novakon vist, collet chucks and other fun stuff

[ihavenofish]

so i went up to novakon today to get an er 25 collet chuck for my NM-070.

the chuck is a chinese made one that looks more or less the same as the ones you see on ebay and at little machine shop. it came in a set with a full range of collets and was $140us - the same as LMS, but you get a few more collets.

part of the reason i got the chuck is because i had runout issues with the machines. as it turned out, the source of the runout was mostly the MT2 collet. the actual spindle runout on the taper was a bit under .0005" by my indicator. which isnt bad, but the crap mt2 collets were from .001" to .005" depending on the direction i put them in. ironically these were somewhat expensive US made collets.

the ER chuck in the machine with a 1/2" tool in it has an acceptable slightly sub .001" runout at 1/2" from the collet. this is fine since i wont commonly use smaller bits than 1/8" and if i do it will likely be in a secondary high speed spindle like a proxxon.

so, all in all a good deal, and a good chuck for the price. it also keeps me from whacking the drawbar with a hammer too often.

while i was there i looked at the machines. nice stuff. was the first time i saw the new revisions. the new version of the nm-070 made me a bit sad i didnt wait for it... vastly improved in every single way over mine. in fact i dont think it shares a single common part.

i also picked up a few of the really cheap HSS end mills they have. ill try them in some aluminium and post whether they are decent or not.

[ihavenofish]

tested out a few of the end mills: 1/4" 2 flute, and 1/2" 4 flute.

they seem to be generally good bit, very good for how cheap they are. the side wall finish isnt so hot on heavy cuts (not helped by my small machine), but its acceptable on finish cuts. the "bottom" finish is somewhat amazing actually. the 1/4" is like glass. you see the swirls, but you cant feel them. this is even better than the name brand hss and m42 bits ive tried. coolant also helps improve the finish substantially.

for the price - $3.50 for the 1/4" and $7 for the 1/2", id say these are great for non finish critical aluminium jobs.

ill try to make a vido over the weekend cutting somethign interesting with them.

[fourwheeler]

It doesn't have to be an interesting piece just something that shows the finish would be cool.

[ihavenofish]

Originally Posted by fourwheeler It doesn't have to be an interesting piece just something that shows the finish would be cool.

haha

it will be interesting... to me. likely a piece of a bicycle frame. trying to see which one fits in the scrap of 6061 i have here.

[ihavenofish]

this was my test cutting with the 1/2" 4 flute bit. description in the images.

i'll leave the decision of whether the 1/2" can take a nice side cut to someone with an NM-135. its not an ideal size for my machine. i actually get significantly faster material removal from the 1/4" simply because it doesnt chatter and i can push it much harder. i will mostly use the 1/2" for facing small parts i think.

stub length would serve me alot better.

[ihavenofish]

after a few false starts, ive gotton a part made. its a crown for a bicycle fork, though its slightly undersized - about 7/8" of true size.

the roughing was done with the 1/4" chinese end mill. i was taking heavy0ish cuts (for my machine) and didnt do a finish pass, so the side wall finish is not great. if the pogram had a finish pass it would have left a fairly decent finish. on a heavier mill with less vibration it would look much better.

top contouring was done with a niagara 1/4" 2 flute ball nose with TiAlN coating. was all i had for ball noses - its intended for steel.

i rant the entire operation dry with a weak air blast blowing chips away. i think coolant would have given me a better finish.

on the roughing i played with the feed rates a bit. generally it was up around 16-20 ipm though, with a 1/8" width and 1/8" depth. the ball nose ran at 20ipm with a 0.005" stepover. for the purposes of this part - which woul dhave finish work, i could do with a .001" stepover and made the whole thing alot more efficent. total time for all milling was 69 minutes, and could easily be brought down to 30 with more efficient programming.

i did some video, but being so long, im going to edit them up for the highlights. maybe tomorrow.

[Frogblender]

Originally Posted by ihavenofish this was my test cutting with the 1/2" 4 flute bit. description in the images. i'll leave the decision of whether the 1/2" can take a nice side cut to someone with an NM-135. its not an ideal size for my machine. i actually get significantly faster material removal from the 1/4" simply because it doesnt chatter and i can push it much harder. i will mostly use the 1/2" for facing small parts i think. stub length would serve me alot better.

What kind of RPMs are you cutting with?

[ihavenofish]

Originally Posted by Frogblender What kind of RPMs are you cutting with?

5000 on everything. top speed of the machine. i actually tried other speeds down to 1000rpm and the spindle torque begins to outshine the frame of the machine . on my machine, the strategy is usually high rpm, high feed, shallow cuts - either side or axial.

little crown gcode has been redone to use the 1/2" cutter at .02" depth, 100ipm, 75-100% width. it runs far far better like that, and will only take 10 minutes instead of 25 with the 1/4" for the roughing. it ends up being more efficient use of the machine and less strain - and noise.

on the nm-135 i think youd take a different approach. nearly 3 times the spindle power, and more rigidity and mass would make deeper, slower cuts more efficient.

[Frogblender]

Originally Posted by ihavenofish 5000 on everything. top speed of the machine. i actually tried other speeds down to 1000rpm and the spindle torque begins to outshine the frame of the machine . on my machine, the strategy is usually high rpm, high feed, shallow cuts - either side or axial. little crown gcode has been redone to use the 1/2" cutter at .02" depth, 100ipm, 75-100% width. it runs far far better like that, and will only take 10 minutes instead of 25 with the 1/4" for the roughing. it ends up being more efficient use of the machine and less strain - and noise. on the nm-135 i think youd take a different approach. nearly 3 times the spindle power, and more rigidity and mass would make deeper, slower cuts more efficient.

Do you have a tachometer to verify your actual spindle speed? Tachs are nearly free on ebay. I bought a model "DT-2234C+" (search "New Digital Laser Photo Tachometer Non Contact RPM Tach" on ebay); I tried various pulley configurations on my drill press, and the tach readings almost perfectly match the RPMs on the little pulley drawings tattooed to the drillpress cover. So I'd say the tach "works good".

However, my NM135 spindle seems to top out around 3500rpm But I think this may be due to a spindle problem (high runout, very noisy, gets hot (the spindle, not the motor)), which the good folks at Novakon are taking care of.

[ihavenofish]

Originally Posted by Frogblender Do you have a tachometer to verify your actual spindle speed? Tachs are nearly free on ebay. I bought a model "DT-2234C+" (search "New Digital Laser Photo Tachometer Non Contact RPM Tach" on ebay); I tried various pulley configurations on my drill press, and the tach readings almost perfectly match the RPMs on the little pulley drawings tattooed to the drillpress cover. So I'd say the tach "works good". However, my NM135 spindle seems to top out around 3500rpm But I think this may be due to a spindle problem (high runout, very noisy, gets hot (the spindle, not the motor)), which the good folks at Novakon are taking care of.

runout sounds bad. hopefully they get that fixed up quick. are you sure its spindle runout and not tool holder? i had terrible runout til i realized it was the collet. its still not spectacular, but its under .001" and thats acceptable to me. my spindle also get very warm after running for an hour. i assume thats normal to some degree. its not so hot i cant touch it.

as for rpm. if you have the latest model, should be 6k. old one was 3500. i wonder if they just used the wrong motor. you could try to look for the label on the motor, but its tucked inside the head so might not be able to see it without removing it.

[Frogblender]

Originally Posted by ihavenofish are you sure its spindle runout and not tool holder? i had terrible runout til i realized it was the collet. its still not spectacular, but its under .001" and thats acceptable to me. my spindle also get very warm after running for an hour. i assume thats normal to some degree. its not so hot i cant touch it. as for rpm. if you have the latest model, should be 6k. old one was 3500. i wonder if they just used the wrong motor. you could try to look for the label on the motor, but its tucked inside the head so might not be able to see it without removing it.

Yes, it is spindle runout - I'm measuring the runout both on the inside taper (angled the dial indicator up a little to get it in there) of the spindle and the outside (the collet is not attached) - the two measurements are the same (IIRC), and they're not good.

Based on your wrong motor comment - I removed the wire egress plate on the head to take a look at the motor - sure enough, I can see enough of the the motor label to read "3500r/min". Blarg . My NM-135 is supposed to be Rev2.1.

[ihavenofish]

so i got my order of end mills for maritool today.

all of them are TiAlN coated 4 and 6 flute end mills, some flat, some ball end, some variable etc etc.

i bought these for steel, so naturally i tried them in aluminium
not really a good idea. they work, but not ideal. the HSS bits are better suited.

in steel they reinforced what i had been thinking about how to run my machine.

1/2" 4 flute variable. runs at 60ipm, .01" depth, full or near full width. anything deeper chatters too much and a bad finish results. very light side cuts are fine as well. coolant seems to not required in this situation. 0.3cfm.

1/4" 4 flute variable. runs at 20-30ipm. .02" depth full width, or lighter side cuts. i need a proper sized collet however. the 6-7mm metric one is too large and the tool creeps out of the holder. runout is hard to control as well because of the creeping. coolant is a good idea here. make alot of noise plunging and leaves a high spot from machine deflection on helical cuts. 0.15cfm.

1/8" 4 flute variable. runs 10 ipm, .12" depth - probably can go deeper. no chatter at almost 1" extension from the holder. plunges well. coolant is ideal here. 0.16cfm.

all these bits are variable flute with small radius's on the corners so they are less prone to chatter and breakage.

so, basically, the 1/8" will be the workhorse for any small work in steel. the 1/2" will be for surfacing and roughing large pieces. i will have to seek out a stubby 1/2" 4 flute to reduce chatter more.

the 1/4" seems to be not really worth having for steel except for deep side cutting. with a proper collet though it might fair alot better. we'll have to see.


i also tried a 6 flute 1/4". its intended for light side cutting. it pulled out of the collet ablout 1mm and snapped off. well, at least it was a $12 maritool and not a $30 niagara like last time. ive had bad luck trying to use these 2 times now, i think i'll stop.