MAXNC 10 speeds and feeds question

This forum is dedicated to those Hobbyists Interested in CNC machining in their home shops. (Digital Read Outs are also topical, as is CAD/CAM as it relates to CNC)

Moderator: Harold_V

Post Reply
dorin
Posts: 533
Joined: Thu Nov 28, 2002 5:24 am

MAXNC 10 speeds and feeds question

Post by dorin » Fri Oct 12, 2018 6:10 am

I have a maxnc 10 I bought used and then had upgraded by the manufacture.
You can see a picture of one here https://c1.staticflickr.com/7/6240/6259 ... 15c9_b.jpg.

I see the manufacturer's website is down, I wonder if they are out of business?
I guess I am not too surprised based on my interactions with them.

I had my machine upgraded to be able to do aluminum. I was wondering about some suggested speeds and feeds for starting out
on this little device. When I asked the MAXNC folks, they could give me no advice.

Does anybody have one of these and or can anybody give me a good guess where to start?

I have 1/4" and 1/8" carbide end mills.
I also have some 3/16 HSS end mills.
I have no idea what my aluminum is! I bought a bunch of surplus squares from a junk shop!

Thank you,
MIke
www.chaski.com

User avatar
Dave_C
Posts: 955
Joined: Mon Apr 21, 2008 10:34 am
Location: Springfield. MO.

Re: MAXNC 10 speeds and feeds question

Post by Dave_C » Fri Oct 12, 2018 1:20 pm

Mike,

I have no idea what your top spindle RPM is on that machine but with 1/8" and 14" end mills I shoot for a spindle speed and a feed rate that will give me somewhere in the .001" or less per tooth for chip load. The smaller the end mill the lower I go so the 1/8" end mill needs something just under the .001" per tooth load.

I've gone to 3 flute coated carbide end mills for aluminum and I have no issues with chip welding. (no flood either, just a very light spray of WD-40) I run at max RPM for both the 1/4" and lower end mills which for me is 2800 RPM.

That comes out at about 7.5 to 10" IPM for the feed rate. I watch my chips and listen to the machine as it runs. I can over ride the feed rate if needed, either higher or lower depending on how it sounds.

I've been using Fusion 360 for CAD/CAM and it gives me the chip load when I set up a tool for any given RPM I may want to run. This saves time of doing the calcs by hand!


Dave C.
I learn something new every day! Problem is I forget two.

dorin
Posts: 533
Joined: Thu Nov 28, 2002 5:24 am

Re: MAXNC 10 speeds and feeds question

Post by dorin » Sat Oct 13, 2018 11:02 am

Thank you!
I never thought about it in those terms before.
-Mike
www.chaski.com

User avatar
Dave_C
Posts: 955
Joined: Mon Apr 21, 2008 10:34 am
Location: Springfield. MO.

Re: MAXNC 10 speeds and feeds question

Post by Dave_C » Sat Oct 13, 2018 2:58 pm

I'm not sure why it isn't taught that way from the beginning as "chip load" is really what determines the feeds and speeds.

So here are some sample calcs:

Let's say we can only run 3,000 RPM (Maybe too hi an example from some mills but a good starting point)

Let's use a 3 flute 1/4" carbide end mill that can turn aluminum at say 600-800 Surface feet per minute, not that we can ever get these small machines that high!

Target is .001" chip load per tooth or .003" inch per rev.

Now all we have to do is multiply the cut per rev times the RPM and that gives us the Feed Rate of 9 IPM. (.003 X 3,000= 9)

So let's do another example and let's say we can turn 5,000 RPM and we are using a 3 flute 1/8" end mill. Now we need a lower chip load as the flutes are quite small. So let's drop down to .00075" per tooth or a .00225" cut per rev times our 5,000 RPM and we get 11.25 Feed Rate.

So my point is that in CNC programing, the chip load per tooth should be the determining factor right up till you are limited by the surface feet per minute of the cutting tool and most of us can't hit that number in aluminum!

The larger the end mill the higher the chip load per tooth might be. So if I had to run a 3 flute 1/2" end mill, then I can go as high as .003" chip load per tooth or .009" per rev. (.009 x 3000 = 27 IPM feedrate) and (.009 x 5000 = 45 IPM feedrate) {provided you have the HP to make that cut}

Pretty simple way to do the programing, at least it works for me.

Dave C.
I learn something new every day! Problem is I forget two.

dorin
Posts: 533
Joined: Thu Nov 28, 2002 5:24 am

Re: MAXNC 10 speeds and feeds question

Post by dorin » Fri Oct 19, 2018 6:51 am

Oh, I forgot to ask..how deep would you cut?
(Or maybe I misunderstood your answer)
Thank you, I appreciate your help.
www.chaski.com

User avatar
DICKEYBIRD
Posts: 176
Joined: Sat Feb 03, 2007 10:45 am
Location: Collierville, TN

Re: MAXNC 10 speeds and feeds question

Post by DICKEYBIRD » Fri Oct 19, 2018 8:56 am

Great explanation Dave, thanks!
Milton in Tennessee

"Accuracy is the sum total of your compensating mistakes."

RCRR
Posts: 31
Joined: Mon Aug 19, 2013 11:53 am
Location: New Hampshire

Re: MAXNC 10 speeds and feeds question

Post by RCRR » Fri Oct 19, 2018 10:49 am

Hi Mike,
I actually own one of these machines and I really like it! I have the larger bed version with the 10k rpm spindle. I use it mostly for precision glass cutting using diamond tools (fully submerged in coolant, a very clean way to do it).

I make all my custom fixtures from scrap aluminum. I use a 1/4in coated 2-flute, no coolant...still gives a nice a finish. I run the spindle at full speed and plow through in manual mode to figure out what it can handle by ear and then go back and set the feeds.

User avatar
Dave_C
Posts: 955
Joined: Mon Apr 21, 2008 10:34 am
Location: Springfield. MO.

Re: MAXNC 10 speeds and feeds question

Post by Dave_C » Fri Oct 19, 2018 11:26 am

Oh, I forgot to ask..how deep would you cut?
(Or maybe I misunderstood your answer)
Thank you, I appreciate your help.
Good question: There are some standards that say never run the end mill deeper than 2 x its width. But they leave out the step over part when they say that. AT twice the diameter in depth the step over may be as little as 20% of the width of the end mill.

So I say play with it and see how it sounds and looks when it is cutting. I have a spindle load meter on my mill so I can watch spindle load. I've run cuts at 90% step over using a 3 flute carbide end mill coated for aluminum and the chips look great and the spindle load is about 35% of full amps.

Start small and work up! Little end mills don't like to cut deep or wide as they tend to break easily, especially HSS.

Dave C.
I learn something new every day! Problem is I forget two.

User avatar
ctwo
Posts: 2720
Joined: Tue Mar 27, 2012 12:37 pm
Location: Silly Cone Valley

Re: MAXNC 10 speeds and feeds question

Post by ctwo » Fri Oct 19, 2018 1:47 pm

Dave, that last part is worth repeating...
Standards are so important that everyone must have their own...
To measure is to know - Lord Kelvin
Disclaimer: I'm just a guy with a few machines...

Post Reply