So how am I doing with this bit?

[harryball]

In the interest of getting more life from my expensive roughing bits if you have some feedback please let me know.

I'm cutting 1.25" cedar with a 3/8" 2 flute roughing bit that has a small pitch, probably 15 to 20. I'm cutting at 4.5 ips and 10k RPM in 3 passes with the last pass being about 0.20". this is done to keep the cutting speed as fast as possible and the board as well held down as possible while cutting. The last pass offers less resistance being such a small cut I can maintain speed without the risk of moving parts even when I hit knots.

I was using a 3 flute rougher and it didn't last long with the heat being generated with such small chiploads. Thus I'm trying 2 flutes. The current chipload is .013 to .014.

I used my infrared thermometer to get the following readings in Fahrenheit.

While cutting,
Max bit temp 102
Most common bit temp 90 to 95

As soon as cutting finished the bit was 86 degrees and down to shop temp (81 degrees) in about 30 seconds.

I measured temps in the kerfs while cutting and I was seeing 110 degrees if I checked the chips immediately behind the bit. The highest temp recorded anywhere at any time was 112 and that was the wood, not the bit.

So the crux of this question is... how hot does the carbide have to get to cause problems? So long as I'm 100 or less am I good? Should I worry about 110 degree chips?

Excuse me if I seem paranoid... but these bits are not cheap. If I need to speed up I can probably get to 5 ips with no trouble. I could also slow down the RPM.

Thanks,
Robert

[carlcnc]

Robert
you should give "AL Roughers " a try.
Enco has them on sale often, they are cobalt though, and a fairly coarse pitch.
On sale they are less than 20$ and last as long as carbide[for me] cutting alder,plywood etc.

Carl

[Brady Watson]

Robert,
Buy coated bits/end mills. I've been preaching for a long time to buy end mills over 2-flute upcut spirals since they are A) cheaper B) ALWAYS the correct diameter and C) the exact same grind as an UCS, but you can get just about any coating you want on it...and they've ALL got them in stock.

For what you are doing, I would use a 2-flute coated end mill. Turn the RPM up to 13,000 so that you have some 'buffer RPM' (using a router right?) and crank that move speed up. You might want to experiement with climb milling to reduce blow-out. You'll quickly see how different the chips are compared to conventional. Climb chips are long and cylindrical & conventional tend to be more like shavings.

The most important thing is that you are getting hot chips...since they carry the heat away. The numbers you are getting are a bit on the cool side. How is the edge quality? There is little data available on what the max operating temperature is of a bare tungsten carbide end mill, but the TiN & TiCN coatings are good to 800 and 1400° F respectively before they begin to oxidize. I've been buying nothing but coated bits when I can get them. The difference in longevity and increased cutting speed is well worth the extra $1-3 for the coating. I can attest to the performance of real diamond tooling (not Diamond Like Coating aka DLC), and how it lasts about 15-20X longer than standard carbide when cutting very abrasive materials like carbon fiber...they cost about 15X more than a standard, but they polish the edges of the part as it cuts.

On a side note...you are cutting cedar, which in my experience is one of the easiest woods on tooling around. I'm not sure why you are getting poor life out of it, but steer clear of 3 & 4 flute tools for woods. They prevent good chip extraction and rub the part 1/3 more times than a 2-flute...generating heat, dulling the edge or 'mulching' the chips that the 3-fluter couldn't eject due to it's tight helix design. The chipbreaker, like the ones you are running are nice tools...not sure why you are not getting the life out of them. See if you can get them coated for a few bucks more...it's worth it!

-B

[jeff_guinn]

Cedar is soft, but exhibits a very high acid content. The acid will attack the carbide binders & weaken the tool. Possibly a coated bit would shield effectively against the acid. McMaster Carr catalog has a good explanation on many different coatings shown in the end mill catagory.

[harryball]

I'll definately take a look at coated end mills. For now I need to wear out what I have.

I'm running a 4HP HSD and 10k RPM hasn't been a problem. My concern with move speed is when I encounter knots, some of these boards have very hard knotty sections in them. I'm afraid to hit one of these hard knots at 6 ips. Or should I even worry about it? How do you compensate for hard knotty sections in otherwise soft lumber?

I tried climb cut first and the finish on the part is very rough but the waste was nice and smooth. I changed to conventional and now the parts come off clean and the waste is rough. Is that not the correct method for determining which is best? I try to run climb on natural wood, conv. on man made materials and then change direction if the finish is better on the waste than the keep.

I am getting hot chips, so that is good. The bit temps were measured just as the bit exited the wood since I can't get in the kerf and measure it while cutting. It sounds like my temps are good in this case. This bit was new, edge quality is good. It cuts the cedar like butter.

This is not a chronic problem, this is my first encounter with heat build up and the 3 flute was my first use of a chip breaker. I don't want my new bits to dull as quickly as the 3 flute did so I'm searching for wisdom :-)

Robert

[richards]

Robert,
I've never used chip breakers before, so my methods may not apply. However, when I'm running at modest speeds, I tend to use a 1-flute cutter whenever possible. The 1-flute cutters tend to evacuate the chips better than my 2-flute cutters. With the proper feed speeds and spindle speeds, edge finish is excellent.

[harryball]

I've not seen a single flute rougher. These 2 flute versions seem to eject chips well, much better than the 3 flute did.

The best thing I did was changing to 3 passes from 2 passes. The final pass is only 0.20" but it means while all the hard aggressive cutting is going on all the parts are still a single board. I'm considering going for broke and trying a 6 ips run with the new configuration and see what happens.

From the information I've been seeing I should be trying for a chipload of 0.017 to 0.019 on low helix roughers... that means to get my chipload "right" at 10k RPM I should be moving at 5.5 to 6 ips. At 18k RPM I'd be at 10 ips! I doubt the alpha has the power to do that.

If I bump up to 12k RPM and 6 ips that's a 0.015 chipload. I don't know what it is... but I admit I constantly try to increase the RPM's... something in my mind won't let me accept that cutting wood at 10k RPM is OK. You should always cut at 18K RPM, because faster is better. That's what I keep thinking, even though I know it's wrong.

Robert

[jhicks]

Robert, sounds like you have accumulated a lot of good data and process is being dialed in. I would also confirm Mikes recommendation about single flute bits. We have used the ONSRUD "super O flutes" extensively and they really do hog some material and leave a pretty nice edge finish. They too are a bit pricey but seem to work on just about anything from plastic to hardwoods and even foam when dialed in.
Check Onsrud web site or call their tech support line. very helpful folks there.

[harryball]

I bring things like this to the board in the hope of learning and others learning during the process. I can confirm the first and hope others find threads like this useful.

I settled on cutting climb for the first 2 passes and conventional for the last .20" pass. I'm running at 12k RPM and 6 ips comfortably using a 2 flute rougher with about a 15 degree helix. I'm satisfied with the results but can not speak to bit longevity just yet. The measured temps look good and since going to 6 ips I've not seen a bit temp over 90 degrees at the parked position.

When I encounter a board with a large burl (collection of knots) I sacrafice it for the greater good and make something else with it. Out of 40 boards there are 3 boards I consider not machineable so not such a big deal. Those boards I can use to make single chamber house sides so in the end there is no real loss.

I happily discovered by using the new 3 pass approach that the board actually seals to the vac hold down better once the first 2 passes are made. The board becomes flexible and allows any irregularity to flex out and seal better to the gasket. This is a "happy" moment because I opted to use only the planer with a sled on the first side to plane the boards. This is faster than the bot and gets good enough results eliminating warpage or twists.

I appreciate the valuable feedback from everyone, it has been most helpful. Solving this will make things go much smoother. I have a few tweaks to complete on cut order and this file will be good to go. I'll be sure to let you guys know how the bit holds up and will look for coated bits in the future.

Robert

[harryball]

Things were going so well today too... all of the sudden there was a "snap" and it got quiet :-( the bit broke. I'll have to say I believe it was the geometry of the bit, it broke right were the flutes begin tapering up to the shank, not a lot of carbide and a natural stress point... but the cutting edge is still sharp. The board was clear and I checked for foreign objects and found none.

I believe I'm as dialed in as it is going to get, sounds good, cuts good, chips look good, temp is good, hold down is solid but the bit just didn't take the pressure. I loaded the next bit and it ran well too. I was able to finish my desired workload today but I'm not confident that the bit (my last bit) is going to last.

Robert