Share and compare your Mikini 1610L cutting data here

I would like to get a thread started that specifically pertains to cut parameters on the Mikini 1610L in an effort to gauge the capabilities of the machine. Please add your info about DOC, WOC, material, cutter, RPM, finish, chatter, etc. and your thoughts about the cut, good or bad.

I'll start:

4140 HT
.5 TiALN 4fl flat 1.25 endmill
1860 rpm
10ipm
.23 DOC
.35 WOC
.57hp

This cut stalls the spindle within 2 sec.



4140 HT
.5 TiALN 4fl flat 1.75 roughing endmill
2317 rpm
3.2ipm
.23 DOC
.125 WOC
.07hp

This cut is fairly decent but increasing the feed much more will stall the spindle.

Oak
.75 HSS 4fl flat
5000 rpm
75 ipm (25 ipm Z)
.50 DOC
.75 WOC
hp? 4.21 per GWizard, I think.

Good finish, very fast, no issues cutting, spindle did not slow down. Total cut was about 2 inches per level, 3 levels.

Swath, just noticed this video... Mikini cuts 4140 at 4000 rpm... Are you just being too conservative? Also, they way you list your tools, what are the tool numbers? Diameter and length, collet diameter and cutting diameter, ? and??

Mikini cnc 1610L - VMC 2.5 profile Press Die in 4140 hard steel - YouTube

4000 is about right for a .375 endmill, mine was a .5 endmill. My terminology is .5 cutting diameter, and 1.25 is length sticking out of collet (which affects feedrate due to deflection). I'm using Gwizard with the actual tool data from Maritool plugged in the program. I guess I'm going to have to start turning up the SFM to maximize enough torque to get these cuts. I tried this cut again:

4140 HT
.5 TiALN 4fl flat 1.75 roughing endmill
2317 rpm
3.2ipm
.23 DOC
.125 WOC
.07hp

It actually cuts pretty well, I turned up the feed rate to about 10ipm and it kept getting louder and louder until I was afraid of a spindle halt although the spindle load did not increase that much, I believe during a heavy cut it was about 21%. I readjusted the hall sensor ring to get the low load and have forgone the max rpm capabilities for now while Mikini looks into my video and figures something out. It still gets to about 3300rpm.

Your right though, it seems the Mikini needs a high rpm to achieve heavy cutting as that is where the torque is.

I was quite afraid of stalling my spindle the other day, doing a 1.5" DOC and loaded up to 60%. It kept pegging in to the red on the needle load gauge, but kept on chugging away. I did the same cut about 20 times and it never had a problem. I'm thinking higher RPMs matched with higher feed rates is the way to go...

Ok Here is some very useful info I got from Phil especially if you use Gwizard. Most of you probably already know this but the the HP of the spindle is linear and it peaks at 3hp when at 5000rpm (machine programed max). So if you use the newest 1.6 version of Gwizard there is a function in the machine setup tab where you can input this info. The feature is called spindle power curve compensation. For the Mikini you can enter the low range at 200rpm (minimum) and high range 5000rpm (maximum), then you can put the peak at 5000rpm and 3hp. It will then scale your max hp value when you are using the speeds and feeds calculator.

Here is the write up of this feature in the latest installment (ver. 1.6 10/31/11):
http://www.cnccookbook.com/

So low RPM is 200, power is what?
Peak is 5000, 3
High is 5000, 3

Looks like your link is broken too, but I found an explanation of it here:

G-Wizard Machinist's Calculator: Change Log

It looks a bit broken to me. It isn't taking the HP rating at the low RPM. If I put 0, 0.5, or 3 hp there, it gives funky interpolated values at other RPMs... Trying to find a bug report on their site...


Don't I recall Phil stating that he is now rating the motor at 4 hp?

Couple of questions for experienced machinists.

1. What are good speeds and feeds and DOC for finish boring with a carbide boring bar in 4140HT? In general.

2. What is a good 1/2" shank indexible boring bar and insert?

3. Where can I find .7-.74 carbide drills?


I'm trying to get a smooth .7495" and 2.25" deep bore.

I first started off helical ramping with a .5" endmill all the way down. This is slow and tends to chip the corner of the flutes.

I then tried drilling a .5" hole all the way through, then opening it up to .74 with spiral interpolation with an end mill. Then boring out to .7495. This is also slow and I'm getting a lot of chatter and a horrible finish with the finish boring (could be the cheap Chinese carbide boring bars, or the DOC could be too light). I know that with boring too light of a cut will result in rubbing and deflection so what is a good DOC to have in 4140 HT steel to avoid this? What are your experiences?

By the way drilling with a .5 carbide drill is amazingly quiet, smooth, and fast. Here are the metrics (I'll make a video once I compile enough cutting footage to make it interesting).

4140 HT
.5 x 2.75" carbide drill
s1144
f2
DOC .1 at a time down to 2.6"

Here is the code:

G00 G49 G40.1 G17 G80 G50 G90
G20
(Standard bore drill )
M6 T20 G43 H20
S1144M03
M8
G00 Z0.3500
X1.2942 Y0.5050
G83 X1.2942 Y0.5050 Z-2.6036 R0.1 Q0.1 F2.0
G80
G00 Z0.3500
M5 M9
M30

I ended up going ahead and getting this one:
http://cgi.ebay.com/ws/eBayISAPI.dll...E:L:OC:US:1123

Holy crap larger carbide drills are expensive! Around $200 for a 47/64.

You will find insert type bars are going to squeal and chatter, I have a solid carbide one with a triangular insert similar and it's terrible. I have much better luck with a brazed carbide bar from Micro 100, keep the corner pretty sharp and it will cut pretty well. Your problem is depth, any boring is going to pack chips in the hole and cause you nothing but grief.

You would probably be better off to drill with your 1/2" carbide, use a reground 3/4" endmill to open the hole to around .740", maybe .745 tops and then just use a .7495 reamer. Your finish should be good, and your size will stay stable.

If you got lucky, you might even get a 3/4" endmill to cut .7495... but then it could cut .7503 or something too.... so a crap shoot there. Still need to rough it within .010" or so though.

Thanks for the advice Brian. I anticipated the chip clearing problem so I went ahead and designed the bore as a through hole so the chips can fall through the bottom. For right now I think I'll stick with .5 drilling then opening it up with a .5 end mill to finish. Even though drilling then finishing and skipping the milling step would save a lot of time and can't justify the cost of a large drill bit or end mill just yet. BTW how does HSS drill work in 4140 HT vs carbide? They are significantly cheaper but I would think they would dull pretty quick.

The cheap brazed carbide bar I was using actually cut pretty good for the first 1/4 before is started chattering bad.

So would you finish bore at .01 DOC?

HSS should work just fine, this 4140HT isn't that hard, correct? Like under Rc 45? You won't get hundreds and hundreds of parts before the tools get dull, but 50-100, no problem.

Boring is so dependent upon the machine, hard to say what you can get away with, but start with slow rpm... probably under 500, finish pass around .010" total on the diameter, so .005" DOC and you will have to keep the feed rate up there a bit, try 3 ipm or so....

This is where it gets tough, too slow and it will chatter, fast enough to not chatter and you get ridges in the finish.... kind of why I recommended a reamer, especially with a thru hole, you could use a HSS reamer and it would blow through there.

Guess I need to get some good drills...

I've ordered some HSS drills so I'm going to try that.

Here is some more cutting data:

Full slot roughing:

4140 HT
.5 TiALN 4fl flat 1.75 roughing endmill
1850 rpm
11ipm
.04 DOC
.5 WOC full slot

Very good cut with no chatter going any faster or deeper starts to chatter.


Facing:

4140 HT
3.15 6 insert Sumitomo coated carbide 45deg face mill
800 rpm
14ipm
.005 DOC
2.5 WOC

This cut is smooth and leaves a beautiful finish. The depth can be increased some but going down to .05 DOC stalls the spindle. At 1.00 WOC you can go down to .01. Although keeping to .005 or less leaves a better finish regardless of WOC.

I'll have another video up before too long.

Here are a couple of videos. The first is just some random footage with my old camera and he second one contains cutting data and is HD. Please comment on the cuts. The deep part of the cut on that profiling op I'm going to try to vice two stock blanks together and drill it out first to remove the bulk of the material, then maybe I can speed it up a bit with the end mill.

[ame=http://www.youtube.com/watch?v=FrIEARRMRB8&feature=related]Mikini 1610L random machining ops - YouTube[/ame]

[ame=http://www.youtube.com/watch?v=_q8rKEAw3z0]Mikini machining ops with new camera in HD - YouTube[/ame]

Swath,

Some of that was almost painful to watch.... especially the boring head. OK, first, I'm not sure where you are getting your feed and speed data, but you are off, by quite a bit.... too much rpm in just about all of your cases and not even close to enough feed rate.

I don't know what size of an endmill you are using to profile your barrel part, but it looks to me like it might be a 1/2" diameter and you are trying to profile 3" deep. If you only want to make say under 20 pieces, struggle along any way you can.... if you want to make these fast and efficiently, you'll have to change things up.

First, start with a "normal" length 1/2" endmill, it'll have 1" depth of cut, go around your part until it won't reach any longer, then get an endmill that will reach the length you need, but, with a 1/2" flute length, a long shank and reduced diameter shank, i.e. it will measure .490" or so while the endmill cuts .500". This will be worlds stiffer, and given you are only taking fairly shallow depths of cut, it'll work much better.

Then at the end, if you have to, use your full length endmill.... now, here, I don't know what your tightest corner radii is, but if it's .25, then don't use a 1/2" endmill, you want to never "bury" it into a corner, you want to be profiling at all times, so if the radii is .25", then try to find a 7/16" or preferably 3/8" endmill to finish with.

Speeds and feeds..... rough numbers..... first lets talk feed, it should never be less than about 1/100th of the diameter of the endmill, so for 1/2" it should be .005", and that is per tooth.... so if you are running a 4 flute it will be .020" per revolution, given your 2000 rpm I saw most of that running at, you should be feeding closer to 40 ipm.

Now, I think your rpm's are too high also, but hey, if you ain't smokin' endmills, more power to you. We figures aluminum and brass... wide open, give it all she has for rpm... with carbide, you won't get too fast.... think we used to figure 600sfpm for HSS in aluminum. For mild steel carbide drops back to about 200 sfpm (roughly), given some of the better coated inserts, that could be 400, but for your run of the mill carbide endmill, again, unless it has special coatings, 200 is a good ball park. You said this was 4140ht, so I'd back that number down to maybe 150 to start with.

Once you have your rpm and feedrate, your hp is extremely limited, so you will have to vary your depth of cut and step over to accommodate the hp available. You will find once you have the right rpm and feed, you will be cutting the material off rather than rubbing and chattering like you are now.

I know it takes a leap of faith and it's a butt puckering moment to plow right in there, but you'l find out in short order the tools will work better and the machine will remove metal faster when things are dialed in. You will break a few tools learning what you can get away with, but in short order you will know what will work.

Oh, the boring head it's a rare instance you can spin one over 500-700 rpm... try backing that puppy way down and see what happens when you try to bore a hole... you should get a long, continuous stringy chip..... usually makes a bird's nest all around the tool... then it's cutting like it should.

One more comment on the boring bar. About the 4th or 5th attempt you can see your part drop in the vise. You then proceed to bore it a few more times at the tipped down angle. Are you using parallels under the part? You need to have good support under the part not just the clamped vise jaws. If you can lay the part at the bottom of the vise even better (which I think you could in this case). Don't be bashful on clamping the vise down tight!

Quote:

---

Originally Posted by Brian L

Swath,

Some of that was almost painful to watch.... especially the boring head. OK, first, I'm not sure where you are getting your feed and speed data, but you are off, by quite a bit.... too much rpm in just about all of your cases and not even close to enough feed rate.

I don't know what size of an endmill you are using to profile your barrel part, but it looks to me like it might be a 1/2" diameter and you are trying to profile 3" deep. If you only want to make say under 20 pieces, struggle along any way you can.... if you want to make these fast and efficiently, you'll have to change things up.

First, start with a "normal" length 1/2" endmill, it'll have 1" depth of cut, go around your part until it won't reach any longer, then get an endmill that will reach the length you need, but, with a 1/2" flute length, a long shank and reduced diameter shank, i.e. it will measure .490" or so while the endmill cuts .500". This will be worlds stiffer, and given you are only taking fairly shallow depths of cut, it'll work much better.

Then at the end, if you have to, use your full length endmill.... now, here, I don't know what your tightest corner radii is, but if it's .25, then don't use a 1/2" endmill, you want to never "bury" it into a corner, you want to be profiling at all times, so if the radii is .25", then try to find a 7/16" or preferably 3/8" endmill to finish with.

Speeds and feeds..... rough numbers..... first lets talk feed, it should never be less than about 1/100th of the diameter of the endmill, so for 1/2" it should be .005", and that is per tooth.... so if you are running a 4 flute it will be .020" per revolution, given your 2000 rpm I saw most of that running at, you should be feeding closer to 40 ipm.

Now, I think your rpm's are too high also, but hey, if you ain't smokin' endmills, more power to you. We figures aluminum and brass... wide open, give it all she has for rpm... with carbide, you won't get too fast.... think we used to figure 600sfpm for HSS in aluminum. For mild steel carbide drops back to about 200 sfpm (roughly), given some of the better coated inserts, that could be 400, but for your run of the mill carbide endmill, again, unless it has special coatings, 200 is a good ball park. You said this was 4140ht, so I'd back that number down to maybe 150 to start with.

Once you have your rpm and feedrate, your hp is extremely limited, so you will have to vary your depth of cut and step over to accommodate the hp available. You will find once you have the right rpm and feed, you will be cutting the material off rather than rubbing and chattering like you are now.

I know it takes a leap of faith and it's a butt puckering moment to plow right in there, but you'l find out in short order the tools will work better and the machine will remove metal faster when things are dialed in. You will break a few tools learning what you can get away with, but in short order you will know what will work.

Oh, the boring head it's a rare instance you can spin one over 500-700 rpm... try backing that puppy way down and see what happens when you try to bore a hole... you should get a long, continuous stringy chip..... usually makes a bird's nest all around the tool... then it's cutting like it should.

---

Thanks a lot Brian that is exactly the type of feedback I was hoping to get. I am getting my data from Gwizard using the parameters of the tool from Maritool (most of which I use are TiALN carbide). The problem is that when I feed at the rates recommended by Gwizard, even with the most conservative numbers it stalls my spindle. So I dial back the feed until it doesn't stall and doesn't chatter too bad. I keep the rpm to what Gwizard recommends because I've learned that the spindle has no power at the low RPMs and if I dial the rpm back accordingly it stalls the spindle. The spindle is extremely easy to stall and will do so with even a very modest cut. At say 700rpm we are only dealing with .3hp. I don't know if this is a limitation of the BLDC technology or a shortcoming of my particular spindle motor or driver board but I've found the spindle to be nearly useless at low rpm (I also can't discount the fact that I'm a terrible machinist as this machine is the extent of my machining experience). It is so easy to stall that I've become paranoid to make any cuts without an elevated rpm and super slow feedrate. As a result I try to keep the rpm high and the feeds slow enough to make the cut without the incessant spindle halts (which require a full system shutdown and restart to clear and are a major major pain in the ass). I knew that this didn't seem right as I would generally have to take the most conservative feed rate from Gwizard and roughly cut the feedrate in half to keep the spindle going. I think Mikini knows this and recommends smaller diameter cutters that can be run at higher rpm. I've heard Phil say a few times that a 3/8 diameter tool is the largest that should be used for maximum efficiency or something to that effect and I think that's why. I'm using a .5 2.5" endmill because that is the smallest diameter that I could get that was also the appropriate length. The boring was just a test on a scrap piece as the rpm generated by Gwizard seemed pretty fast so I went with numbers I got from a youtube video that seemed to give good results. I know it pushed the piece down and I realized that after it happened and remounted it but having a rigid piece didn't change anything. For reference what speeds and feeds would you cut 4140 HT at using a .5 2.5" TiAlN carbide endmill or a .5 1.75" TiAlN carbide rougher? Oh and I'm using the long endmill from the beginning instead of stepping up the length as the depth is increased because of the machine time. At that rate is takes approx an hour or so per part (hopefully I can cut that time down with the drilling) and there will be somewhere between 8 and 24 parts in a fixture jig and I don't want to be swapping tools out so often. For lack of a an ATC I would like the programs to run as long as they can on each individual tool. Could my issues be the spindle itself for what ever reason just not getting out enough juice to do the cuts? It still will not reach max rpm, maxing out at around 3300. Maybe the power is also being limited as well.

I'm no expert either, but I think you would be better off reducing your WOC and keeping the feedrate at what GWizard gives. If you have truly halved your feedrate, you can go to half the WOC and get done in the same amount of time.

I do think you will be much better off going to shorter tools when you can, as suggested... Even if you need to change tools after 45 minutes, that original tool will last longer and be MUCH more rigid, yielding a smoother cut.

And no, you are not alone getting frustrated with stalling the spindle. It is VERY frustrating, and I have priced out an AC Vector drive replacement option. I just need to dig in to how the Mikini drives the BLDC. If it is just a PWM signal we may have an easy swap to do to get a MUCH more capable spindle for under $2k.

Thanks Mike,

I'm definitely interested in hearing more about this VFD spindle.