Problem- Carbide tool life in wood routing

[aarongough]

Hey all!
I'm having some issues with tear-out when machining birch ply, I tried using a new endmill and noticed that the tear-out totally disappeared and that tolerances all of a sudden improved greatly.

After about an hour of machining though the tear-out reappeared. The tolerances still seem to be ok, under-cutting is not an issue at the moment...

How long do carbide tools usually last in wood? I'm using solid carbide two flute upcut end-mills running at about 20k RPM and 80 IPM through birch. I'm using both 1/8" and 1/4" endmills. Should I be able to use them for hours? Days? Weeks? Months??

I know that no-one is going to be able to give me an exact answer, but I'm curious about what the ball-park should be.

Thanks!

[CarveOne]

If it doesn't have the proper edge geometry for wood it probably won't last as long as it would with the proper geometry. Precision ground solid carbide cutters should last longer than HSS cutters. Some woods can have a significant amount of silica in it that will dull any cutter fairly quickly.

There are too many variables to give a reliable answer. When it gets dull have it sharpened or get another one. When you do the same work with the same cutter type and vendor you will gradually get a feel as to how long they last in your particular situation.

CarveOne

[ger21]

Plywood can be quite abrasive and dull tools much faster.
If you want to eliminate tearout, you'll need to use a downcut spiral bit. Only brand new bits will cut plywood without tearout. How long they'll last is very difficult to say, but almost any bit will dull enough to cause tearout in ply very quickly. This doesn't mean it's too dull for cutting, it's just not the proper tool for clean edges on plywood.

At 80ipm, your rpm is about double what it should be. Cutting it to 10,000 rpm will almost certainly give you longer tool life. Heat is a major cause of dulling tools, and too slow feedrates and or too high rpms is a major source of heat.

With 1/4" bits cutting MDF and baltic birch plywood, I'm usually cutting between 125-150ipm, and 10,000-12,000 rpm.

At 20,000 rpm, you should be cutting at 400-500 ipm.

[aarongough]

Thanks guys, sounds like I need to play with my speeds and feeds a bit.

I have a further question: I haven't been able to find any decent information on what compression spiral bits are supposed to achieve, they seem to downcut and upcut? Is this type of bit something I should be looking at to reduce tearout?

Thanks!

[aarggh]

If your using decent carbide cutters you should not be seeing any appreciable cut quality difference after only an hour.

As an example, I bought several packs of 1/8th, and 6mm carbide 2 flute cutters. Although I expected them to not last long as they were very cheap, I'm still on the same 1/8th bit after around 4 months of work, and i'm still using the same 2 flute 6mm cutter after around 2 months off and on use. Workload isn't huge but it's been enough to cut several meduim sized 3D plaques, and numerous small sheets of hardwood, MDF, aluminium, and plexi-glass.

Are you running the feed too slow, or the cut too deep causing the bits to overheat and ruin the edge? What colour are the flutes after machining?

Are they just cheapo crap cutters, or you know for sure they are good?

Are you cleaning the waste as you go? This is important, especially so for MDF.

I have spent the last 3 decades doing a fair amount of hand routing for small reno's and jobs, and used to spend a small fortune on good quality router bits, but started buying the better (some are rubbish) of the cheap Asian ones for next to nothing, and I've invariably found they give no perceptable quality difference in most cases, and last just as long, or certainly almost as long, as the expensive ones. And at around 1/5th to 1/10th the cost, makes it a no brainer. Similarly, I have found almost the identical situation with the cnc cutters.

The only cutters I have blunted or ruined so far have been from overheating.

cheers,
Ian

[michaelthomas]

I would agree that your rpm's are much too high. I use .008 to .010 inch per tooth on 1/4" bits, and around .015 inch per tooth on 3/8 to 1/2 cutters in wood, mdf, and ply.

Try to never plunge straight into your material, too. I use a 30 degree ramp in on cut. Much less heat will build up if you are always moving forward.

Try to plan your rpm's according to how large the work is. If you are cutting large pieces with plenty of room between direction changes, you can run more rpm (and more feed to keep chip load the same). If you are doing small pockets or little pieces you will need to lower the rpms to compensate for the machine not being able to maintain a very high feedrate (despite what is programmed). I hope that makes sense. Whatever feed rate you choose.....maintain your chipload by adjusting rpm.

RPM x Chipload x Number of Flutes) = Feedrate in IPM

[aarongough]

Originally Posted by michaelthomas I would agree that your rpm's are much too high. I use .008 to .010 inch per tooth on 1/4" bits, and around .015 inch per tooth on 3/8 to 1/2 cutters in wood, mdf, and ply. Try to never plunge straight into your material, too. I use a 30 degree ramp in on cut. Much less heat will build up if you are always moving forward. Try to plan your rpm's according to how large the work is. If you are cutting large pieces with plenty of room between direction changes, you can run more rpm (and more feed to keep chip load the same). If you are doing small pockets or little pieces you will need to lower the rpms to compensate for the machine not being able to maintain a very high feedrate (despite what is programmed). I hope that makes sense. Whatever feed rate you choose.....maintain your chipload by adjusting rpm. RPM x Chipload x Number of Flutes) = Feedrate in IPM

Thanks, I'll try some test cuts tomorrow at lower spindle speed and see what the outcome is.

Main reason I ramped up the RPM was because my machine isn't terribly rigid, and with a higher chip load I saw chatter at a much shallower depth oof cut... But I shall re-run my speeds and feeds testing and see what the outcome is...

[aarongough]

Originally Posted by aarggh If your using decent carbide cutters you should not be seeing any appreciable cut quality difference after only an hour. As an example, I bought several packs of 1/8th, and 6mm carbide 2 flute cutters. Although I expected them to not last long as they were very cheap, I'm still on the same 1/8th bit after around 4 months of work, and i'm still using the same 2 flute 6mm cutter after around 2 months off and on use. Workload isn't huge but it's been enough to cut several meduim sized 3D plaques, and numerous small sheets of hardwood, MDF, aluminium, and plexi-glass. Are you running the feed too slow, or the cut too deep causing the bits to overheat and ruin the edge? What colour are the flutes after machining? Are they just cheapo crap cutters, or you know for sure they are good? Are you cleaning the waste as you go? This is important, especially so for MDF. I have spent the last 3 decades doing a fair amount of hand routing for small reno's and jobs, and used to spend a small fortune on good quality router bits, but started buying the better (some are rubbish) of the cheap Asian ones for next to nothing, and I've invariably found they give no perceptable quality difference in most cases, and last just as long, or certainly almost as long, as the expensive ones. And at around 1/5th to 1/10th the cost, makes it a no brainer. Similarly, I have found almost the identical situation with the cnc cutters. The only cutters I have blunted or ruined so far have been from overheating. cheers, Ian

There's no change in color in the cutters after a run... I'm sure that I'm not running the optimal speed and feed as I'm still relatively new to all this... The actual finish on the side of the cut is totally fine even with my 'old' (6 month old) 1/8" bit... Just the top ply of the birch plywood is messed up be tear-outs.

The cutters I'm using are made by YG, not sure how good they are. Less expensive than some other stuff I have seen online like Amana Tools, but I'm not sure if that translates to 'not good'...

[michaelthomas]

Some plywoods have a pretty poor veneer to substrate bond, and there is very little that can be done to get a quality finish on the veneers across the grain.

A downcut will help on top, upcut will help the bottom, or a compression for both sides at once. You need to take a pass deep enough with the compressions to bury the upcut portion of the bit in the material, though.

[ger21]

If your using decent carbide cutters you should not be seeing any appreciable cut quality difference after only an hour.

Not in actual cut quality, but when cutting plywood, you will definitely see the veneer chipping more on cross grain cuts.

Main reason I ramped up the RPM was because my machine isn't terribly rigid, and with a higher chip load I saw chatter at a much shallower depth oof cut... But I shall re-run my speeds and feeds testing and see what the outcome is...

What is your depth of cut? If you're making very shallow passes, you can sometimes get away with a higher rpm.