More broken bit woes... help!

[jeffreymcgrew]

Hey all. Geeze have we had a lot of problems lately. So now we're started consistently breaking bits. The bits only seem to last a sheet or two before breaking.

I'm cutting with the Porter-Cable router, and I've tried several different speeds:

4ips @ 13,000 rpm
4ips @ 17,000 rpm
5ips @ 13,000 rpm
5ips @ 17,000 rpm
6ips @ 13,000 rpm
6.5ips @ 13,000 rpm

Several of these are right in the 0.10 to 0.15 chip load area when I run the chip load calculator. The bits are breaking because they are getting too hot I think. The collet and bottom of the router aren't hot, but the bits are screaming hot just post breakage. It's a brand new collet too, and we're tightening it down plenty. We're using 1/4" compression and 1/4" straight flute cutters from Amana tool, solid carbide. Lots of complex curvy inside and outside cuts. We're always taking a 1/4" deep pass at a time, no deeper. We're cutting 3/4" solid-core maple 13-ply plywood ("Appleply") and 3/4" cheap paint-grade 13-ply birch plywood.

We're now at least two days behind where we need to be, and if I can't get this working soon our little business may be sunk. :-( As it is right now we're stuck, for I can't get new bits on sunday and I was supposed to get at least two more sheets cut today. So any and all help I can get, feeds, speeds, ideas of what we're doing wrong, and how we can solve this problem would be really appreciated.

[fleinbach]

I had problems with several manufacturers bits breaking when I started 3 years ago. Then I tried Whiteside. I have not broken a single bit since I switched to Whiteside. I do most cutting with a 1/4 up spiral. I have cut 1" MDF at 10 ips single pass. I have cut solid oak at 6ips .25 deep per pass. I have cut yellow pine stringers at 6ips .35 deep per pass. I have made test cuts in all these materials at varying speeds and have never broken a bit.

[jeffreymcgrew]

huh. so you think it's as simple as that? That Amana tool's bits aren't really up to snuff for this heavy cutting?

We cut a lot of stuff in the past at 4 ips & 13,000 rpm without so much breakage. But that was with the 'old' brain, not the new 4G controller. We'd like to run faster with the 4G now, if we can, but it seems that even if we run close to the speeds we were (5ips @ 13,000-16,000) that we're breaking bits...

Anyone out there using the Amana bits without issues?

[fleinbach]

To tell you the truth though several of my suppliers carry Amana bits I have never used one. I suppose the reason is every time I think about using them I change my mind when they give me the price. I pay $18.00 for a Whiteside 1/4 2 flute upspiral. But even if the Whiteside cost more I would still purchase it due to it's increadable reliability.

[richards]

Do you really need that fine of a chipload? I run plywood at a minimum of 0.015. Usually I run at 0.020. The larger chips seem to carry away the heat better.

At 4-ips / (13000 RPM * 2- flutes) you're getting a chipload of 0.00015, which is about 10X smaller than the chipload that I like. Even a single flute cutter gives a chipload of 0.003 at that feed rate and RPM.

Before I bought a spindle, I almost always used single flute cutters because my Porter-Cable just didn't have enough 'umph" to cut properly at the slow speeds required for optimum chip load.

[richards]

There is a big error in my formula. I gave the feedrate in inches-per-second, when the formula expects the feedrate to be in inches-per-minute. (Sorry, but I only got 2-hrs sleep last night before being called out to fix a computer-network problem. My old mind coupled with lack of sleep is not a good combination. Add to that the fact that I just used a calculator because the Linux machines which I had available this morning won't run the excellent chip-load calculator that is part of SB3 and you'll realize that old men shouldn't be allowed to use calculators without adult supervision.)

The correct formula is chipload = (ips * 60) / (RPM * flutes). So (4 ips * 60) / (13,000 RPM * 2-flutes) = 0.0092, which is about 1/2 what I would like to see.

[harryball]

"Lots of complex curvy inside and outside cuts"

This gives ample time for heat build up since you are running no where near your advertised ips in those types of cuts. You are probably seeing 2 ips or less in the curves causing your chipload calculations to be ineffective. You may need to change to a single flute cutter to bring your speeds into line.

Robert

[patricktoomey]

I use the Amana tools 1/4" 2 flute compression cutters to cut 3/4 Chinese birch. It's some tough stuff with unpredictable densities and the odd piece of metal between the plys. I generally cut in 2 passes around 4ips at 10,000 RPM. The bits are warm but not hot and I get 40-50 sheets of cabinet parts from a bit. If the bit is getting really hot I would try speeding up the feedrate or dropping the RPM's. I run a spindle so RPM is easier for me to control. The bearings went out last week and I'm waiting for replacements and I'm using a PC router in the interim. I definitely am not as comfortable with the router and I'm having a hard time keeping the RPM's up but using the same Amana cutters I just slowed my feedrate to 3ips and have not had any really hot or broken bits. There must be something else going on over there, are you sure your router doesn't have a bent shaft or some kind of really bad runout causing the bits to wobble in the material and overheat?

[jeffreymcgrew]

Mike: This chip load thing is gonna kill me. It seems that no matter what values I plug into it, it's telling me to run the bits at 6-8 ips if I'm running at 13,000 rpm to get into the 0.015-0.020 chip range with a two-flute bit. But if I do run those numbers, the bit break, and I think it's because of the ramping and the dense maple ply I'm cutting. I'll try to order some single flute cutters so that I can get the numbers down some, but I need to get back to cutting today and there isn't anywhere local that I know of to get single flute bits...

Robert: Yeah, that's what I was thinking too. The curves never let the bit get above it's ramp speed, so I'll just need to slow the whole thing down. I'll try to find some single flute cutters locally and see if I can get that to work.

Patrick: I'm going to slow down to 3ips, and see if the bits live long enough to at least get this job out the door. I'm not sure that the router doesn't have a problem (if I was I wouldn't be in such trouble) so how does one check? I doubt it's a bent shaft, we've been cutting with this router for a year without trouble. It could be the runout. How do I checK?

Thanks a ton everyone...

[Brady Watson]

Jeff,
I wouldn't get too hung up on chipload numbers. The important thing is that A) you are not breaking bits B) you are not burning the material and C) You are getting a nice edge.

The simple 'grassroots' approach that I always took was if you are breaking bits, you need to either slow down the move speed or speed up the router (effectively reducing chipload and cutting force). If you are burning, slow down RPM or increase move speed. In some cases you have to reduce stepdown distance to reduce the amount of force being put on the tool and speed up the move speed to prevent burning. The grassroots formula doesn't apply when you are breaking bits due to overheating (like running @ 24,000 RPM and 1 IPS in a material that just doesn't burn)

I haven't found a 1/4" straight bit that I could keep from breaking under normal cutting. To get around this, I do an 1/8" deep pass with a downcut spiral, and then finish the rest of the cutting with an upcut spiral (end mill) to get a nice edge on both sides...this is what I call a poor man's compression bit. Sinch PW doesn't do ramped entries, I found this method to work well. If you have Insignia, you can do a ramped entry with a compression spiral and cut in one pass...just slow the tool down (like 3-4IPS) if you are cutting full depth, and experiment with different RPM settings WHILE the tool is cutting.

-B

[jeffreymcgrew]

Brady, as always, thanks for the advice. However I'm more confused then ever. You, and Robert, are saying to slow the Shopbot down and speed up the Router when I'm breaking bits. Chipload is saying the opposite, speed up the Shopbot and slow down the Router. In the past, when I was breaking bits before, it was because I wasn't moving fast enough. Once we set the Shopbot to a faster speed everything worked. Now it seems it might be because I'm moving too fast through much denser material, and so I'm getting too hot there. I know there is a 'middle spot' here that I need to hit, but I'm getting really frustrated for I'm just not getting it when it comes to chipload and speeds it seems.

I guess I really need a spindle for this kind of work, for Chipload is telling me to either run at RPM's the router can't do, or run at speeds the Shopbot and/or bits can't do.

However I finally got something that seems to be working. Found a local single-flute bit, and setting it at 4ips @ 17,000 rpm it seems to be working. At least it's not breaking. For now. I was running 3ips @ 13,000 but the router was bogging down too much.

And of course, when it rains it pours, also had a bad stall happen right in the middle of the job and lost a part. Not a huge deal, but I was really, really, really hoping that we solved that problem already... Maybe I just need to bite the bullet and swap up to an Alpha & a Spindle, because this is really killing me...

Thanks again everyone, any other advice would be very appreciated...

[Brady Watson]

Jeff,
I have given up on a good 2-flute straight 1/4" bit...They are the only bits that I have broken in several years of cutting! The reason being that the cross sectional area of the 1/4" 2-flute straight is pretty small. There really isn't much meat there, so it is prone to snapping in half if A) You overheat it B) You push it too hard thru dense material C) It doesn't like the RPM when critcal vibration for that bit sets in...

A single flute is a better choice OR use a spiral. The spirals have a much larger cross sectional area and are pretty tough.

-B

[jeffreymcgrew]

Well, we don't want to be using 2-flute straight bits. We normally use 2-flute compression spirals, and cut softer cheap birtch. This solidcore maple is much harder, and it broke our compression bits. I've got some on the way to me now in the mail, but there isn't anywhere local that I know of that stocks compression bits (and is open on the weekend too). We can get straight flute bits on the weekend, so we swapped to those. Problem is that we were breaking *any* 1/4" two-flute bit we tried. Including the spirals.

Going to a single-flute bit seems to work. I've got some one and two flute compression spirals on the way to me now, and I hope this single-flute straight bit holds for at least three or four more sheets so I can at least get this job out.

Brady, you've got a spindle yes? I'm starting to suspect that part of the problem is our complex curves and cleanup passes are generating too much heat, for the PC router can't vary the speed while cutting and it's never getting above ramping speed. So when I set the RPMs to work in that range, the job goes back to 'full speed' when cutting long straight cuts and the bit breaks from heat. So either I'll need to vary the jobs more, or slow the whole thing down so that 'full' speed isn't far from 'ramp' speed. Until we get a spindle that is.

We have Insignia. Haven't done much ramping into cuts yet. We typically are making three passes, each at 1/4", to cut 3/4" plywood. Should we instead be running our compression bits full-depth, and slower? We don't care about cut speed so much as cut quality, many of our designs involve areas that would be really hard to sand so we try to get the cleanest cuts we can...

Thanks again

[Brady Watson]

Jeff,
Yes I have a spindle, and it doesn't bog down. I still think that you can get a good cut with the setup that you have.

You are not getting the advantage of the compression bit by stepping down .25" per pass. Reason being, the 1st pass does the same as a regular 2-flute end mill...since the bottom portion of the compression bit is an upcut. Subsequent passes where the downcut portion comes into play may shave off some of the hairs left from the 1st .25" deep pass, but in my experience, it's the same as an end mill. Notice I said end mill and not upcut spiral. End mills are cheap, very tough and solid carbide...find a local tooling supply and get one. They are ALWAYS cheaper than an upcut spiral 'router bit'...

The most important factor in all of this is how the material is being held down...How are you holding down your parts? Parts/material that move, vibrate and cause bits to break...

I think that you would have very good luck using my 'poor man's compression' bit method a couple of posts up. Just break the top skin (1/8" deep) with a downcut then do the rest with an upcut or endmill. You will get a very clean edge on the top and bottom faces with zero tear out. Yes it involves a toolchange...if quality of cut is your main concern, this shouldn't matter.

-B

[jeffreymcgrew]

Brady, thanks for the advice. I'll look into getting some endmills then.

We're currently screwing things down. Gotta get a vacuum table going ASAP... I do think the movement is also playing a part in this.

[jeffreymcgrew]

so just an update. The single flute cutter at a chipload of .015 worked fine. No heat, no breaking, and I ran about eight sheets today with complex cuts. So there you go, I guess I've got to keep the cutters closer to the 0.020-0.015 range, and some of the materials we cut a lot of in the past were more forgiving when in the 0.010-0.050 range.

Thanks everyone for all the help, and thanks to Shopbot for giving me a call as well. Thanks for all the support, I really needed it today lol....

Thanks again. I wish there were more CAD/Revit/modeling questions here, for then I might be able to help out too.

[sawkerf]

Jeffrey, At what point on the bit were they breaking? Was it low on the fluted portion or high up in the solid shaft near the router collet? I've broken a bunch of those little boogers and I've determined that it was a combination of a loose Z axis V-bearing that caused vibration and a bad collet. I also believe that the bad bearing probably caused the collet to fail. Hope this helps. Kip

[patricktoomey]

Based on what Brady said about there not being as much meat on the 2 flute compression spiral I went back and looked at the Amana bit that I'm using and I think I see why I may not be having the problems you guys are talking about. I'm using the 2 flute MORTISING compression spiral which is a different animal. Only the bottom 1/8" is an up spiral, the rest is a pure down spiral with a very short transition between. This may make a huge difference. I just make sure my first pass is always more than 1/8" deep to get the down spiral portion engaged to prevent veneer tearout. I remember trying traditional compression spirals a long time ago until finding this bit. In case anyone is interested here are the details...

I get them from toolstoday.com
Amana Tool
Part #46350
Mortise Compression Spiral
1/4" Dia
1" Cutting Length
1/4" Shank
2 Flute
2 1/2" Overall Length

[jeffreymcgrew]

Kip: they are always breaking just below the collet, and are screaming hot when they break. The collet is brand new. How do I check the router bearings? When I run a single flute everything seems fine, if that's a clue.

Pat: Thanks for that tip. I was just thinking about something along those lines last night. Just to be clear, I was breaking any and all kinds of bits in this material, not just straight flutes... But a single flute at a chipload of .015 seems to hold together. I've ordered some single flute compression cutters, we'll see how those do...

[jwool]

my turn: im breaking bits, i get 8 sheets per bit, running onrud upcut spirals, @ 4ips @ 17,142.6 RPMS, which is .007 on SB chip load calculator. Im running 5hp Columbo spindle on Aplha120. The Onsrud tech guy told me these bits should run between .006 to .008 for chipload. I recently broke 2 bits after running 8 sheets of wood per bit.. i figure i should get more sheets per bit..

Im cutting 3/4 mdf all the way through on a single pass, when i called SB to ask them about this problem they told me to come to the forum b/c they are not into manufacturing @ SB... i was shocked..........

So if im runnning within the tolerance claimed from ONSRUD and the SB chipload calculator, why are my bits breaking ? I'm aware of moving parts breaking bits, yet we dont cut small pieces, im double checking my vac pump "15 hp Roots", resurfacing my table, hoping a cutup spoilboard may have caused this problem.

the bits are part# 52-910 from ONSRUD, they are $18.00 each, hopefully i can get 20 sheets per bit . any ideas?

BTW FRANK, are Whiteside bits the same bit HomeDepot carries ? or are they a different grade of bit not to be used for mass production on CNCs ?

Thanks
Jwool

[jwool]

sorry Frank bout the Homedepot reference, i was thinking about the corebox bits you mentioned to me few months earlier

where do buy the whiteside bits from ?

thanks again

[harryball]

Jwool, I've had a similar experience, but before I share it...

Chip load is somewhat of an art, the real deal is not doing the math and getting .08 but looking at the chips you're getting and how the machine is performing. At 4 ips there will likely be little performance difference between a few hundred RPMs. Dialing in exactly 17,142.6 RPM isn't that critcal... if you're in the sweet spot at 16,900 then 17,200 next time probably isn't going to seem any different.

It sounds like your bit may be getting too hot OR you could have a problem with the collet.

First the easy part, are there any marks on the shank of the bit from the collet? Some shiny marks where it looks like it's been pinching or rubbing? If so, replace the collet. Check for dust and debris in the collet and collet nut, clean them well. Make sure the groove around the inside of the collet nut is clean. I find debris can pack in there quite well.

As for heat, I've found MDF can heat bits up pretty good if I'm not moving fast enough for the RPM's I'm turning. Are you getting chips or powder in your cuts. If you are getting powder you need to increase the cut speeds or decrease the RPM's. Check your edges and corners for black burn marks. Burn marks are another sure sign speeds need to change.

I wish I could be more helpful... remember it's art as well as science. The science and math gives you a place the start and the art tunes it in where it should be.

Now for my experience, I'm running a 1/8" bit to cut one of my full sheet cuts. I run all my grooves then cut a full 3/8" plywood sheet into 12 equal panels. Early on I was running at 14k and 1.5 ips in 2 passes. This is what the math said I should be running. I didn't want to break my 1/8" bit... but it would break after only a couple of sheets. I noticed that my saw dust was packed so tight it was like wax blocks between the cuts. I could pick up what looked like wax blocks of saw dust. I didn't understand... yet.

After much reading on this board and attending a camp I started thinking. Those wax blocks form from heat melting the glue in the panel... that's why my 1/8" required so much cleaning every time I used it. I also realized the saw dust I was getting was just that... dust. So I decided to keep speeding up just to see what would happen.

I ran at 2 ips, then 2.5 ips, then 3... then 3.5. At 3.5 ips I noticed CHIPS... real bonifide chips and when I moved the parts the saw dust was not glued together. I tried 4 ips and I didn't like the way it sounded, I backed off to 3.5 ips and that same bit has ran 20 sheets so far.

I hope something helps you out. Don't be afraid to buck the math and look for something that makes sense.

Robert

[jwool]

Robert

Thank you for the info, Onsrud said with MDF it might be hard to determine "chips" b/c MDF is glued sawdust itself. I looked and my dust and its not fine dust like flour. I assume the only thing i can change during the cut process is the speed of the spindle.

Originally i had burnmarks when i first started using my SB, but since i have played with it & talked to ONSRUD the burnmarks have gone away and my parts are more precise...

Regarding the "sound" it makes, mine makes a high pitch squeal, i asked SB if this was normal, they said with a 1/4 inch bit with 3/4 inch material, it was common & their machine in their shop did the same....

As for the collet: the collet leaves a mark on the bit where the bit and collet meet, i assume this is natural clamping metal to metal ? how often should a collet last ? change them when a bit breaks? some bits have broken inside the collet, some outside the collet

Collet Nut: dust always gets in the collet, surely you dont have to clean it after every sheet, SB recommends everyday, but if i could cut 30 sheets in a day, how often should i clean ?

my bits are hot when they break ( of course) but, after i cut a sheet of mdf the bit is not hot, i'm thinking there is a possibility of the hold-down being an issue, b/c my spoilboard is really cutup due to my experimenting?

Once again, thank you for the help

[harryball]

First, 18k RPM (which is essentially what you are running) sounds fast for me on MDF unless you are running really fast cuts. I checked one of my 3/4" MDF projects and I'm running at 6 ips at 15k RPM in a single pass using that same bit.

Sound is subjective. You have to know what "right" sounds like. With MDF I do hear the squealing at times, but in cuts running at speed that tones down a good bit.

Someone correct me if I'm wrong... but there should not be marks on the bit shank. That's what I understood from the Onsrud rep. Rub marks on the shank of a bit mean uneven pressure. I'm sure there is flexibility to the rule, like being able to tell a bit has been used or not... but distinct pressure marks should not exist if the collet is making even contact.

If bits are breaking off inside a collet (and once the first bit breaks inside the collet) something is wrong. Your bit should seat all the way into the collet and should make full contact. Any breakage should occur at or below where the bit is being held. I'd venture so guess the collet is damaged if a bit broke inside.

I clean the collet and collet nut every day. If I run a significant number of sheets, 10 or more, I might check and clean it during a bit change. With MDF I'm more wary due to the high dust volume around the cutter head. The dust packed in the nut is mostly a problem when changing bits. Once a bit is in place it'll stay until you loosen it then dust will get between the collet and the nut.

I run the risk of burning myself every tme I change a bit. I'm more wary on new projects than established file. When the cutting stops I remove the bit with my hand... bits are warm, but not hot. If a bit is so hot I don't want to hold on to it I take that to mean something is not right.

Holddown can be a problem but I'm not sure how that would contribute to breaking a bit unless it rides up above the cutting flutes. By then you should know something is wrong.

Good luck working it out... I believe I'd start with a new collet.

Robert

[fleinbach]

jwool,


You can purchase Whiteside bits from HTTP://www.southernsaw.com they are located in Baltimore. I believe I paid around 17 or $18.00 for a quarter inch two flute upspiral.

I also experienced a high pitched squeal using the Onsurd bits at all speeds. This does not happen with the Whiteside at any speed. I know there are lots of people on this forum who have no problem with Onsurd bits I'm just not one of them.

[garyb]

Jwool,
Robert has given you some very sound advise above, I would have to agree that your problem appears to be a bad or worn collet based on the information you supplied.
If in a production situation the recomendation is to change your collect approx every 3-4 months.
You should clean your collet at every bit change, get yourself a 33-10 collet brush kit, you will find it very worth while.
I use both Onsrud & Whiteside, both good bits. but if I get bit screem with either then there is usually something wrong with my set up.

Problem solving of this nature may not work well through the forum, call your local Onsrud rep and have come out to your shop, he will give you an accessment of your set up and get you on the right track.

[richards]

Have you checked for run-out at the cutter? You can get a $15 dial-indicator that will be adequate to measure problems to 0.001-inch. Attach the indicator to a block of wood and then clamp it to the spoilboard. Adjust the router/spindle height so that you're measuring the cutter's shaft just above the flutes. Turn the cutter by hand slowly and watch the indicator. If things are working properly, you should not have more than 0.002-inches of runout AT THE CUTTER.

We expect a lot more from a small cutter than the physics of the design would normally allow. Being certain that the cutter is running 'true', that the material is securely fastened, that the V-rollers are riding the rails properly, that the cutter is sharp, and that we're running at the proper speed all works together.

I've found that brand name on a cutter doesn't mean too much. I commonly use Onsrud, Whiteside, Freud and a house brand from AA Carbide in Salt Lake City. The only brand that I prefer to NOT use is CMT. Their cutters work very well, but they are LOUD. Although I've never had one break, they just sound terrible.

I've also found that 3/8-inch cutters work much better than 1/4-inch cutters. I get much less deflection, less chatter, less noise, and faster cuts with 3/8-inch cutters compared to 1/4-inch. Most of the time when I have to use a 1/4-inch cutter because of the required radius or design parameters, I first use a 3/8-inch cutter to do as much of the work as possible before inserting the 1/4-inch cutter.

[jwool]

Thank you guys for the help,

Robert: On your 3/4inch MDF projects are you cutting completely through on a single pass? Im wanting to stay with single pass cuts if possible. On the speed you gave 6ips @ 15k, on the chip load calculator that gives .012 for a load which is out of the range from ONSUD .006-.008, but i know the "math" just a starting point of reference.
Collet: i was told from Onsrud that the bit must be 7/8 of the way into the collet, your saying its suppose to be 100% completely inside the collet where the bit end meets the collet end (flush) ?
Rate of change/cleaning: currently we are straight cutting squares, no Vcarving or anything that would require bit changing ( pretty much replacing a tablesaw), maybe after 8 sheets i shall clean the collet etc... From what im understanding in your post, dust is not suppose to get into your collet no matter what when cutting ,correct ? Im using the collets that came with my SB, called Techniks, are there better collets out there you guys are using that i should be using ?
I dont understand how you can prevent MDF dust from getting into a collet & collet nut, after all its 2 pieces of metal meeting, one of which has multiple slices in it by design,,,

Frank, ty for the website, i'll look into the Whiteside bits, glad to know im not the only one who hears the squeal, I wish i knew what "right" sounded like !!!

Gary, tomorrow i'm calling my Onsrud Rep to get him to take a look @ my setup & job requirements, should be interesting.

BTW, if you look @ the new videos on SB's website of them cutting 3/4 inch material in single pass, there is "the squeal " you can hear in the vid,,, mmmmmmmm

When i finally got my SB up & running i was happy, but then i run into something like this & I question my faith in the SB, im still on the learning curve & realize im still wet behind the ears, i really appreciate the info & help you guys have given me,

Thanks again

[jwool]

Mike, where do i get one of these dial indicators?

[fleinbach]

Jwool,

I cut 90% MDF, and occasionally I cut 12 foot sheets of 1" MDF for closet shelving in one pass with a 1/4 inch bit. When I am cutting parts out of sheets of MDF I generally cut between .25 and .50 depths. I have never broke a white side bit except when hitting a screw. And once or twice I have actually cut a screw right off without breaking the bit.

Once by accident I was jogging at 30 inches per second and forgot to raise the spindle and hit the edge of a half a sheet of MDF. The impact was so great it jumped my X-car off the rails. I was totally surprised when it did not break the 1/4 inch bit.

[harryball]

I cut in a single pass. I know the chip load is technically out of range but in reality it's what works with the bit with the MDF that I have. I don't happen to have the MDF the MFG based their measurements on so I shouldn't be surprised if it's out of range. Now I didn't want to confuse you but yes, different MDF can cut different meaning you may need to change cutting speeds.

Here's a good rule of thumb: The bit should be installed as far as possible into the collet, it should ALWAYS make it AT LEAST 7/8 of the way in. I generally place my thumb nail on the bit just touching the top of the flute run out with the underside of my nail. I install the bit by running the top of my thumbnail up to the collet face. I end up leaving about 1/16" but make sure the flute does NOT enter the collet. If the flute must go into the collet to make it almost all the way in you either need a different bit or a plug for the back of the collet.

Dust will get into the collet... it just won't get between the collet and the nut or the collet and the bit until you change the bit. It's when you are changing you should be most concerned. It takes a little time to build up but eventually it will cause a problem.

I use the collet and nuts from ShopBot, I also ordered a 3/8" collet from Onsrud. There may be better but these seem to do just fine for me.

I know it may be hard to understand SB's position on this, but they are not experts on bits or manufacturing techniques. They do have good information, but honestly Onsrud and this forum are probably a much better source of information on the subject. If they did mfg product support they wouldn't have time to do technical support on the hardware.

Robert

[randy]

Jwool,

Try Harbor Freight for the dial indicator. For higher quality (and higher price) try one of the major distributors.

Randy

[richards]

Dial indicators are available from shops that supply machinists. I use the local Do-All store here in Salt Lake

DGI SUPPLY
1515 S. Pioneer Road
Salt Lake City, UT 84104-4113.
Telephone: 800-92-DoALL

You can also buy magnetic bases and other attachments to simplify the setup. Total costs for various parts and pieces should be roughly $100 - but the cheapest dial indicator and a block of wood works perfectly for this type of project.

[elcruisr]

Let me chime in real quick. First question would be collet age and has it ever been crashed. Collet life can be as short as a few hundred hours but typically more like 400. One crash can trash a collet. Also, don't save on collets. Cheap collets are lousy collets!

Next I run my chipload on MDF pretty high. I'd single pass 3/4 MDF with a 1/4" single flute compression spiral at 5"/sec at around 15,000 to 16,000 and have never broken one like that.

Don't know who your Onsrud rep is but see if they'll let you talk with Scott Fiemster. He's one of the most knowledgeable. If they won't give it to you contact me. I'll get you his number, he knows manufacturing well.

[jlg]

I have broken a few bit by cutting thing thicker than the cutting flutes of the bit. ( cutting 1 inch wood with a 1 inch bit) The flutes on the bit are even or just below the top of what ever material i'm cutting. When I do this the bit heats up and brakes just below the collect. This even happens even cutting foam.

[routerman]

Jeff, try using a cool tool...it seemed to help with me and broken bits. www.arizonavortex.com (http://www.arizonavortex.com) it gets the really cold and cools the bits.