to mill some
aluminum for a project (a jig for another process in our company) but I know
next to nothing about milling such material. What I need is to cut a large grid
out of a 5ft x 10ft sheet of 1/4inch thick MIC6 AL. The machin
48 matches
Mail list logo
