Noisey Bit

[fleinbach]

I am getting an extremely loud high pitched noise since I switched from Whiteside to Onsurd bits. I was using Whiteside bits for the past year and they cut very quiet. I switched to Onsurd and now get a high pitched noise almost unbearable at 16,000 rpm. It is reduced in half if I spool down to 14,000 rpm. To give you another example of how loud the sound is, I can’t here my 5 HP vacuum system running over the sound. When using the Whiteside bits the most annoying sound was the vacuum. Everything I am describing here is using a ¼” 2 flute up spiral solid carbide bit cutting MDF at .25 depth at 2.8 in/sec. I am using the same profile Onsurd bit at the same rpm and feed rate cutting the same material that I was using the Whiteside bits, but the Whiteside was much quieter. It seems strange that this is the case but I can’t figure out any other change that would cause this. As soon as I get a chance I am going to pick up some more Whiteside bits to see if they are still as quiet or my hearing is coming back.


Also I have broken 3 Onsurd bits cutting just a few parts .25 deep at 2.8 in/sec. The only time I ever broke a Whiteside bit was when I hit a screw. And most of my cutting with the Whiteside bits was 3/4 to 1" deep at 10 in/sec and never even broke one.

I just though I'd throw this out to see if anyone else has ever experienced anything like this.

[beacon14]

Frank,

How old is your collet? Maybe worth a try to see if a replacement collet helps.

[fleinbach]

I have a 3HP Columbo spindle new in July. This problem happened immeadiatly when changing from Whiteside to Onsurd.

[elcruisr]

If you're breaking bits at those parameters then something is out of whack somewhere. First off, a collet is only good for around 100 hours of work. These are a disposable commodity and can create major headaches if not replaced. Don't buy bargain basement collets because they have more runout than you can shake a micrometer at, high precision only! Next would be are you getting the cap nut torqued correctly. We solved some headaches by using a torque wrench to achieve the recommended 85 ft lbs.

Have you checked to make sure the spindle is dead on plumb with the table?

You need to get the feed and speed values from Onsrud but I run single flute Onsrud bits like you are using at 12,000 rpm at 5"/sec in 1/2" mdf. If a bit is screaming it's turning too fast, if it's growling it's too slow. For the kind of work you're doing I would also be running a single flute tool, not a 2 flute. 2 flute tools run too slowly will scream like mad because the chip load is below proper levels. If you check the chip loading for what you are doing, you need a bigger chip to carry away the heat and load the tool properly. These are not router bits but CNC tools unlike the Whiteside bits. The geometry is a little different. They need to be run correctly in a good collet and they will deliver great results but we users have to run them like they're designed to run!

The only Onsrud bit I've ever broken was when I hit a clamp, and I've been through several hundred!

Eric

[simon]

Eric
Have you missed out a zero or two somewhere? 100 hours of use for a collet seems awfully short - about a month in the life of a well-used shopbot.
Surely it is only changing bits that wears a collet. If you clean them each time you change bits they will last a long time.

[elcruisr]

Sorry Simon, that's straight from Onsrud, the collet manufacturers I've contacted, several other sources in the CNC industry and backed by personal experience. For us that means a new collet sometimes every two weeks. That includes cleaning the taper and brushing the collet with each bit change. It seems that it's the vibration from cutting that's the problem, not changing the tools.

Eric

[fleinbach]

I would have contributed to this thread sooner but the past 3 days where very hectic.

Eric,
I once purchased a windshield wiper from my local Pep Boys and about 4 months later it was failing to clean the window properly. I went back to Pep Boys and explained my problem and was told "didn't you know the manufacturer recommends changing wiper blades every 3 months, so naturally you need a new one." How strange since the car was 6 years old and the passenger side still had the original one but it forgot to fail after 3 months. Or maybe they aren't actually working at the same time. I bring this up to point out that manufacturers make product claims that sometimes border on ridiculous.

"These are not router bits but CNC tools unlike the Whiteside bits."

I'm not sure what you meant by this. Did you mean Whiteside bits are not for CNC use? If so you can read this "Whiteside router bits specializes in CNC router bits" on this web page. http://router-bits-shaper-cutters.com/information/whiteside_router_bits2.cfm


READ COMPLETE ARTICLE HERE http://www.taunton.com/finewoodworking/pages/w00045.asp (I'm not sure why but you need to copy and paste this link as it did not get hyperlinked when I edited)
All bits where tested on a CNC machine

What I am about to say next may or may not be enough information to come to a conclusion but it is my experience and "experience is the best teacher" as they say. I will also admit, Eric, your experience with CNC is probably 100 times mine.


Here are my results’ cutting 3 /4 to 1" MDF. I will use hours of cutting time for reference since parts can be cut from sheets from 5 minutes to over an hour depending on how many parts are on a sheet.
I have used other bits but this example only pertains to cutting with a 1/4", solid carbide, 2 flute, up spiral bit:


5 Onsurd bits:
Cut Time: approximatly 15 hours
Spindle speed: 14,000 to 16,000
Cut Speed: 1.0 to 2.8 in/sec
Maximum Depth of cut: .28"
Outcome: 2 bits broke hitting screws. 3 bits broke during normal cutting

8 Whiteside bits:
Cut Time: approximatly 150 hours
Spindle speed: 12,000 to 20,000
Cut Speed: 2.0 to 10 in/sec
Maximum Depth of cut: 1.0" (and this was at 10"/sec)
Outcome: All 8 bits broke hitting screws.

Conclusion bit life:
Onsurd average 3 hours
Whiteside average 18.75 hours (If I learn to stop hitting screws I think this number would be much higher)

I might add that twice I made the mistake of leaving a piece of MDF screwed to the table and ran into it while jogging home at 30"/sec with the Whiteside bits. Both times the force was so great the X car jumped off the rails and teetered on the 1/4" bit. I was amazed as the bit did not break either time and I was able to cut again with no apparent adverse effect.
The only time I ever broke a Whiteside bit was when hitting a screw.

At this point it seems at least for me Whiteside is winning.

[elcruisr]

Frank,
I'm not knocking Whiteside bits, most of my hand router bits are Whiteside bits and they are excellent. But we work in very different areas with our CNC machines. I production cut thousands of sheets of 3/4" plywood, melamine, particly board up to 1 1/8", MDF, foams and solid wood each year. My current big run is for 80,000 parts! I look for tooling that let's me cut as fast as I can with the cleanest results with a minimum of tool changes. The Whiteside bits I have tried where carbide tipped and are really great in a hand held router but did not give me the results I need in a CNC spindle. Conversly the Onsrud products have performed better than anything I've run and I've tried a lot. That being said they do have to be run as designed within feed and speed and depth of cut. For the tools you where talking about they where being turned way to fast for the feed speeds and depth of cut was very shallow unless they had a cutting length of 1/2" or less. The high pitched scream is a vibration that is going to shorten the life of that tool. To really test the tool and it's useable life it should be run as intended. If I run a normal street car with an unmodified engine at redline rpms it won't last long either. I've never broken any tool made by any manufacturer yet that did not hit a clamp or that was not being run within it's designed parameters with the exception of bit's under 1/8". Those have pretty short life expectancies anyway.

On my machine I can take a 1/4" two flute tool and run it in one pass on 3/4" MDF at 5"/sec at around 13,000 and it should run all day, my tool of preference would be a single flute compresion spiral though. Shallow passing at something like .28" should be done with a shorter cutting length. I'm told by my tool grinder a tool should be loaded at over half and preferably 3/4 of it's cutting length to avoid vibration issues. That's what I mean by using the tool as it's designed, load it up as it was meant to be at the chipload it was designed for and it will give the best results.

I've found one of the biggest learning curves we face as shopbotters that is really overlooked is learning about tooling design and geometry and how that translates into the work we do. I figured after 20 years of woodworking I knew a thing or two about router bits. The more I study the subject now the more I find I have to learn. It's really a fairly complex topic that I find very interesting and there are a wide range of opinions out there! What much of it boils down to is there are different optimal tool geometries for each different type of material out there and that can even change depending on the feed speeds and desired finish of the cut. Then there are all the different carbide grades that perform different jobs well but are not suitable for all jobs. Then there's all of us individuals with all of our opinions. What fun, what fun....

Eric

[fleinbach]

Eric,

Thanks for all your time and effort explaining your experiances under varying conditions. I certainly do not have as much time and experiance as you. I realy need to go buy another Whiteside bit to see if the Noise stops. It just seems ironic that I was experiancing a very moderate noise level using the Whiteside bits. Then the first time I switched to the Onsurd (and remember all other cutting parameters where the same as the Whiteside) I recieved this high pitched unbareable noise. Did something else change at the same time? The only way I will know for sure is to try another Whiteside and see if the noise is reduced to where it was. If it also produces the noise I will look elsware for the problem.

[dingwall]

Frank, I don't know if this would help or not, but maybe using smaller brass screws instead might save a bit or two. At least at slow feed rates.

[fleinbach]

Sheldon,

I thought of Brass and also Aluminum, but I'm unaware of a manufacturer that make either with self cutting threads. And even if they did my guys would never get them in without striping the head. They strip the hardened steel ones often enough.

[garbob]

Whiteside VS Onsrud on a PC Router

I have always used Onsrud bits for everything, but due to the slowness of my PRT96 machine there is no way that I can get the chipload that they recommend.

The cost of Onsrud for the time I get from them is horrendous. Someone recommended Whiteside to me a long time ago for cutting 1" mdf in one pass on my machine and I thought that they were crazy.

Long story short - bought a few 1/4" compression bits from Whiteside (UD2100) at about a 1/4 the cost of comparable Onsrud bits for cutting red oak laminated panels that are 7/8" thick. I am cutting these panels at 1 1/2" per second and the higest speed on my PC 3 1/4 hp router (the variable speed switch has never worked, will only run at top speed) in a SINGLE PASS and the finish is amazing. There is absolutely no tearout at the top or bottom. I have cut about 10 sheets of intricate parts from 3/4" ply and about 20 thirty inch by 13 inch oak panels and there is no sign of the bit getting dull. The only bad areas are where the bit enters and leaves the material causing about a 3/16" burn mark.

Fantastic bits for the poor old PRT machines running PC routers.

Gary

P.S. An example of the oak panels is at my site http://www.sugeri.com under Automated cutting/Carved Items - the 92 Elwood sign.

[fleinbach]

Gary

Great web site. Nice work.

I didn't think I was crazy stating that I was getting far better preformance from Whiteside bits over Onsurd. Finaly someone is confirming my findings. I just got back from purchasing some more Whiteside bits. It may be a couple of days before I actualy get to find out whether or not the Onsurd bits are the cause of the noise but I will post my findings then.

[bruce]

This is a pretty old thread, but I thought I'd add to it with both a comment and a question:'

Like Frank, I've noticed that my Onsrud bits make a heck of a lot of noise. Good to know that there are quieter options.

My question is this: I've been cutting 1/4" MDF, and I've noticed that I'm not getting perfectly perpendicular cuts, especially on parts of the cut where the bit is climbing. My assumption is that the bit is deflecting. Has anyone noticed that Onsrud bits flex like this, or is there another explanation for my problem? (I'm confident that the bit is true to the table: it's in the process of cutting that things go out of whack.)

Merry Christmas everyone!
Bruce

[elcruisr]

If the bit is that noisy then your either feeding to slow or running the rpms to high. If you are experiencing deflection then go for a shorter cuting length tool or better yet step up to a 3/8" tool.

Eric

[fleinbach]

The problem has been solved. I switched back to Whiteside bits and have'nt expierianced the noise since. Plus I have'nt broken one single bit since switching back to Whiteside either.

I realize many people in here will disagree with me about my opinion of Onsurd bits but my experiance with them has not been good. I bought 5 each 1/4" solid carbide Onsurd bits and broke every single one while in the process of cutting MDF. And in a very short time also. Yet while cutting using exactly the same paramiters I have never broken a single Whiteside 1/4" solid carbide. Nor have I heard any unusual noise from them.

[cnc_works]

Bruce, I have been experiencing a similar problem with the sides of my cuts in 3/8" acrylic not being perpendicular. For example, if I were to cut a circle, I was cutting about 3 to 5 degrees off perpendicular, making a cone with the small side up. Same thing happened cutting a square. Didn't seem to matter whether cutting climb or conventional.

Called ShopBot and Tim told me to check various aspects for tightness and it all checked out fine.

I was using an Onsrud bit designed for acrylic, so I called them and their tech guy said my collet or router bearings was worn. I checked and sure enough, there was a little bit of play on my PC890. I replaced it and now have perpendicular sides. YMMV.

Donn

[elcruisr]

Frank,
just because you ran them in the same parameters does not mean they where used as designed by the manufacturer. They will each be designed with different geometry. Each manufacturer has their own rake, cutting angle, twist angle, etc. They are designed to run at a certain rpm and feed speed also known as a chiplod. If you operate outside of the manufacturers specs then you will have problems. If a bit is that noisy it's not running right. If it's not running right you will probably break a small bit like that. I'm not trying to defend any one manufacturer but trying to say a tool has to be used properly just like any other cutting tool in the shop.

Eric

[fleinbach]

Eric,

Thanks for the info. When I get more time I may research this farther to find out why it happened, but for now I can cut using the Whiteside bits under varying conditions, in different materials, with nice clean cuts, without any problems. It I start having any problems with them I will certainly have to look for a solution, but until then they cut everything I need cleanly and accurately.

[burchtree]

Frank the correct term for the noise you were hearing is chatter. Chatter needs to be avoided as much as possible because it is hard on the whole machine not just the cutter. Go with the bit that works.

[bruce]

Donn,

Thanks for your info. My router is definately getting old, so I'll bet the problem is with the bearings. I haven't had time to do a run-out check, but I wouldn't doubt if there's some problem there.

Bruce

[jsfrost]

This could go in many places, but I’ve chosen here, because it involves the two bit manufacturers discussed. The goal is to show that bits, machine, control software, toolpath, machining strategy and other items can interact in surprising ways. I have an Alpha, PC router, and created the toolpath using the Insignia Engrave function. Although the bit appears to be the problem, the actual cause may well be the idiot incorrectly using it.

Simplified goal: Cut a .2 inch deep beveled edge on the inside curve of a 5 by 8 oval in maple. This was successfully done using a Brand X 90 degree V, then repeated successfully using a brand Y 60 degree V because I thought it needed a less radical slope. We then did a new toolpath with the identical oval, with a different DFX within the oval. The oval now cut from X min to X max, then cut the remaining half oval with X behaving normally and Y doing a pseudo random walk, resulting in a nasty ditch in the center of my piece. When the cut was aborted, Y zero had changed several inches. Preview and aircut normal, repeated attempts to cut in wood showed an essentially identical meandering in Y starting at essentially the same XY. Eventually( a short word for the better part of a day), I found that I could always cut successfully with brand X, and rarely with brand Y.

Jim Frost