[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

[mcphill]

Can you plunge the bit in fast, and then do a "real" cut on the way back up/out? Not sure if the tool is made to cut that direction, but how else can you ever get a boring bar out without ruining the finish, or stopping the machine to move the radius in to clear the bore?

[SWATH]

I don't know how it's done but I may just have to do it manually if the Mikini doesn't support no drag boring (which I'm not even sure how to implement, like how to do tell the machine where the cutter is oriented?). It certainly ruins the finish on the way up and if you stop the spindle at the bottom and retract the boring bar, it will score a slice in the wall of the bore. Reverse boring probably won't work either as the engagement angle is probably too shallow and will cause serious chatter, that is why I think it is ruining the finish on the way out. The only solutions that I can see are A. Do it manually. B. Do no drag boring. C. Explore different insert geometry that won't chatter on the retract.

[Brian L]

Glad to see a response, was worried I might have offended with the "almost painful to watch" comment. GWizard might be great in some instances, but for someone starting out, you are best to "do the math" yourself until you have a feel for "your" machine.... i.e. what I can cut with my Milltronics is going to be worlds different than you can cut with the Mikini, so somebody else's numbers are just about worthless.

The most important things you should research are what the manufacturer suggests for feeds and speeds, almost everybody has a catalog or PDF on the website with cutting data.... this endmill can run 225 sfpm in 4140 and feed .004-.008" per tooth... those are the numbers you need to work with. As you have realized, gutless wonder is going to cause you some issues with anything low rpm.... so use the higher end of the suggested spectrum and that should help a little. You do need to keep the feed rates up though, too slow and it will just chatter and rub, which dulls the endmill much faster than hauling butt. If you have to keep your radial engagement (WOC) smaller and your depth of cut shallow.

For example, you would be better off doing say .030" to .050" width of cut and .25" DOC at the higher feeds and speeds, than to chatter along at 5 ipm and 2400 rpm. OK, 1/2 endmill, in your 4140, not knowing the ht level, I'm going to guess and say that endmill should be able to run 200 sfpm, so the rpm is 1530 rpm, and the feed rate, let's stay conservative and only go .003 per tooth, that's going to be F18.3, so start with those numbers and say .100 depth of cut and limit your width of cut to say no more than about .075" to .100", that might require a few roughing passes at the ares where you have more stock.

You should go watch/research some of the High Speed Machining paths you'll find on youtube, these are going to be very applicable methods to the Mikini as they were developed to run high metal removal rates on minimal hp and rigidity machines.

Boring, you are kind of stuck if you don't have a fine boring cycle. If you have enough relief ground into the tool tip that you have about a 30º angle, you can usually spring cut on the way out and get a reasonable result. Shy of that, stop the spindle, put in an M0, open the machine, push your finger against the bar to spring it away from the cut, and then retract the Z... make sure you have another M0, or maybe two, right after that, wouldn't want the spindle to start spinning while you have your fingers on the bar. This is what we used to do on manual machines in the "old days".

If you want to run steel on these machines, and the claimed 3hp is really a myth, then you need to investigate more motor, better drivers, or see if you can adapt a two step pulley to the spindle and motor. We had a Leadwell CNC years ago, ran 500-6000 rpm in "high" and them you could slide the motor forwards, drop the belt to "low" and you had more like 250-3000 rpm, and I know that doesn't sound like a lot, but doing that, it would cut stainless steel with it's 5hp spindle motor about twice as fast as the big Fadal we had that was 25hp.. it had a top speed of 10,000 rpm and was a gutless wonder on the bottom end.

[mcphill]

Gearing down for low speed cuts was another option I was contemplating...

[SWATH]

I'm not sure if it's supposed to be like this but the flat on the boring bar is not centered resulting in kind of a negative rake angle. I'm not sure if that's a problem because the insert kind of has a lipped edge so it still may be a positive rake but I would think the flat should be centered. What do you all think? I just want to make sure I didn't get a defective product.

(Edit): On second thought I just realized why it's that way. To keep the cutting tip in the radial center of rotation...duh.

[Brian L]

Yep, that's exactly how that particular bar is supposed to be. If it didn't have the 10º negative rake on top, it wouldn't have enough clearance to cut without rubbing the bottom edge of the insert in the bore. As it is, you probably have a listed minimum bore that this bar will do.

[SWATH]

Thanks again Brian. I'll try some of those cuts and see how it goes. No offense taken at all. I am currently enrolled in the school of hard knocks and cannot get offended when someone tells me I'm doing it wrong. Most of the tools I'm using state 340sfm .0025 IPT at 1x diameter DOC with full slot in 4140. The rougher states 400sfm.

[Brian L]

You don't have the hp to do anything even remotely like that. Just from the sounds of it, that cut would eat up every bit of a "real" 3hp, maybe even more. So the rpm and feed per tooth you can use, just modify the depth of cut and width of cut if you aren't doing a slotting cut and you can find out from there what the machine is capable of.

[mcphill]

6061T6
Carbide single point tool in fly cutting arbor
2000 rpm
5 ipm
.010" - 0.060" DOC
2.5" WOC
? hp (made up the feeds and speeds myself .1575 according to GWizard after the fact)

Almost mirror finish with lowest DOC and flood coolant.

[SWATH]

Can anyone give me any tips on v-carving? I've not done it in metal before but have a text monogramming job to do in the next few days.

I have a 120, 90, and a 60 degree 4flute TiALN carbide chamfer mill of this variety:
Regular Length Solid Carbide TIALN Coated Chamfer Mill - MariTool

The material to cut is 410 stainless steel. Unfortunately my top spindle speed is 3300rpm so that is limiting factor but I just need to carve some text to maybe .05 deep (max depth), maybe less.

I'm thinking of using the 60deg cutter. What do I need to know? Tips and advice, etc. I just don't want to ruin the part or the tool. I only have one shot at the part and it has to be perfect. I'll obviously try the cut in scrap Al or steel first but I've never cut stainless.

[mcphill]

Sorry, I don't. I have not done any V-carving. I know you want the highest spindle speed you can get since you are effectively approaching a zero diameter tool - this is why I use a ball end mil instead, at least there is some cutting at the very tip that way.

Don't bother practicing on aluminum, it would be totally different and much easier than stainless. Steel would be closer, but still a bit different.

Go SLOW! Use coolant. Did I figure right that GWizard suggest a -0.068 ipm feed!?

[Brian L]

It says on the website that those endmills are not intended for spotting, so I wouldn't attempt to engrave with one. Get a specific engraving tool, or use a small ball endmill, HSS would work given your relatively slow rpm, stub length would be best.

410 SS shouldn't do too bad, it can be a bit rough on the final machined surface, i.e. a surface doesn't look real smooth, but with flood coolant and going slow, you should be ok. Like you said, practice on a piece of mild steel, won't be that different.

[SWATH]

Thanks for the advice. I'm trying to figure out if there is a way to program the operation using a ballmill but my CAM doesn't seem to support it, you can only specify v-mills for v-carving. Since I'm pressed for time, I don't really have time to order a better tool, don't know what tool to get even if I did have time, and the job is essentially 6 .5" tall letters, I'm thinking about maybe trying the 120deg chamfer mill. I know it's not the best because of the tip point (I assume that's why) but I'm hoping the more blunt chamfer angle may be more forgiving to the tip. With that one the max DOC would be .02". I also have a center drill I could try, like this: Carbide Combined Drill And Countersinks - MariTool

I've heard some people using those for engraving, what do you think, could that be a better option given the shallow DOC?

[howecnc]

Program for whatever tool your software will allow and use the ball mill at the machine. I have done this in the past but I don't know your application. You may have to adjust your tool length to control depth and cosmetics.

[Brian L]

Centerdrill will work, don't go too deep, most engraving is on the order of .005"-.010" deep max. 120º tip isn't really the answer, your line width might bet pretty wide at even .005" deep. Why don't you pick up a ball end carbide rotary file? Get one of those at Home Depot for any dremel tool.

A friend sent me a huge 3D file to mainly test my new bigger memory on my mill and I ran this example with a carbide 1/8" ball rotary file...... granted it's mdf, but I was moving 30 ipm too.....

[SWATH]

Here is a pic of the v-carving in Al. It turned out really well although detail on the right is a tad deeper than on the right. I'm not sure why but I assume I had it somehow slightly misaligned in the vice. I started out trying the center drill but it was terrible so I went ahead and used the 90deg chamfer mill and it worked perfectly with a MUCH nicer finish. Now I just need to do it in SS.