[acannell]

I am trying to actually make a few bucks selling parts with my sherline, so its important to be able to remove as much material as possible as quickly as possible.

I seem to be getting consistently good results with a 3 flute roughing end mill in 6061-T6511. Its a Niagara 75215 roughing end mill, available from mcmaster.

This wasn't my idea, I first saw this endmill (very similar) being used here:

Roughing End Mill | North Branch Reels

At 0.050" doc, 9 ipm, with a full width 1/4" diameter slot, seems to be okay. It makes noise, but it doesn't sound like bad noise. (see video below) That said, I've only been machining for about 3 months.

I can also plunge very quietly (almost no noise at all actually) at 0.3ipm. In the video, it might seem to make alot of noise during the plunge, thats because my spiral lead in move is really jamming the end mill in..didnt fix that in time. But when its a straight plunge at 0.3ipm, its silent.

Also, I've noticed that at 12ipm it sometimes sounds even quieter. Not always, but sometimes. Its not stable enough at 12ipm for me to use it regularly.


YOUTUBE Sherline Aluminum .050" doc, 9ipm, 6061

The video shows me cutting at 9ipm, this isnt a fresh endmill, I've used it to make about 7 similar brackets so its got whatever wear that might cause to it.

The mill is setup with fairly light gib tightness, and backlash around 3 thou.

I'm pretty happy because this lets me make 6061 parts in reasonable amounts of time. The tool path for the pictured part is about an hour with manual tool changes.

Im wondering if an experienced machinist could tell me how I could analyze the machining results at this speed to tell if its really appropriate or not. I guess the finished parts tell the whole story, but I'm wondering if maybe there is more to it than that.

Also, I wonder if I can get the speed up to 12ipm regularly, or even 15ipm? How can we make this faster?

[GeneK]

I can't tell for sure but it sounds to me like you are using the 2800 rpm spindle. I use the 10 K spindle and run about 7 or 8K I think you should be able to get to 10 or 12 IPM.

GeneK

[acannell]

I can't tell for sure but it sounds to me like you are using the 2800 rpm spindle. I use the 10 K spindle and run about 7 or 8K I think you should be able to get to 10 or 12 IPM.

GeneK

Yep thats right, the 2800 spindle. You just mean the pulley swap right? I keep the motor?

muhahha sounds awesome, I cant wait to try it

[SCzEngrgGroup]

If you're RPM is 2800, then 9 IPM is exactly where you should be with that DOC. If you can increase RPM, increase feedrate proportionally, up to about 31 IPM at 10K RPM.

Regards,
Ray L.

[acannell]

If you're RPM is 2800, then 9 IPM is exactly where you should be with that DOC. If you can increase RPM, increase feedrate proportionally, up to about 31 IPM at 10K RPM.

Regards,
Ray L.

Awesome!!

Does cutting at the higher ipm and spindle rpm require more or less rigidity of the teeny sherline?

[acannell]

Also, the sherline can only feed at 22ipm maximum, what spindle speed would make the most sense there assuming 1/4" slot and .050"doc..or does a different doc and radial engagement make sense?

Is there a way to find the sweet spot of max material removal balanced with vibration tolerance or is it trial and error?

[SCzEngrgGroup]

Also, the sherline can only feed at 22ipm maximum, what spindle speed would make the most sense there assuming 1/4" slot and .050"doc..or does a different doc and radial engagement make sense?

Is there a way to find the sweet spot of max material removal balanced with vibration tolerance or is it trial and error?

Finding the ideal feed/speed for a particular machine is a matter of trying different values, and seeing what works best. Every machine is different. Too slow, and you'll start loading the tool and generating hear. Too fast, and surface finish will degrade. Running 2800 RPM and 9 IPM, or 10000 RPM and 31 IPM, you're running about the same chipload, so impact of rigidity will be roughly comparable, though the higher speed will require ~3X the spindle power.

Download a copy of FSWizard, and use that as a guide, then do some experimentation: http://zero-divide.net/index.php?page=FSWizard_SA

Regards,
Ray L.

[GeneK]

Also, the sherline can only feed at 22ipm maximum, what spindle speed would make the most sense there assuming 1/4" slot and .050"doc..or does a different doc and radial engagement make sense?

Is there a way to find the sweet spot of max material removal balanced with vibration tolerance or is it trial and error?

I also upgraded to the A2Z kirk lead screws and with the 4 tpi screws you get rapids around 40 ips with the Sherline steppers. If I get rich I plan to go with the Gecko and a little larger steppers. Again I highly recommend the 10K pulley set for the Sherline.

GeneK

[Fastest1]

Why are you limited to 22ipm? I have had stock screws and could go much faster than that. I have the A2Z now and can approach 300ipm rapids. None of those speeds are useable but they are attainable. Are you using Mach?

[acannell]

Why are you limited to 22ipm? I have had stock screws and could go much faster than that. I have the A2Z now and can approach 300ipm rapids. None of those speeds are useable but they are attainable. Are you using Mach?

The stock sherline system has that limit. I'm not sure if its the driver electronics or the motors themselves. I use cambam and emc2, and Im sure emc2 could have its hal modified to have faster speeds.

I'm actually okay with 22ipm. I tend to hand massage (thats what she said) the cambam toolpaths to eliminate rapids and also hand modify the gcode if needed to get unneeded rapids out, so I dont really need any faster, plus I cant really machine stuff faster than that anyway.

[hndswthtshdws]

You can change the rapid speed in Mach. If you not comfortable with 22 ipm, set it to 10 ipm or whatever. I don't see any reason for hand massaging code for this, even if it is as simple as a find and replace.

[acannell]

You can change the rapid speed in Mach. If you not comfortable with 22 ipm, set it to 10 ipm or whatever. I don't see any reason for hand massaging code for this, even if it is as simple as a find and replace.

I dont care about the rapids being 22ipm, I care about the rapids existing at all. My cam software doesnt always create the most efficient gcode, especially when I start putting keepout areas inside toolpaths for parts with multi-stage fixtures.

[Fastest1]

Still running a 1/4-20 screw and 1.8 degree steppers?

Why would you remove the rapids? Especially if your max is only 22ipm. You did mention making money in the same sentence. I am confused.

[acannell]

Still running a 1/4-20 screw and 1.8 degree steppers?

Why would you remove the rapids? Especially if your max is only 22ipm. You did mention making money in the same sentence. I am confused.

i mean removing any motion of the axes that isnt cutting material, i.e. pointless rapids from place to place. low cost cam software tends to generate alot of that inside pockets with islands, ive noticed. so sometimes i edit the code to make the toolpath one continuous journey, or as close as possible to that..plus rapids are hard on the machine.

[ChrisAttebery]

Is that roughing EM doing anything for you? Usually they are used in deep cuts where you want to break up the chips. On a .050" cut you probably have one or two teeth that actually aren't doing any cutting.

[acannell]

Is that roughing EM doing anything for you? Usually they are used in deep cuts where you want to break up the chips. On a .050" cut you probably have one or two teeth that actually aren't doing any cutting.

I think it has some other geometry that may be helping because I could not cut anywhere near this fast when I was using a 3 flute standard endmill at the same doc.

[acannell]

wow...

so I picked up a 5400 non-cnc sherline mill...it immediately feels MUCH more rigid than the bells-and-whistles 8 direction 2000 series I've been using that has a huge cantilevered swingarm that the z axis is connected to...

so i put on my trusty 3 flute roughing endmill and decided to do a side by side comparison...

i could tell the 5400 mill spindle was running slower than my 2000 series..not sure if something is wrong with it or if its just an older model..

so i turned it up full speed and plunged into the 6061...TOTALLY DIFFERENT response than the 2000 series..felt like i was just drilling...on the 2000 you immediately get hard resonating and chattering...on the 5400 when i started plunging to fast it was a much softer "choking"..

then i tried a 0.050" deep full slot..9ipm was my standard max speed on the 2000, and that should be 3 turns of the handwheel per second...it went very nicely in the 5400..so nicely that i could turn the handwheel as fast as i could and it seemed to be cutting okay. so i went another 0.050" deep..for a 0.1" deep full slot...and it was STILL OKAY!!! that means I may be at 12ipm or something 0.1" deep!!

then i switched to the 2000 series and could barely plunge without heavy chattering..and when i tried to do a 0.1" deep cut it was LOUD resonating...

this is all pretty imprecise since its all by hand speed, but its enough for me to take the cnc parts off the 2000 and put them on the 5400....losing the 8 directions and deeper Y axis is fine with me if I can cut more than twice as fast through aluminum..

once the cnc parts are on, I'll run my usual toolpath for an aluminum part I make, and Ill bump the DOC and feedrate up to see how it goes!

i wonder how much better it would be with the 10000rpm spindle too!

stay tuned!

[acannell]

okay i put all the cnc parts on the 5400 mill and then ran a couple proper cnc controlled cuts...

first I tried 0.050" deep, full slot, at 12ipm...handled it very well..seems as quiet or quieter than 9ipm on the 2000

then..i tried 0.100" deep, at 9ipm...

STILL SEEMED QUIETER than 0.050" at 9ipm on the 2000!!!

so if you are serious about making aluminum parts on the sherline, avoid the 2000 like the plague. the 5400 is more than twice as fast..
.
and this is with the headstock spacer block which looks to be more than an 1" thick.

i will be doing ALOT more tests in the near future to see where my new limits are on this machine.

also, I ordered the 10k pulleys today, so that may make it possible to increase the material removal rate even further somehow, hopefully there is some sweet spot somewhere in the feed/speed spectrum that will really get chips flying and i bet its at a higher rpm than 2800

and im planning on adding a coolant system too, i got a new enclosure for the mill and ill be adding a sump and pump.

i dont really think anybody else gives a crap about all this but whatever, if i can make aluminum parts at 50% the speed of a cnc bridgeport id be thrilled, even if they can only be 5" square lol

ill take videos and pictures once i actually run a full toolpath

[NSR_CIVIC]

There are a few of us sherline/ spectralight guys left around here..

Kevin.
Nsr customs.

[acannell]

Okay...got the 10K pulleys installed..

Now I can run at 0.070" DOC, 0.250" full slot with roughing endmill, at 18IPM, no problem, sounds like a router and is very even..doesnt seem like its trying except you can hear the motor rpm change slightly as the load increases occasionally, I'm pretty sure I'm maxing out the torque from the motor at full RPM. I even tried 0.150" DOC at 9ipm (I think) and it seemed to handle it.

I'll have more precise data soon. I know I keep saying that, but everything is in flux. The mill isnt even on a base, and its sitting in a metal pan I made for flood coolant which isnt welded and just rocks around. When I get the flood coolant going, or at least mist, I'll try and see where the new feed and speed limits are.

What appears to be a certainty is that if you are trying to cut down on time when making thick aluminum parts, the 5400 and the 10k pulley set are MUSTS.