Question on shortening cutting time

[keithmcelhinney]

I have been working with my nm135 for a couple of months now and got some good parts done. Now I am looking at doing some parts to sell and naturally want to be able to cut my time down as much as possible. I am doing mostly contours and some pocketing. I have used the 2 flute (long) and a 3 flute (short) 3/8" carbide end mills. I run at 3200rpm with the 2 flute at about 7ipms and the 3 flute at about 9ipm. My cut depth is .05. Now it runs pretty good but it takes a LONG time. I tried a 5/8 carbide end mill for clearing the pockets and proceeded to break it almost immediately. It was when I first started and I had my plunge too high I think. But it seemed like the spindle couldn't handle plunge cutting with such a big end mill. Naturally I don't want to spend $60 and try it again without making sure it is going to work. Does anyone have any suggestions how I can speed it up? Should I go a little deeper? I can't see going any more than .06 but don't want to break end mills or screw up the machine.

Also I was looking at roughing end mills. Would this be worth looking at when I am not going very deep? Would I be able to cut deeper?

What are you guys running when you are trying to remove a lot of material? I have 2 parts that I am removing 4-5 square inches and an inch deep. I do not need to have a good finish on it since I do a finish pass on everything. Any suggestions as to end mill size,depths,speeds would be awesome.

Thanks!
-Keith

[ihavenofish]

I have been working with my nm135 for a couple of months now and got some good parts done. Now I am looking at doing some parts to sell and naturally want to be able to cut my time down as much as possible. I am doing mostly contours and some pocketing. I have used the 2 flute (long) and a 3 flute (short) 3/8" carbide end mills. I run at 3200rpm with the 2 flute at about 7ipms and the 3 flute at about 9ipm. My cut depth is .05. Now it runs pretty good but it takes a LONG time. I tried a 5/8 carbide end mill for clearing the pockets and proceeded to break it almost immediately. It was when I first started and I had my plunge too high I think. But it seemed like the spindle couldn't handle plunge cutting with such a big end mill. Naturally I don't want to spend $60 and try it again without making sure it is going to work. Does anyone have any suggestions how I can speed it up? Should I go a little deeper? I can't see going any more than .06 but don't want to break end mills or screw up the machine.

Also I was looking at roughing end mills. Would this be worth looking at when I am not going very deep? Would I be able to cut deeper?

What are you guys running when you are trying to remove a lot of material? I have 2 parts that I am removing 4-5 square inches and an inch deep. I do not need to have a good finish on it since I do a finish pass on everything. Any suggestions as to end mill size,depths,speeds would be awesome.

Thanks!
-Keith

you dont mention waht you are cutting. if its aluminium, put the rpm to 6000 (if your machine version handles that), and take shallow axial cuts at a much much higher feed rate. for example, you should have no problems cutting .375" deep, .125" width, at 35 to 50 ipm with a 3 flute .375" uncoated carbide. you probably should use at least a mist coolant (spray bottle) to help keep the chips from sticking to the tools, as well at climb cutting when possible. avoid doing cuts more than 75% of the cutter width.

on plunging... dont. any vibration from plunging seems to damage caribe end mills and most of these small bench mills have plenty of give in the head to cause this. its best to ramp or helix into a cut (on any machine really) at about 30-50% of your normal feed rate. you can also get a tool with a small radius on the tops, which will reduce chatter and the likelyhood of breaking the bit. if helixing isnt an option due to cam abilities, you could drill a pilot with a larger bit than your end mill and start from there.

[keithmcelhinney]

Thanks for the quick reply!

I am cutting 6061 aluminum and I use flood cooling. I am waiting for my 6000rpm spindle and right now have the 3500. I am a totally newbie at this stuff and really am just learning as I go. I am (naturally) a little confused as to proceed. I need to cut pieces out of plate so how would I cut at only .125 width? It will have to cut at full width. Here are some pics of what I am cutting:





Most of it is out of 1/2, but there is one part on the back of the forward controls that is 1.75" on one side and 2.125" on the other that I have to contour all the way through with some pocketing.

Please let me apologize for the newbie questions. I really want to learn how to do this properly.

-Keith

[fourwheeler]

Thanks for the quick reply!

I am cutting 6061 aluminum and I use flood cooling.

-Keith

Any pics of your enclosure? I am wondering how you are containing the flood coolant.

[ihavenofish]

Thanks for the quick reply!

I am cutting 6061 aluminum and I use flood cooling. I am waiting for my 6000rpm spindle and right now have the 3500. I am a totally newbie at this stuff and really am just learning as I go. I am (naturally) a little confused as to proceed. I need to cut pieces out of plate so how would I cut at only .125 width? It will have to cut at full width. Here are some pics of what I am cutting:





Most of it is out of 1/2, but there is one part on the back of the forward controls that is 1.75" on one side and 2.125" on the other that I have to contour all the way through with some pocketing.

Please let me apologize for the newbie questions. I really want to learn how to do this properly.

-Keith

ahhhh. so its not pocketing but a cutout. i think i might just say use a smaller bit. 1/4" 3 flute, preferably with a radiused edge if you can find one. ive always had better luck slotting with smaller bits. you could probably get away with .125" depth per pass, full width, at about 10-15 ipm. then take a finish pass of about .01" width, full depth all the way around. at your current spindle speed, carbide is a complete waste of money, and id probably find a nice sharp m42/cobalt bit. the 1/4" one i use is in the $8 range. you shouldnt have an issue getting through 1/2" to 3/4" plate with a 1/4" bit. any deeper though and youd need to go back up to 3/8" likely. these cobalt bits are alot more durable than carbide in terms of breaking tips.

[keithmcelhinney]

Sorry I wasn't too clear. I do do pocketing when I am cleaning material out on the 1.75 and 2.125 deep pieces. And it is a bunch of material. That is one of the slowest parts of the cut. I also do some pocketing on the forward controls on my new design, but it is only .1" deep. Here is one of the pieces. I pocket the area above the extension:



I will try the 1/4 bit for profiling. It would be awesome to be able to run at that speed. Even more awesome if the bits are only $8!

I have the little enclosure for the table right now and am planning on doing a full enclosure asap. It makes a big mess right now!

-Keith

[keithmcelhinney]

Where do you guys get your end mill?

Thanks again!
-K

[ihavenofish]

Sorry I wasn't too clear. I do do pocketing when I am cleaning material out on the 1.75 and 2.125 deep pieces. And it is a bunch of material. That is one of the slowest parts of the cut. I also do some pocketing on the forward controls on my new design, but it is only .1" deep. Here is one of the pieces. I pocket the area above the extension:



I will try the 1/4 bit for profiling. It would be awesome to be able to run at that speed. Even more awesome if the bits are only $8!

I have the little enclosure for the table right now and am planning on doing a full enclosure asap. It makes a big mess right now!

-Keith

the part you show here would work well with the first strategy i suggested. as for end mills, i get my HSS/m42 bits at a shop a few blocks from me in toronto. for cutting steel, ive had good luck with maritool carbide so far.

[Frogblender]

i get my HSS/m42 bits at a shop a few blocks from me in toronto

Where?

Check this out: See How to wire up misting/flood pump?? for details

[ihavenofish]

Where?

atlas machinery on queen. cheap, open saturdays, walking distance. no real selection or stock, but they happen to have these really nice sowa brand 3 flute 1/4" end mills for $9. they also carry some monster cutter 2 flutes for $12, but as i mentioned in aluminium, carbide seems to be worse at these low spindle speeds.

i also got some of the chinese HSS end mills from novakon. i made a thread ab out the results. quite ok for the price, but dont leave a great sidewall finish.

[zaebis]

cutting alum at .05 @7IPM is way too conservative. With my NM135 I dig at least 0.15 with any size endmill and well over 20IPM+ even for full slot passes. Two flute 35 helix uncoated carbide.

For profiling cuts just like those in your pics I use 1/8 since you would always have it full contact so to speak why cut more than needed. You would be wise to make a final pass full depth but alternatively (judging by your pic) polish the part afterwards for looks.

The problem you are experiencing (and I am just guessing here) is that when you do profiling in a few passes (e.g. taking away .05 one pass at a time until you cut through) is that many CAM software will use the same plunging speed as cutting speed for profile operations and that will not play out good for smaller carbide tools. Look at the Gcode file by hand, find all references to Z plunging and make sure they all have F2 after them (plunging Z level at 2IPM) and the next line must return cutting speed back to F25 for example.

With 2 flutes HSS 1/8 diam at 0.1" deep I can do 40 IPM in 6061 no problem. You would need 5500-6000 rpm though. Also coolant to lubricate or else then endmill will clog in seconds.

[Frogblender]

With 2 flutes HSS 1/8 diam at 0.1" deep I can do 40 IPM in 6061 no problem. You would need 5500-6000 rpm though. Also coolant to lubricate or else then endmill will clog in seconds.

6000rpm @ 40ipm with a 1/8" 2-flute equals more than .003" per tooth. Which seems to be alot for a 1/8" bit. For example, NiagaraCutter, OSG, and Micro100 all recommend between .0005 and .001 ipt for their 1/8" bits.

RobbJack is the only vendor I could find that specs .003ipt for their 1/8" aluminum bits, and that is for the rougher.

I'm having perpetual trouble running much about 20ipm on 1/8" bits (yes, I'm flooding properly). In my case the bit snaps after minutes or 10's of minutes of use, usually high up on the shank/neck/flutes where the bending moment in the greatest. I am now tending towards bits as short as possible, to reduce the bending.

What brand of bits do you use?