Hi all,
By hot roll I assume you mean something like A36. Alloy comp not
controlled just mechanical. It tends to be low alloy scrap plus 4140.
Using a TiAlN coated 1/4 carbide I can use 2200 rpm and 11 ipm, doc
0.05, any more and it screams at me. This is basically slotting, on a
side cut same rpm, and feed, .7 doc for radial of only .025. Makes for
a lot of passes. This is on a Cinci contourmaster 1963 vintage,
converted to servos. Going deeper and slower doesn't seem to help. Since
TiAlN likes to run hot I machine dry. It is not unusual for small jobs
to run for a couple of hours.
On a machining site someone recommended ... increase the feed until you
break a mill, then back off 10%. Pretty aggressive.
Rumor has it that AlCrN coated carbide with flood coolant lasts a long
time; and that was in a production environment. If ... (when) I get my
big machine up I'll give more serious stuff a go.
I do a lot of A36 because it is cheap and OK for experimental work but
CR machines like a dream by comparison. HTH
Dave
On 2/18/20 10:09 PM, John Dammeyer wrote:
Thanks everyone. The trouble with the machinist workshop program and some of
the others is they are targeted at production speeds. I'm not even sure about
the alloy of Hot Rolled Steel which is what will be used here.
The part is designed to hook around the ears of a pipe crucible so accuracy
isn’t that big a deal and at the moment, HSS is all I have. With manual
machining, as Wallace said, you can turn the hand wheels and get a feel for
what it should do. And yes the machine is pretty rigid.
http://www.autoartisans.com/milton.htm This picture was when it first arrived.
I do have a coolant pump but have yet to use it. Not sure what kind of coolant
to use. A large part of my machining has been aluminium castings. I've not
yet set up mist coolant. Any suggestions for what type of coolant to use for a
machine that is only used occasionally?
All things considered the CNC conversion is the easy part. My heart is always
in my throat a bit when first start running a CNC program. That's the really
hard part.
John
-----Original Message-----
From: Stuart Stevenson [mailto:stus...@gmail.com]
Sent: February-18-20 7:04 PM
To: Enhanced Machine Controller (EMC)
Subject: Re: [Emc-users] Feeds and speeds
John,
Do you have flood coolant or mist coolant?
I would be inclined to try the cut full depth if you have flood or mist
coolant. 1/4 inch is on the borderline of having the strength necessary to
make a full depth cut. I would think 5.5ipm might be a little aggressive
but I would leave it programmed at that feed and speed and turn the
feedrate to about 20% to start the cut. After you get into the cut I would
move the feedrate up about 10% to see, hear and feel how mill is cutting. I
would keep moving the feed up until I saw, heard or felt the mill working
too hard. I would then start turning the speed up a little at a time to see
how the mill responds.
I think 30sfm might be a little slow but you can adjust the speed after
entering the cut.
If you can adjust the feed and speed to make the full cut sound good and
you have another part to run I would change your program to enter the cut
as you did the first time but the add lines to make it more aggressive
after you have entered the cut.
If you are leaving a little material to clean up the you can drastically
increase the speed and feed after you turn around at the end of the slot.
Is the slot you are cutting wide enough to allow at least .010 thou. for a
finish pass and maybe a spring pass.
I would make the finish pass and spring pass in a conventional cut rather
than a climb cut.
Stuart
On Tue, Feb 18, 2020 at 8:47 PM John Dammeyer <jo...@autoartisans.com>
wrote:
I've got Mecsoft AlibreCAM generating the tool paths for this in the
attached photo. It's Cold Rolled steel 3/16" thick. I'm using a 1/4" HSS
end mill. I'm trying to figure out, using Machinists tool box, exactly
what feeds and speeds could be used for milling the slot.
I was thinking 30 SFM and with a 4 flute end mill doing 0.003" per flute
the toolbox comes out with 460RPM, 5.5ipm for S460 and F5.5 and 10% of
tool diameter for depth per pass so 0.025"
Is that too conservative or likely to break something? Doing it manually
I'd do it by feel but once it's automatic it's harder to decide SFM and
chip load.
Thanks
John
_______________________________________________
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users
--
Addressee is the intended audience.
If you are not the addressee then my consent is not given for you to read
this email furthermore it is my wish you would close this without saving or
reading, and cease and desist from saving or opening my private
correspondence.
Thank you for honoring my wish.
_______________________________________________
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
