Share and compare your Mikini 1610L cutting data here

[mcphill]

Guess I need to get some good drills...

[SWATH]

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.

[SWATH]

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.

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

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

[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.

[mcphill]

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!

[SWATH]

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.

[mcphill]

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.

[SWATH]

Thanks Mike,

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

[mcphill]

I think I may have found a MUCH easier upgrade option... Could keep our motor, but change the drive to a Vector Drive unit...

http://www.parkermotion.com/new_ulm/.../driveblok.ZIP

[SWATH]

Interesting. If you used the same motor would the specs/performance be different or better with that driver? Assuming of course the Mikini driver worked properly. I'm starting to wonder if this spindle is better suited for machining Al rather than steel. Steel requires a lower rpm but your HP is also diminished to nearly nothing as you go slower. I find myself trying to maximize rpm and minimize feed rate on this BLDC system. In fact I have learned that larger diameter (>.625 or so) HSS drills cannot be used. They require too low of an rpm. I tried a 19mm HSS drill at S350 and f.25 which rubbed like hell then still stalled the spindle. A 14mm HSS drill ran pretty good at S485 f1 as long as you peck and retract since the load is nearly 100% on the down cut and frequently relieving the load seems to help keep it running. At these drilling speeds you are dealing with less than .1 available HP. Carbide is probably the way to go on larger drills since you can run them faster, but damn they are expensive. Can the power characteristics be changed with the driver to have the motor deliver more power towards the lower rpm range?

Here is how I understand the Mikini motor system:

[mcphill]

I don't know the answer to your question, but I am working on it. Some of the drivers I have seen will apply as much as 250% power for a few seconds - I think this would overcome the stalling issues we are having.

I also question that acutal performance of the spindle board. One of the VERY nice things on some of these drivers is that they need NO feedback (hall sensors ) from the motor. They use the magnetic feedback from the actual power lines to determine "rough" speed and position and they systems are relatively self-tuning.

I won't have any results this year, but hope to have a potential improved system running Q1 next year. If I need to go to an AC motor and drive I will...

[SWATH]

I tried boring with the new carbide boring bar. I ordered a 4.5" long bar but they sent a longer, I think probably 7". I decided to try it anyway and get a shorter one later if I need it or just cut the carbide bar down. The inserts I'm using are Ceratip 32.50 CBN and I'm trying the .016r and the .008r. So far it cuts much better than the C6 carbide but I've dialed in a few things better. To get a decent ribbon I ran at S300 F2 and a .01 DOC with the .016r insert. This ends up being .067ipr. Going down to .005 DOC caused chatter. I took the DOC as high as .1 and it got out of hand as the spindle slowed and began to cause chatter. I will likely try to do a DOC of .02-.03 to help stabilize the the cut with this radius and perhaps slow the feed down to about .004-.006ipr but ramp up the SFM to about 125. I will try a DOC of .015-.02 with the .008r insert

So to recap:

S300 (59sfm)
F2 (.0067ipr)
.016r CBN insert CCMT GK chipbreaker
DOC .01

cut pretty good but you can not retract while the the spindle in still turning or you will ruin the finish.

I'm going to try

s640 (125sfm)
f2.5 (.004ipr)
.016r CBN insert CCMT GK chipbreaker
DOC .021

and

s640 (125sfm)
f2.5 (.004ipr)
.008r CBN insert
DOC .013