Chip-free two-sided melamine

[tbhayes]

I'm looking to process 3/4" two-sided melamine with a particle board core for closet shelving components. I need to be able to rip 4' x 8' panels lengthwise, and any type of sliding table saw or vertical panel saw that has a least a 96" stroke is priced close to what a ShopBot would cost. Add in a line boring machine, and some other equipment necessary for RTA fittings and the equipment costs are almost identical to a ShopBot.

So, here are my questions...

Can the ShopBot cut two-sided melamine chip-free? If so, how long can I expect the bits to last?

Is the spindle the best option for this application?

Can I initially save some money on the vacuum hold down system and mechanically fasten my stock to the table? Some 4' x 8' panels may only need three rip cuts before going to the edgebander.

The ShopBot may seem like overkill for what I need it to do, but I like the idea of reliable, consistent quality and depending less on the skill of my shop labor.

Basically, I want to use the ShopBot as a table saw to rip and cross-cut my panels, drill for shelving holes, hinges, slides, etc. and reduce the number of times each piece is handled.

Is anyone currently doing this?

[Gary Campbell]

Tom..
David B. is currently doing a lot of what you list above. I would reccommend at least a 4HP Spindle for single pass cutting of 3/4" material. Also would reccommend a compression spiral. You may be able to get "creative" with other hold down methods, and many do, but vacuum is really the only way to go. IF your cut components are large it really doesnt take a lot of vacuum $ to hold them. We use ours on a regular basis to dado, cut screw pockets, size panels and drill for hinges,slides and shelves.
We dont cut melamine, mdf or particleboard, so I will let the guys that cut it give you a guesstimate on the bit life. Hope this helps.
Gary

[beacon14]

Yes, I do cut a fair bit of 2-sided melamine and I get pretty consistently chip-free cuts - I'll never say that I get no chips at all but overall my edges are much better than I used to be happy with from the table saw, especially on the underside. I'm using a 1/4" compression spiral from Whiteside (ordered from routerbits.com) and am paying $1 or less per sheet for tooling.

I just upgraded from router to spindle (2.2 Hp HSD) and would say that what I have now is the minimum for any real production requirements. The 4Hp would be better but I am limited with my electrical power. I got by with the router but was replacing bearings every few months.

As for the vacuum - don't bother trying to make do without it. It saves so much time and trouble and improves results so much that it should be your first project.

Finally, the Shopbot is not overkill for your use, it's perfectly suited. Sure it can do a lot of fancier stuff that you may never have a need for, but that can be said for any tool in the shop. As long as it can do what you need it to do, it's worth having.

[thewoodcrafter]

I cut a lot of melamine, nested cabinet components.
I get about 25 - 30 sheets from a bit.
If you are just ripping a few cuts from a sheet you may get 100 sheets per bit.
I too vote for vacuum hold down. Much less time and trouble than clamps and you really can't hold melamine with brads.
Get a spindle for sure, build a 4 zone vacuum table and buy 2 shop vacs, you'll never look back.
If you want real production add an air drill for your holes.
You will find other things to cut.

[myxpykalix]

To round it out i would recommend www.centuriontools.com (http://www.centuriontools.com) for quality bits to make sure both edges of your melamine don't chip when they are being cut. Call Fred and talk to him about specific bits to use.
I would bet you would get more use than 100 sheets per bit, but i'm just guessing, but it would be a good question to ask him. Roger and David sound like the expert here on this though.Hmm..maybe THEY ought to check out centurion also? lol.

[elcruisr]

The number of sheets you cut per tool is purely a question of the inches of cut per sheet and chip loading. There are also some tricks like ripple cutting that will extend the life more. I've cut sheets with 40 complex parts that mean a life of about ten sheets. Large simple parts can mean 40+. I don't think anybody is going to cut up 100 sheets of nested cabinet parts with any tool short of diamond and it's not recommended for particle board.

Different brands of melamine are going to effect tool life. Some melamine faces are so hard they can actually notch a carbide tool after a short run, I've had some of that horrid stuff in my shop! Others are much kinder to tooling. Then there's the occasional chunk of trash in the core that can pretty much trash any cutter that hits it.

Look at your software package as much as the machine. You'll spend a fair amount of time on that computer until you have a good library of parts. The stock software may be exactly what you need or you may have something in house already that you can work with.

The vacuum hold down should not be overlooked! I use a 15 hp regenerative blower and for the production work I do I consider it a minimum. I also run a 5 hp spindle and would never want to go smaller than a 4.

Investigate your tooling and see what works best for you. I'm a big fan of Onsrud, they've done me well for over 200,000 parts. You'll want a compression spiral. There are different geometries and lengths of the lower, upcut, spiral. For me the Onsrud 60-121 single flute compression spiral does best in melamine. I can single pass feed it at 7 to 8 inches/sec at 18,000 and get really good results. Good results for me mean NO chips in the edge. I've got picky customers......

[erniek]

Hello,

My first post, I recently purchased a PRT and am using it to cut 2 sided melamine. I am using a 3/8 compression spirel bit from Onsrad and am getting excellent cuts. The first bit is dull after cutting 2 sheets. I'm told by the supplier that I should cut about 50 sheets if the feed rate is 10 inches/sec. I was cutting at 18,000 rpm. and 3 inches/sec. Which probably explains why it dulled so quickly. Now I'm trying 10,000 rpm. Anyone know if I'm on the right track? I guess I should have bought an alpha. Is it wortwhile to upgrade a PRT to an alpha?

[elcruisr]

Is it a single flute or two flute cutter?

[erniek]

It is a two flute cutter, the 60-123MW from Onsrad.

[handh]

I have been using the 2 flute cutter from Onsrud and I usually get around 75 sheets on a cutter, like others have stated its according to how much cutting is done on a sheet. One thing that I will also add is that dust collection is a major factor in tool bit life. By switching dust collection systems our cutting life went way up.

Jeff

[handh]

We cut in two passes on 3/4 melamine, the first pass is set to .625 and then the second for the final thickness, we get better hold down and cut quality is great, really no chipout, one thing is to purchase nice melamine don't use the cheap material. The particle size in the melamine makes a lot of difference in the quality of cut.

Jeff

[erniek]

Jeff,

What feed rate and spindle speed are you running at?

[elcruisr]

"Now I'm trying 10,000 rpm."

Onsrud likes to see about a .016 to 018 chip load per cutter in laminated particle board per their factory tables. To do that at the speed you're feeding you would need to be turning about 5,000 rpm. That's gonna stall a spindle. For your feed speeds you really should look at single flute cutters like the 60-121. That would let you get a good chip load at 11,000 rpm and your cutter would last longer and the tool is a few $$ cheaper. When I was running a PRT I use to turn closer to 12,000 at those feed speeds but was seeing a little better edge.

[handh]

Spindle is 12,500 and feed is 7.5 inches/sec

Jeff

[handh]

One thing is to make sure you are getting actual chips. Take a caliper and measure the chip size. It depends on the brand of melamine, you will have to adjust for your own.

[toolguy]

Tom,
I sell tools for a living.(also own a shopbot prt Alpha which I love) I know it's hard to get the correct bit with the right RPM's and feed speed to match all the different materials out there. I have 10 different customers who all claim that the bits they have are the best and last the longest. What I tell most guys is that you buy a bit recommened for whatever material you are cutting. Double sided pvc would use a compression bit. I would run the bit at it's recommeneded speed usually 18,000 or more. and feed it as fast as you can until it starts to chip then backoff. this will allow the bit to dissapate the heat. Also dust collection is a must. Poor dust collection and poor hold down ( vibration of your part) will kill a bit. Most cutter suppliers have a feed speed chart, but they don't really know what your are cutting. I hope this makes sense.
Bruce

[elcruisr]

Bruce, with his machine he can not feed fast enough to get anywhere near a proper chip load at 18,000 rpm. Most spindles on Shopbots can't turn any higher than that either. There's no point to a 22,000 or 24,000 rpm spindle at the feed speeds we can achieve with an Alpha much less a PRT!

[toolguy]

Eric,
The Porter Cable routers can turn between 10,000 and 21,000 Rpms. I agree that the Shopbot should not be run that high. I have an ELTE router on mine that I run at about 16,000. That wasn't really my point. My point was that there are so many different configurations of bits that you have some trial and error. Feed the bit until it chips out and then back off. I know dozens of people who feed too slow and get poor bit life. Of course there are times when you have to feed really slow. I know I use a lot of 1/8" bits. Most of my experience has been with larger routers like Komo, Weeke, Onsrud and biesse. Those machines are big, have 10 to 20 HP routers and run very fast. So I'm talking in general about bits. I'm always willing to learn what everybody else thinks, and this is a great forum. It's one of the reasons I bought a Shobot.
Bruce

[erniek]

So should I just run the PRT at maximum speed and keep reducing the spindle speed till something bad happens? Or should I stick with the 10,000 rpm and keep increasing the inches per second till it starts losing position? Then back it off a bit.

[toolguy]

Ernest,
No you should run your speed at whatever makes you happy. I'm a newbie with Shopbot. I'm just telling you how the bigger machines are run. I do not know the limits of the shopboot yet. I am however open to suggestion. I'm sure other shopbotters will have an opinion and it may differ from yours and mine.
Bruce

[elcruisr]

Hmmmm, I'm very familiar with big iron like Komo, FlexiCam, etc. Don't know of any operators worth their salt that take that approach. Most base their speeds on chip load, hold down issues and desired cycle times.

Do know of a few who think their $150,000 machines are a magic wand that doesn't require much knowledge to run and I out compete and outproduce them easy.

[erniek]

After dulling the first $75 bit with two sheets of melamine, my main concern it to get much longer life out of the cutter. I will try the single fluted compression bit on my next purchase. I tried cutting at 6" per sec/ two passes and found that the second pass doesn't always line up with the first in the X-axis, So I tried cutting at 3" per sec and jogging at 6" per sec and had the same problem. Next I tried cutting at 3" per sec and jogging at 4.5" per sec. No problems. Is the maximum cut speed going to change as the bit gets duller?

[toolguy]

Eric,
Ok you guys quit beating me up. I agree with your earlier post feed speed chip load hold down all are important.
Just for your info go to Courmatt International.com then to compression. I know this chart won't work for my ShopBot but they're using them for a guide line for some machines.
They also have listed a chip cutting formula.
Bruce

[erniek]

Got an email from Jamie at Shopbot.

He's suggesting 9000 rpm at 3 ips with the two flute cutter. Or get a single flute cutter at 15000 rpm.
He also mentioned that at 9000 rpm the spindle will have half the rated power.

Thank you Jamie

[jhicks]

I know it may sound strange but we have been running melimine for closets using Onsrud #56-451 which is a 5mm 2 V flute straight route bit or their O flute vesion 56-431.
Onsrud hasnt tried it but said of the 2 the v should work better with the V flute geometry so thats what were running but the O flute is cheaper and did work OK on the early tests.
These are technically specified as bits for hard and soft plastics or solid surface in te case of the -451.
So after these were suggested to us we tried them and were quite pleased with edge quality, dado's, shelf pin holes. The drill thru quality on the bottom does exhibit break out so cant run thru shelf holes but the ease of no bit change for all tool paths and the lower cost compared to compressions is a no bainer.
we are tracking wear and initially went thru one in 10 to 12 sheets but we were cutting a mix of 13 ply, 7 ply, and melimine with the same bit.
Now we have one bit for each material and are tracking life but easily we expect 10 to 20 sheets of melamine on a $25.00 bit which can be sharpened at least once for $3.00 and still deliver the tolerance for holes etc.
we have a PRT so its slower than you alpha folks but 13,000 rpm at 160 IPM/2.666IPS does the trick here with a modest vac hold down system of rigid shop vacs.
We were taking 2 passes but now take 3 for cut outs with max depth single pass for dados at .265 deep.
Something we didnt think would work well but glad we tried it.
Turn on, walk away, parts done with no bit change and ready to assemble.
Something you might want to consider.

Anyone drilling thru melamine with 5mm and getting no breakout? weve tried line boring bits, driil bits, and spoken to many suppliers all say. "oh yea, thats a tough one to do" and most say to offset the back and drill both sides vs trying to go thru.
if anyone has the magic formula, Id love to hear it.

[benchmark]

Quote:
Got an email from Jamie at Shopbot.

He's suggesting 9000 rpm at 3 ips with the two flute cutter. Or get a single flute cutter at 15000 rpm.
He also mentioned that at 9000 rpm the spindle will have half the rated power.

I was told that a spindle is rated full power down to 6500 rpm. ?

Who is correct ?

[thewoodcrafter]

I would think Jamie.
I have seem the graphs of RPM vers HP for a few brands of spindles and they do not develop full HP till they get up some RPM's, seems like 50% RPM and up.

[benchmark]

Hey Roger,

My Information came from Shopbot also.



Paul

[thewoodcrafter]

Paul,
It depends on the brand, HP and max RPM rating on the spindle. Find the manufacturers web site and see if they have the graph on your spindle.
These should be shipped with any spindle purchase, it is good information to have on hand.

[rhfurniture]

Power curves for different versions of my Firmec (similar HSD). The "off the shelf" version is curve 78.

8586

[erniek]

Well, I tried cutting at 9000 rpm single pass and 3 inches per second. I found that the PRT was losing position so went to two pass cutting.

I'm getting fibres sticking out from the edge that need to be sanded off by hand.

Jerry, That sounds interesting cutting with a straight 5 mm bit. Would you still use a 5mm if you had a second spindle?

[elcruisr]

You know, thinking back to when my machine ran PRT controls I think we decided that 2.1 inches/sec was about the most dependable speed when through cutting 3/4" stock without loosing position.

[bstern]

Hi Jerry,

What you need is a "through-hole-point" bit like the ones from Morris Wood Tools.
http://www.morriswoodtool.com/10mm.htm#Through%20Hole%20Point%2010mm%20Shank%20D rill,%20Style%2032M (http://www.morriswoodtool.com/10mm.htm#Through%20Hole%20Point%2010mm%20Shank%20D rill%2C%20Style%2032M)

Page down and you will find the ones I use on a 10mm shaft.

If you are running 10 to 12K RPM or up you can use a pretty fast plunge rate. Unfortunately I have them on an three headed 3300 RPM aggregate and use strategy of fast plunge till it hits the top of the material then slow to .2 ips for .25 inches then fast till you get to the bottom of material then slow again through the bottom. I get chip free holes using this strategy.

[jhicks]

Thanks Bob, we have tried those as well but maybe I'm missing something. Even with a brand new surfaced spoil board vacuumed down, we get break out with that bit.
Is there some other secret?
Our plunge rates at 12K or 13k RPM have been dialed from 20 to 40 IPS with no good results on that bit, brad point bits, or the 5mm.
We finalized 35 IPS as our plunge rate but wish we could dial in a good thru hole.
Any other tips are welcome.
Thanks

[bstern]

Hey Jerry,

I am getting great no chip results with those bits 3300 RPM and .2 IPS plunge.
Have you tried that slow?
That's one reason we had a 3 headed aggregate made to speed up our drilling.

[handh]

I'm thinking Jerry you are talking about 35 IPM instead of inches per second on the plunge. At 35 IPM that would be .58 IPS plunge which is still about twice the speed as Bob's suggestion. Hope my math is right.

Jeff

[jhicks]

Jeff, you are correct on IPS vs IPM, sorry but stand corrected. Thanks for the correction.
We'll try the reduction but in the past slower plunges started to burn the hole, bit, and melimine surface.
Will try again to dial down for improved results and let you know if we get there.
Thanks