Using small end mills on a lower-RPM machine (PCNC 1100)
I'm making some folding knives on my PCNC 1100, and in order to machine the lock bar (pic here) I'm using a 1/16 end mill, .25" flute length. And I'm having trouble determining the best feeds and speeds given the Tormach's 5100rpm spindle limit.
I plugged the end mill geometry and specs (mfg recommends 500SFM, 0.001 chip load) into GWizard, and it's recommending a speed of around 25k RPM. From what I've read, that's generally where these small end mills perform best at. Unfortunately, my machine can only do 20% of that.
If I limit the speed to 5100RPM, I'm having a really hard time getting reasonable feeds and depths of cut out of Gwizard without seeing the tool deflection number go red. It's suggesting a feed of 1 IPM with a 0.01" depth of cut. At that rate, my lockbar cut would take over an hour. And the tool is moving so slowly that I'd be concerned about rubbing.
Any best practices to keep in mind when using small end mills on a low-rpm machine?
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
You must not have GWizard set for a PCNC1100 if you are getting that high of a rpm.
I have cut some features using a 1/16" end mill in steel and aluminum with my 1100, I used GWizard and ran quite a few of the parts. Depth of cut is the critical part of GWizard, everything else it figures out great. I have 100% faith in its outputs. Just remember GIGO.
I always rough my material down with larger end mils and then finish with the smaller to get the needed small radius cuts, another trick is to drill out the corner first.
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
On my machine (novakon pulsar) I cut the lockbar at 5200rpm and about 1 IPM w a 1.8mm (0.07) 4 fl endmill in titanium. It takes about 30min to cut. http://uploads.tapatalk-cdn.com/2016...e16faacdac.jpg. It's too small a cut for any hsm strategies so it's straight my slotting.
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
Quote:
Originally Posted by
R.DesJardin
You must not have GWizard set for a PCNC1100 if you are getting that high of a rpm.
I have cut some features using a 1/16" end mill in steel and aluminum with my 1100, I used GWizard and ran quite a few of the parts. Depth of cut is the critical part of GWizard, everything else it figures out great. I have 100% faith in its outputs. Just remember GIGO.
I always rough my material down with larger end mils and then finish with the smaller to get the needed small radius cuts, another trick is to drill out the corner first.
I did temporarily override the max RPM setting to see what GWizard would recommend *if* it wasn't RPM-constrained.
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
Quote:
Originally Posted by
brianbonedoc
On my machine (novakon pulsar) I cut the lockbar at 5200rpm and about 1 IPM w a 3mm (.078) 4 fl endmill in titanium. It takes about 30min to cut. It's too small a cut for any hsm strategies so it's straight my slotting.
Interesting, thanks for that example. What depth of cut were you running?
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
Quote:
Originally Posted by
brianbonedoc
On my machine (novakon pulsar) I cut the lockbar at 5200rpm and about 1 IPM w a 3mm (.078) 4 fl endmill in titanium. It takes about 30min to cut.
...
It's too small a cut for any hsm strategies so it's straight my slotting.
Just for clarity, was it a 2mm end mill or a 3mm end mill?
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
Total novice with no experience but when I was limited to 5000rpm and using sub 3mm mills I had most success with 1 or 2 flute mills allowing me to increase feed rate to prevent rubbing.
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
OOPS - I meant a 1.8mm end mill. Corrected post above.
I just checked Fusion 360 and my recipe is this.
Machining time: 10min 47s
Feed distance: 42inches
1.8mm 4fl TiN coated EM.
5200 rpm
0.00019 feed/tooth
DOC= 0.035
Slotting
4 ipm
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
It is literally a trivial exercise to add a 30K rpm 1 hp router spindle to the 1100, co-linear with the main spindle. The cost is about 8-9" of the 17" Z movement, maybe 200 bucks out of pocket, and 4 hours to build. Use a DeWalt or other variable speed router spindle, and precision collets from Precisebits. No air or water cooling, no offset- X & Y axis has full range. Having built one, my 1100 has a speed range of 100-30,000 rpm. (I do need to add a breakout board to control the spindle with M codes- manually turning on right now). Given the length and typical DOC for small cutters, one is simply putting wear in a part of the Z axis that doesn't get used much. I use the high speed spindle for anything under about 1/8"; haven't had the nerve to try a 1/4" carbide cutter in Al at 10K. I'm running a 1/32 EM at 45 ipm, 0.018 doc slotting in acrylic, could probably do 60 ipm with no trouble.
Build a high speed spindle adapter and have the best of both worlds- the envelope of the 1100 and more speed than the second gen speeder.
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
Can you post a picture show in your setup? If if I understood correctly you are saying that your router spindle is coaxial with the main spindle? How do you accomplish this?
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
I made a plaque to go on my mother in laws casket when she passed away.
I made it out of 1/8 X 4 inch brass bar.
I ruffed it with a 1/4 inch end mill, then took the corners out with a 1/16 end mill then I engraved her favorite Bible verse with a .010 end mill.
I bought 6 cutters and I busted 3 of them getting the verse done.
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
I run my 1/16 2f carbide bits@4ipm, usually only 0.02in deep, doing patterns, honeycomb pattern reverse from the knife shown previously it's basically ding a bunch of little pockets, I do 5ipm down to 40tho deep sometimes but I go firm to 4ipm to do engraving that is up to 20tho deep so I get a nicer finish. Here's done of the stuff I've done, the bb8 is 0.1in deep, I did that at 4ipmhttp://uploads.tapatalk-cdn.com/2016...b32c634b80.jpghttp://uploads.tapatalk-cdn.com/2016...9849cc50a3.jpghttp://uploads.tapatalk-cdn.com/2016...9fc85589ec.jpghttp://uploads.tapatalk-cdn.com/2016...86dae3f4c6.jpg
This one is 0.15 deep in every hole.
http://uploads.tapatalk-cdn.com/2016...b033507db0.jpg
I just got a tialn coated 2fl ball, most of that engraving was done with a ball end mill, I'll see how hard I can push that little guy and let you know if you want.
Sent from my SM-G900V using Tapatalk
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
Quote:
Originally Posted by
tbev
I run my 1/16 2f carbide bits@4ipm, usually only 0.02in deep, doing patterns, honeycomb pattern reverse from the knife shown previously it's basically ding a bunch of little pockets, I do 5ipm down to 40tho deep sometimes but I go firm to 4ipm to do engraving that is up to 20tho deep so I get a nicer finish. Here's done of the stuff I've done, the bb8 is 0.1in deep, I did that at 4ipm
Looks pretty great. What machine and spindle speed was this on? Thanks!
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
Quote:
Originally Posted by
GLCarlson
It is literally a trivial exercise to add a 30K rpm 1 hp router spindle to the 1100, co-linear with the main spindle. The cost is about 8-9" of the 17" Z movement, maybe 200 bucks out of pocket, and 4 hours to build. Use a DeWalt or other variable speed router spindle, and precision collets from Precisebits. No air or water cooling, no offset- X & Y axis has full range. Having built one, my 1100 has a speed range of 100-30,000 rpm. (I do need to add a breakout board to control the spindle with M codes- manually turning on right now). Given the length and typical DOC for small cutters, one is simply putting wear in a part of the Z axis that doesn't get used much. I use the high speed spindle for anything under about 1/8"; haven't had the nerve to try a 1/4" carbide cutter in Al at 10K. I'm running a 1/32 EM at 45 ipm, 0.018 doc slotting in acrylic, could probably do 60 ipm with no trouble.
Build a high speed spindle adapter and have the best of both worlds- the envelope of the 1100 and more speed than the second gen speeder.
Very interested to see some pictures of your setup.
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
Tbev please share your coolant system info/pics on this forum. I have a project coming up and very interested in learning how to accomplish this process.
Thanks...-uman
Re: Using small end mills on a lower-RPM machine (PCNC 1100)
Quote:
Originally Posted by
Uman
Tbev please share your coolant system info/pics on this forum. I have a project coming up and very interested in learning how to accomplish this process.
Thanks...-uman
http://www.cnczone.com/forums/tormac...pc11-flow.html
PC11 FLOW!
Pics and vid, most of the things I did you can do for free.
Sent from my SM-G900V using Tapatalk
