MDF cutting

[joa]

I cut some MDF last night. Whew, that stuff is nasty! I'm definitely going to have to make a vacuum system, it gets over *everything*.

What feeds are folks running with this? Is it possible to cut through 3/4" MDF with one pass? I debated about whether to to cut on the table saw or the SB and chose the latter cause that stuff is heavy and I'm too lazy to put it on the saw! It seemed to cut alright though I took two passes and went slow. Was curious how fast folks are cutting MDF.

Thanks and keep those machines running!

[b1705@bellatlantic.net]

Joa, not only is MDF dusty, it is VERY bad for your personal health! The glue/resin they use is not one of the building blocks of life, and until you get your dust collection set up use a good respirator! If you got past your session last night without a headache, you did better than most...It is beautiful to work with because it machines so well, and that's why a lot of people put up with it. the price is pretty attractive too.I use a spiral upcut bit on it at about .5" and it cuts well.Bill P.

[troy@signaturearch.com]

I cut 5/8" MDF 10 hours a day, 5 days a week. I have (3) PR96 machines. The dust is a problem and it is true that i put up with it because it mills really nice. I use a WoodRite dust collector (two bagger 1200 cfm) for dust collection, above and below. i designed a vacumn table (similar to the one on this webpage) to collect dust below the cut as well. I use a 1/4" two flute spiral as well but a down cut so that the dust is pushed to the table below. It works well, we blow the shop out once every 2 weeks. I cut the 5/8" at 1"/sec, single pass. You can check out my product at http://www.signaturearch.com

Feel free to E-mail on any MDF cutting questions troy@signaturearch.com (mailto:troy@signaturearch.com)

[ummomob@yahoo.com]

I had cut 1" MDF in one pass using a 1/4" two flutes straight bit. In this case is very important to hold the material very strong and cut at .5"/sec or less no more than this.
From Mexico happy cuts.

[sheldon@dingwallguitars.com]

I developed an allergy to MDF a while back and have really cut down on my usage.

We have not been successful in our dust collection efforts using a brush foot. Our next dust collection attempt will be a filter wall built from pleated 1 micron filter cloth and a 3000 cfm barn fan. I'll post the results. I think a filter wall of this type would be a good idea for any shop using mdf on a regular basis.

[groover@americanwoodsign.com]

I am aware of the toxicity of MDF. I am now doing a rather lengthy project using MDO. This stuff is remarkably stable unless it gets wet - then it reacts like MDF. I have been told it is really nothing more than very compressed paper or cardboard. How about it? Is the dust (and it make a LOT of really fine dust) toxic or dangerous? I have not noticed any ill effects in the last two week that I have been using it without a mask or respirator.
Hugh

[kaaboom_99]

I would think that any really fine dust is not a good thing. I would recommend a dust mask or respirator when cutting this stuff

[sheldon@dingwallguitars.com]

Wood dust is considered a carcinogen. I can't see there being much difference at the micron level weither the dust came from natural or processed wood fibres.

[smartin@donek.com]

I used the door sweep around the bottom of my dust hood for about a year. When I couldn't find another one, I used a mountain bike tire inner tube. It works 10 times better, because it actually seals to the table. You just need a slightly larger hole in the dust hood where the the router bit penetrates it. All the air flows past the router bit and collects a lot more dust.

[Mayo]

Regarding the difference between natural wood dust and processed wood fibers like MDF :

"Real" woods contain fewer man made ingredients like glues, resins, formaldehyde and or mildewcides. When that router bit turns these chemicals to dust or gasses, it's probably not a good thing.

I wonder if the tree farms have to supply Material Safety Data Sheets... I know the companies that manufacture treated lumber have to provide the MSDS because the chemicals they use are toxic.

[smiller@heartlandscenic.com]

All man altered materials require an MSDS sheet, and those are availible from any lumber suplier. MDF is no more toxic then many products including a plywood, but yess the fineness of the particles can more easily get where you don't want them. MDO is also a fine product as long as edges are not as important. We run 2 shopbots and if our dust colector is working fine it handles most all of the mess, as well the foot keeps the dust from getting kicked up so bad. But the best I can do is let it run and walk away from it when I can. This also is good on my ears. My shop is big enough I have that option atleast when tool paths and type of cut allows. Other then dust and noise I feel there are few safty conserns compared to many of our tools. I do think it is probably the safest tool in our shop including a screwdriver.

[jay_mack1@hotmail.com]

Hello all,

I was working with MDF this weekend, building a speaker box with a couple guys. I'm looking to use it to carve intricate plaques. I was routing a dado, by hand. (no bot yet) I was cutting a 3/4" dado with a 1/2" pattern bit, running along a straight edge, I cut up close to the edge and then cleaned up, by coming back. This would cause the outer edge to blow off. Is MDF capabile of cutting fine details, without the router bit blowing out thin material...

[srwtlc]

Hi Stickman,

I've used MDF often for testing V-carved letters and designs and sometimes for finished panels. It V-carves real nice. It also works good if cutting with a stright, profile, spiral, etc., as long as you leave enough thickness between cuts. If you have too thin of a wall compared to the depth of cut it will snap off quite easily.

Scott

[stickman]

Need some advice on cutting MDF. I've got a few templates to cut out. I want to cut in a single pass. This is what I have at my disposal for tooling:

1/4" upcut and downcut spirals.

1/2" Single flute

1/2" Double Flute 1/4" shaft (I don't like this combination)

I'm figuring a 16,000 rpm @ 1 - 1.5 inch per second.

Thanks for your help

[gerald_d]

Jay, how thick is the mdf?

Forget about the 1/2" bit with 1/4" shank for through-cutting.

[stickman]

Gerald,

Sorry about that crucial piece of information: 3/4" MDF.

That was my thought exactly on the 1/4" shank. I found a v-carve bit the other day, 1 1/2" x 1/2" cut depth with a 1/4" SHANK! That would scare me.

[gerald_d]

We would use 1/4" bits because we have a small router, but the guys with 1/2" routers would probably use the 1/2" bits. However, we would make half the dust, get twice the detail on inside corners, and make half the noise, but we will take double the cutting time, although the programming and board handling times will be the same.

Having said all that, we will run 2 passes at 1.5 inch/second at 25 000 rpm (for single flute).

[elcruisr]

Wow, you guys must eat up some tooling with those RPMs. I can through cut 3/4" MDF in a single pass with a 1/4" upcut spiral at 2.5" / min at 10,000 - 11,000 rpm and get a good clean job of it. Yes I run a spindle not a router. My preferred tooling would be a 3/8 up spiral and I have used 1/2" tooling as well with similar feeds and speeds.

Eric

[stickman]

Eric,

I run a PC router, my slowest speed is 10,000. I would think at that rpm and 2.5/min I'd think I'd snap my 1/4" upcut bit right off. Feeding to fast for the cut? Or am I just being a newbie?

Gerald, when I've been cutting, I've been using a 1/4" upcut spiral. Three passes. So yeah there is time involved, that's why I was looking to speed some of that up.

Jay

[elcruisr]

Only time I have broken tooling was in solid wood, never have yet it 3/4" MDF. If it's good quality tooling and really sharp there should be no problem. Now if the tooling is dull it'll probably get pretty hot quick and the increased cutting forces of a dull tool might cause a failure. Since you're running a PC router I'm not sure how much rpm drop you'll experience. If it sounds like it's bogging down you could step up a notch on the RPMs.

Actually most people are surprised at how low you can run the RPMs and get good quality cuts. Check out Onsruds site for their reccomended feeds / speeds and an explanation of chiploading. Optimal chiploading is what you're after for cutter life and edge quality.

Eric

[gerald_d]

Eric, I have a theory about why you are successful with such "low" speeds, and remember that it is only a theory . . . . .

With your "spindle" (2-pole three-phase squirrel-cage brushless motor and high-frequency), when you dial in 10 000 rpm, you get very close to a true 10 000 rpm, irrespective of load. That style of motor does not drop speed drastically when loaded.

Us guys with the "routers", that have brushes, talk of our "dial-in" speeds, but under load we actually get a much lower speed. We really don't know how fast our cutters are actually turning. If we did dial-in 10 000 rpm with our gimmicky thumbwheels (for which the manufacturers are shy to state rpm) we would probably stall the motor under load and break the bit.

So, my theory is that "spindle" guys talk a different language to "router" guys when we talk of speeds. Spindle horsepowers are also not inflated like the router horsepowers.

Anybody else have thoughts on this?

[stickman]

Eric,

Aren't you using two motors on your Y axis?

Jay

[elcruisr]

Yes but the cutting forces in mdf are pretty small. I went that route to increase our cutting speeds in 3/4" plywood a few points. We cut thousands of parts in elliotis ply and an increase of .25" / sec adds up into dollars on a large production run.

Eric

[garbob]

Full cut through 3/4" mdf in one pass

I have used a 1 1/2 degree tapered 1/4" shaft cutter with a 1/8" ball nose from MSC to cut mdf in one pass - it really works. I got the info here on the forum, but I can't find the thread for the feeds and speeds, this was a while ago. All that I remember of the original thread that the guy was cutting 1" thick mdf in a single pass at 1 inch per second.

The part number from MSCs catalog on page 442 was 02958023 (TEB250-1) in May 2002 and the cost was $35.76.

I cut a few sheets of 3/4" mdf and it worked great. I loaned the bit to a friend for use on hand router, he broke it and paid me for it. Never replaced it as I hate mdf.

Hope this helps!

Gary

P.S. I found the link, it was Bill Palumbo
http://www.talkshopbot.com/forum/messages/28/1020.html#POST6026

[stickman]

Well to give you guys an update. I cut my templates this morning. I used a 1/4" upcut bit. At 13,000 rpms, using Gerald theory of 10,000 on a router might not be, I pushed it to 13,000. I cut at a speed of 1.75 and the pushed it with 2 inches. I did however duck behind the control cabinet at the first cut. Erik, not to be scared or anything. But with my first cuttings, I've gone with the conservative methods of multiple passes. I like the results, the only thing I was unhappy with was a little chatter at the start and finish. I need to spend some time learning about ramped entry's. What I'd really like is to get a chance to watch someone's machine do that and then learn from them. Thanks, so very much for your help. I look forward to more challenges. They make me a better operator and programmer! Thank You, Gerald and Erik.

[elcruisr]

Gerald is right to a point about the rpm drop while using a router head instead of a spindle. However most people don't really catch on for a while about the differences in CNC tooling design and running their hand held router with a regular router bit. I've had some long talks with some people in the tooling business and had quite an "education" on the subject. In fact I had to relearn a lot of my 20 years of knowledge of router bits.

CNC tooling has a more complex design than the router bits we all ran for years in our hand held routers. It's all about achieving a proper chipload and cutting force. From what I've been told by guys who work around the tooling design side of things, a tool run too fast (RPMs)and too lightly loaded (feed speed)or run to shallow (depth of cut)will give far from ideal quality of cut and a short life. We can also swing the other direction and get chatter and bit breakage. They are designed to run smoothly in a certain load range in a certain material. Our job is to educate ourselves about the tools we use and apply them correctly. The info is there we just need to avail ourselves of it. In our shop we use quite a few of one certain bit in a certain material and we have dialed that one in for maximum speed of cut and quality. It took some experimentation but we finally figured out that the tool manufacturer really did know what he was talking about with their feed and speed info. The speed being much lower than my old experiences with router tooling would have lead me to believe. The same was true with the number of flutes we needed. Old experience said two or more, reality in the CNC world was one.

So the point is we all need to do our research in tooling and it's best use as much as we need to learn about and research our machinery.

Eric

[sagreen83]

Ok... so here is an interesting twist to this thread.

I just got off of the phone with Onsrud. I was asking them about the 57-910 and 52-910 1'4" spiral up and down cutters. They are telling me that with MDF, use a feed rate of 200-450 inches / minute and 18000 RPM with a full depth 3/4" cut. He told me that most people cut too slow with their bits.

This equates to 3.33 ips to 7.5 ips. Thats faster than I ever dreamed of running a 1/4" bit. What am I missing here? Are the Onsrud bits that much better than other bits that you can run them this fast without problems?

Thanx,
Scott...

[fleinbach]

Scott

I just got my Alphaprt 120 up and running a couple of weeks ago and have cut several sheets of 3/4 MDF single pass at 9 in/sec 18,000 rpm using a 1/4" Whiteside up spiral. I even cut one part from 1" MDF, equating to about 6 running feet of cut, with one pass, but I slowed down to 7 in/sec I didn't want to push my luck.

I use Whiteside because it was conviniant they had them at my local Woodworker Supply. They are pretty tuff bits. I accidentaly maneualy jogged at 12 in/sec into the side of a piece of 3/4 MDF with enough force to jump the X car off it's rails taking a chunk out of and goughing a giant scratch in the MDF. The X car was teatering on top of the MDF. The bit didn't break to my amazment.

[paco]

Holly #!*?& !!!

Did you lose some accuracy from "pushing" that much?! Are you setup with a spindle or a router?!

[sagreen83]

Ok...

I just ran at 6in per second with the bits that I mentioned above and it worked great! I cant believe it!

Frank do you run at this speed cutting circles and squares (all different kinds of cuts) or do you slow it down if you arent doing straight cuts?

Thanx,
Scott...

[sagreen83]

Ok... Correction

6"/sec ran ok on a strait cut, but when I started cutting circles.... Very Bad! I slowed down my cut to 3"/sec and 2 pass and everything worked ALOT better.

At 6"/sec, 1 pass something is deflecting... Dont know if its something in the shopbot / porter cable, or its the bit or what... But I wont do that again!

Scott...

[fleinbach]

Yes, I have cut circles at 9 in/sec and they came out fine. I have a 3 HP Colombo Spindle

When cutting along the X axis in a stright line the bits cutting forces pull into the cut, cutting slightly off the intended center. The cut is other wise very straight as long as the cut has substantial material on both sides of the bit. If the cut is along the edge, but in just enough to get a full bite it waves down the board. If you make the cut using multiple passes accuracy is excellent.
I will be doing some more testing this weekend to find out if single pass cutting using differant speeds make any differance.
I have checked and tightened all connections. I am fairly sure I know what needs to be done to help aleviate the problem. I will be working on a fix soon.

[paco]

I wonder why it could be different in cutting circle than square??!!

I'll be watcing your testing!!!


Really, I will!!!

[gerald_d]

The controller has to think very hard when cutting circles - 2 axes have to run together at continuously changing speeds and resonances.

Squares are very, very, simple in comparison - one axis is "locked-down" while the other one runs at a fixed speed.

[paco]

So, Gerald, because computer have a hard time the carrier jump off rails...? It should be something about the shape of the cutter...down cut cutter Scott?

[gerald_d]

Paco, I did not say anything about like that!

[paco]

Hmmmm...
Ok, then do you (or anybody) have an idea about this observations? I just don't see clearly why a cutter (lets say a straight flute) would have more difficulty in shapes than in squares at a defined HIGH cut speed... Just to go deeper about the last posts (http://www.talkshopbot.com/forum/cgi-bin/discus/show.cgi?tpc=29&post=16132#POST16132) of this threads... Curious...

[gerald_d]

Paco, read carefully what I said. The answer is there. It has nothing to do about the cutter - it is caused by the controller/motors/structure/resonances.

Thread on this topic (http://www.talkshopbot.com/forum/messages/26/1370.html)

[paco]

Hmmmmm....

[sagreen83]

Paco... Yes this was a downcut spiral bit.

I spoke with Onsrud again this morning. Their speed estimates were based on a 1/2" cutter. I was using a 1/4" cutter. So, they say that their recomendations are to cut through a maximum of 1.5 x diameter of bit. So in this case 3/8" in one pass. And since this was a 1/4" bit the speed should be between 100 and 220 inches per minute. So my 3 inch per second 2 pass was right in the ballpark of what they were talking about.

But this brand new cutter caused a few burn marks upon plunge. I noticed that there is a setting in Parts Wizard to plunge into the material slightly offset from the start point. Havent tried that one, but does anyone know if there is a setting in parts wizard to ramp into the cut?

Frank, any updates on your testing?

Thanx,
Scott...

[fleinbach]

I am organizing them and will post them soon

[paco]

See!!!

Control software characteristics might explain "roughness" in circles/shapes definition... but not deflection at cutting at high speed in circles/shapes than in "squares"... Bit should, the way I see this, cut equaly in any directions... In other words; I don't see why a bit could cut correctly a square at defined speed but not a circle/shape at the same speed setting?!...

Opinions and theory?!

[fleinbach]

First and foremost when you read this keep in mind the Alphaprt or any model CNC will only cut as well as the skill of the operator. When the Alpha is properly adjusted and proper cutting techniques are administered you will obtain high quality parts I am sure.

I made the error of expecting more then should be expected. I was thinking mainly of getting the maximum pieces from the material by making a cut line that would produce usable pieces on both sides of the line. Trying to make accurate size cuts in 3/4 MDF in one pass is never going to be possible with a machine at this price range. Nor probably even in a more costly machine. Though I have no experience with any other CNC I do remember reading a 200 plus page book (This was actually pointed out on an earlier post but I don’t remember which one) on the forces affecting the quality of cut CNC machines are capable of. The author went into great detail about all the variables that can affect the quality of cut. He even described having been involved in engineering two machines between 1 and 3 million dollars.

There are many factors involved in obtaining clean accurate parts. This is most likely one reason why all cut path software I have seen have an offset field for a final pass. The first pass or passes are biting into and removing large amounts of material causing extreme forces on all parts responsible for keeping the bit on track. No matter how well constructed these parts will have some degree of movement if enough pressure is applied too them. This final pass removes a much smaller amount of material therefore exerting far less pressure allowing the bit to follow the cut line far more accurately. All that is necessary to obtain accurate parts is to remember this and not try to make them in one pass. When I had my old Prt96 if accuracy was not important I would ignore making a final pass. But if I wanted accurate clean parts I would set the final pass parameter.

Trying to make accurate single pass cuts in 3/4 MDF with this CNC (or any other) is never going to be possible no matter how well adjusted they are. Though you can make extremely clean single pass cuts in 3/4 MDF with the Alpha they will not be accurately sized. Even though the cutting forces pull the bit off the intended line they remain very smooth with proper feed rate and spindle speed combinations. The forces when cutting 3/4 inch deep are too great for one pass accurate size parts. The Alphaprt is very capable of making clean single pass parts from 3/4 MDF as long as accurate size is not important.

If intending to cut a part and maintain accuracy a combination of cut parameters is necessary and varies with each choice made. There can be several right choices. First you must know how much error will be induced at your intended setup. Here is an example cutting a part from 3/4 MDF.

1. My first setting is to cut around a part counterclockwise in one pass at 10 in/sec. I know that my tool removing 3/4 inch in one pass will pull into the material a maximum of .0468 " from the intended cut path at this depth. So I will set the final cut offset to .050. The first cut will try to cut around the part by this offset but the cutting forces will pull the bit toward the actual part perimeter by .0468 leaving approximately .0032 of material to be removed by the final pass. Removing this small amount of material on the final pass will create a very smooth cut and accurate sized part.

Below are the results of my testing for the past two days to determine the tracking capability my Alphaprt under various cutting parameters.

Before conducting these tests I went over all connection points and bearing adjustments taking out as much free play as possible. All tests where made using a home made gauge on the X car to measure any movement of the Y car on the opposite side from the motor. This gauge has a ratio of 6 to 1 making it easier to see smaller movement with the carriage moving. I did make a few runs with another gauge on the motor side just to see how much it was contributing. I found that the motor side does contribute to about half of the movement. The motor side movement seems to be coming from the flexing of the bracket holding the motor. I checked and found it to be as tight as possible. Any farther tightening won’t allow necessary movement to engage the gear track. The opposite side movement is due to a combination of parts. I did make a video of a few test runs showing these results.

I ran these tests by cutting 8" slices off of scrap 3/4 MDF. I used 4 different bits to include 1/4 up spiral, 1/4 down spiral, 1/4 straight and 1/2 up spiral. I ran speeds from 12,000 to 23,000 RPM and feed rates from 3 to 10 in/sec. RPM seemed to have the least affect on the results. Lowering the feed rate below 5 in/sec while making full depth cuts reduced the error by half. The spiral bits all produce nearly the same results while the straight bit showed markedly worse performance. I only made one pass with the down spiral as after 6" of cut it was becoming very erratic. The reason was on the last 2 inches it had severely packed the cut with chips compressing them to the point of almost being solid again.

The highest error while traveling along the X axis was slightly over 3/64"

I next decided rather then just seeing it on a home made gauge I could measure it with a micrometer right at the bit. I accomplished this in the following way. I cut a piece of 1 inch MDF down the X axis 3/4 inch deep at 10 in/sec with a 1/4 inch up spiral. Next I moved the Z axis down to 0 (table surface) and cut the remaining 1/4 of material depth from the other direction. This left a distinct shoulder. I next sliced the piece off at 1" so I could put my micrometer on and measure the difference. The difference was .049 or slightly over 3/64 inch. I then tried again but this time my cut depth was only 1/4 inch. This was much better producing only .020 inch of difference in the cut. So the more material you remove at one time the greater the margin of error.
I had been concentrating on the X axis all this time since it was the one I had encountered the problem with trying to cut equal sized rips on. So I repeated the tests above only this time down the Y axis. The readings though better then those down the X axis where similar.

This error was first noted and is compounded significantly when trying to cut equal length rips from a sheet of MDF. For the most efficient cutting action I chose to cut each line first up the sheet in one direction then return down the side in the other. Now consider that on the first cut the bit is pulling into the rip 3/64" then when coming back down on the second cut it is again pulling toward the first cut by another 3/64". So compounded you get a 3/32" error in size creating a board that is smaller by that amount. Now remember that while coming down the second cut you are also cutting the first line of the second piece. Only this time the cut is pulling away from the intended second board. When you go back up the next line in the other direction you are now pulling off course away from the previous cut. So what you wind up with is a board 3/32 inch larger then intended. Now since one board is 3/32 smaller and the next is 3/32 larger the intended size difference is doubled at a 3/16 inch difference in size.

Conclusion
Varying spindle speeds and feed rates affect tracking very little. Reducing depth of cut has the greatest affect. Taking a 1/4 deep bite at a time reduces the error significantly. This holds true even at 10 in/sec.
So my conclution is if you want high quality parts made at the fastest rate possible with the Alpha but finished size is not important pick a bit and match its cutting parameters for a one pass quality cut. On the other hand if you want high quality exact size parts you will need to accept making more then one pass and include a finish pass removing only a small amount of material.

[paco]

THIS IS GREAT DATAS FRANK!!! Thanks for sharing!
I have questions for you;
Did the finish results with down cutter VS up cutter significant different on flexing the machine (the way it flex and the intensity of the flexing)?
Do you suggest that the final finishing pass be full depth (still, looking to remove little amount of material; from 0.010" to 0.03125") of material instead of multi-pass as "first" pass? As this could improve finish quality...
Would you hold that the general suggest depth of pass (to obtain high toleranced parts) be no more than 1.5 X the diameter size of the cutter? Or less?!
Thanks again! 8-)

[fleinbach]

Paco

I only made one pass with the down cutter and it was 3/4" deep. After 6" of cut thing where getting a bit choppy. The cut was very wavy at the end. I was glad the board was only 8" wide because from the way things where vibrating I had the impresion the bit was picking up the whole X car. This seems to be confirmed by the heavely packed chip in the last 2 inches. They where tightly packed and created a ramp approximatly 3/8" high at the end. The X car appeared to jump up right at that point like the bit traveled up the ramp. This may not be the appropriate way to use a down spiral as I have only used it when cutting 1/4" luan in the past. It worked great in that application.


Yes, full depth taking off small bites creates a very smooth surface. In fact I used a 1/2" straight bit with a 2" cut lenght and removed a .010 layer along the edge of my table which has two 1" pieces of MDF surfaced down to 1 7/8" in one pass. This made a very clean edge.

[elcruisr]

If you want clean accurate parts with any kind of speed you'll need to get away from those 1/4" tools. As you noted the 1/2" tool gave a better edge. I've achieved part accuracy of .005" with 1/2" tools at 4"/sec doing .5" passes with a .05 finish pass. I am cutting with a spindle by the way. I can generally hit parts between 1/64 and 1/32 at 8.5"/sec with 3/8" tools single passing on 3/4 plywood and 3/4 mdf. The same material at 10"/sec is generally at 1/32 withing tolerance.

Alot of this is about tooling, tooling, tooling. Cheap tools will give bad results or need to be worked slower or dull so fast as not to be worth while. I've tried alot of brands over the last 2 1/2 years to arrive at this conclusion and bent the ear of many a CNC operator. I've pretty much settled into one brand these days. Then the machine has to be adjusted right and then the software needs tuning. Take the time to learn your machine and it will pay off big! CNC is not a magic wand!!!

This is on a PRT upgraded to Alpha steppers.

Eric

[dingwall]

And that tooling supplier is...?

[elcruisr]

Well I've tried MSC, vortex, courmatt, whiteside, eagle, onsrud, mastercut and about 6 others whose names I can't remember. I'm not saying they are the best for everyone but for what I do I use 95% onsrud these days. I use a few tools they don't make like a PCD slotwall cutter from courmatt and a few 1/16 upspirals from msc for special jobs.

I production cut for outside customers as well as our in house work and push the 'ol 'bot pretty hard. Sometimes it's been two shifts a day! (Thankfully no more since the Alpha upgrade)I need tools that give good cut quality at all the feed I can give and will stay sharp as long as possible.

Onsrud is also the only company who has put a tech rep on my shop floor with tools in hand to help speed me up. They cost a little more but it's factored into the job and they've always delivered the goods for me.

Eric

[fleinbach]

Correction on my previous post about using a down spiral cutting bit.

Today one of my guys put in a down spiral 1/4 bit by misstake. We cut several parts from the 3/4 MDF sheet at 10 in/sec with a spindle speed of 16,000 rpm using the 1/4 down spiral bit at full 3/4 depth. 2 pass's where made, the first .050 from the finish line, and the second being a cleaning pass. The cut quality was very good creating a clean edge with no noticable tool marks.

[karlo (Unregistered Guest)]

I just bought a alpha96 with a 3h.p spindle. I have read through this post and still have to ask, for cutting 3/4" mdf should you use 1/4" shank or 1/2" shank? Also is it preferable to use an up spiral or down spiral?

[ron brown]

Karlo,

I hesitate to push a bit much past 2X diameter a pass. If you are buying a true spindle, collets will be available for almost any diameter from 1/16" to 5/8". There is a 3/8" compression spirial many have had good results with on 3/4" material.

Ron

[bjenkins]

Karlo,

I would suggest a couple factors enter into my decision of bit diameter. First, I agree with Ron and would have to say 3/4" MDF is at least two passes with a 1/4" bit. You can spend extra time cleaning up edges-- a bad trade off. Unless you have detail that prohibits it, I'd opt for the 1/2" bit. You can make the cuts in one pass and get better finish on curves in my experience. That's just my opinion based on my experiences so far.

[fleinbach]

I do not have as much experience as many but I can only state that I have cut about 120 sheets of MDF when I had my Prt96 all with 1/4 bit usually at 2.8 in/sec and 16,000 RPM making 3 passes. Since I set up my Alphaprt 120 with a Colombo spindle I have cut 12 sheets of 3/4 and 1 sheet of 1" MDF. Some cuts where one pass, full depth, with a 1/4" Whiteside solid carbide at 16,000 to 18,000 RPM and 10 in/sec. There was no need for a better finish as these edges where being attached to another part. On the rest of the parts I made a second full depth finish or cleaning pass and received an edge that was not perfect but good enough for my application.

[ron brown]

Side note:

Porter-Cable has a 3/8" chuck for their routers. The insert is about $9 and the complete unit is $25 IRRC. I only buy the inserts and new snap rings.

Wax in the proper spots, just a touch - never on the shank area of the insert or bit, will make life a lot better in the world of bit changing.

Ron

[elcruisr]

Karlo,
as Ron pointed out there are some excellent 3/8" tools out there or this kind of work. They are much stiffer than the 1/4" tools and less expensive than the 1/2". They also generate less dust! I've run hundreds of sheets of 3/4" mdf as fast as the Alpha will go with good results on 3/8" tooling. We generally only go to 1/2" tooling only on stock over 1 1/8".