CNC Wood "Fuzzing" (Roughness) Problem

Hi,

I'm experiencing some bad "fuzzing" (roughness) when doing 2D profile cutting and need some advise.

Here's a run down on my setup and settings...

CNC: Probotix Fireball V90 - probostep motor upgrade, anti backlash nuts x/y drive nuts, 40V power supply upgrade, CNC USB software
Router: DeWalt DWP611 router
Collet: Precise Bits Dewalt 611 Precision-Grade Collet
Milling bit: Precise Bits - 1/8 in. dia. DeepReach 2-flute Fish-tail End-mill, 1.125 in. max DOC, 3.0 in. OAL (solid submicrograin carbide)
Dust collection: 1 HP Central Machinery (Harbor Freight) dust collector
Software settings: Pass depth 0.0625 in, feed rate 40 IPM, plunge rate 10 IPM
Router RPM: Appoximately 18-20k (setting 5 on the router, out of 6 speeds)
Wood: 13/16ths Poplar and Soft Maple

I am cutting the wood all the way through and leaving 4 thin tabs (one on each side) of the designs I am cutting. I started with poplar and then heard maple doesn't "fuzz" like poplar and has a tighter grain, so I tried some soft maple, but then experienced the same results. I've also tried changing the router RPM and feed rate with the same results.

I am wondering if I need to try some "rock" maple (hard maple) or another type of wood? Perhaps it is still possible to mill poplar or soft maple with different settings and not experience fuzzing? I have also questioned changing to a 2 HP dust collector as I noticed my 1 HP dust collector doesn't quite get all of the dust and chips. Could it be dust and chips left in the path of the passes that is causing the bit to mill like this? Am I using the wrong type of bit for the type of wood and cutting I am doing? Any other ideas for what could be causing this? Any ideas or suggestions would be greatly appreciated! I'm not sure what to try next.

I'm also attaching some photos so you can see what I'm talking about.

Thanks!

Dustin

Attachment 223520

Attachment 223522

Attachment 223524

Attachment 223526

Attachment 223528

That roughness is not what I would call fuzziness. It's just a poor finish.

I route a lot of poplar, and it's the worst cutting wood I've ever routed. It's very difficult to get a good finish. Especially on end grain, which all of your pictures appear to be.

From my experience, the harder the wood, the better the finish. I've cut poplar that varied in density where half the cut was perfect, and the other half looked like yours. Here's a few things to do to get better results, but your fighting a losing battle.


1) Use a razor sharp bit at all times. My guess is that your .0625 deep passes have dulled the tip of your tool, and you're always cutting with the dullest portion. While your machine is probably not very rigid, your slow feedrate and high rpm are only contributing to dulling the tool. You should be ramping in rather than plunging, but there's no need to ever go 10ipm in wood. With 1/16" passes, you should be plunging at 50ipm and cutting at 100 ipm. However, if the tool is not very sharp, higher speeds could make the cut worse. But with a sharp, new tool, higher feedrates will keep it sharp longer.

2) Use downcut spirals, rather than upcut. Upcut bits tend to tear the wood more than downcuts, and usually give a slightly better finish. This is especially true on a wood like hard maple, where upcut bits can tear out large chunks along the grain. The downside here is that downcut bits don't like deep cuts, so you need to keep the chips clear. Compressed air works well for this.

3) Use a finish pass. Cut your parts .01-.02 oversize, and finish with a single full depth pass at reduced rpm. This will clean up your part with the mostly unused upper portion if the bit, and removing a small amount will give a much better finish.

But again, with poplar, you may not be able to get the results you're looking for. Especially on end grain.
You might also try looking for 1/8" shank bits on Ebay. You can get very high quality bits similar to the ones you're using for between $3-$7 each.

Hi Gerry,

Thank you for your reply and the great tips, I really appreciate it!

I'll try increasing the feed rate and plunge rate. Do you think the pass depth of 0.0625" is okay for a 1/8" dia. bit? I was told I could go up to 0.125" on the pass depth, but I figured 0.0625" would be easier on the bit. A full depth finishing pass sounds like a good idea too. I'll give that a shot. I know you mentioned using a lower RPM for that, but would you also recommend a lower feed rate too?

I've also heard a downcut spiral bit could be good to try, but I haven't been able to locate a good source for a 1/8" dia. downcut spiral bit with a DOC of at least 1" (since I'm cutting 13/16" wood. I'll do some more eBay searching. Do you have any links you could point me towards?

In all of my experimenting with milling poplar I think you are right... I don't know even with the best milling settings if I could really get a smooth finish. I've been doing cleanup with a dremel tool and a sanding band, but I have to do a LOT of cleanup. I would prefer to only have to do a little (if any at all). That's why I tried the soft maple, but I am having the same problems with it too. The photos I took are actually of a design milled from soft maple. It does sound like milling a hard wood would be a better bet. I am considering trying "rock" maple (hard maple) next. Is there any other wood you would recommend that is clean (mostly free of knots) and nice grain like poplar and maple, but that is a harder wood that would give me nice smooth sides on 2D profile cutting?

Thanks again,

Dustin

Actually, I meant to say reduced feedrate, not rpm. Yes, you can cut 1/8" deep per pass, provided it doesn't cause the machine to flex.

Personally, I wouldn't try to cut that deep with a 1/8" bit. I don't know if you'd be able to find a downcut that long. Thinking about it, a downcut may not make much difference with that small of a bit. The larger the bit, though, the bigger the difference you'll see.

You might want to try birch.

Use sharper endmills. I use G. W. Schultz carbide end mills which are razor sharp and I get fantastic finishes even though I'm not running them at the kind of RPMs they should be run at in wood. My most common cut is in guitar bodies, making a 7/8" deep cut with a 1/2" 2 or 3 flute high helix GW Schultz solid carbide end mill. I make this 7/8" deep cut in ONE pass, at 3000 RPM, cranking the mill handwheels (manual mill) just about as fast as I can. The finished surface is almost polished.


The OTHER brand of end mills I've tried that work just as well are the Ultratool brand.

I've found from experience that if you can get the end mill with a Zirconium Nitride coating, then it lasts a lot longer. And with the abrasive nature of wood, it's really important to get the coated version. On an uncoated end mill, I can only rout two guitar bodies before the edge quality has degraded to the point where the end mill is now not good enough for wood but it's still great for aluminum.

With the ZrN coating, cutter life for wood application is greatly enhanced. How much? I don't know. I have yet to replace that cutter and it's been five bodies cut so far.

I make a variety of Solid Body electric guitars.
My profile cut is .125 deep per pass with a .375 EM.
I'll cut Poplar, walnut, maple...
Doesn't really matter what wood.
But sharp tools and dry wood are the keys!
I think that skinny bit on a contour cut isn't quite right.
I'm cutting 1.75" stock


Sent from my iPhone using Tapatalk

You're never going to get a smooth finish on a contoured surface like that with a "fishtail" endmill. That's basically a flat-ended bit; what you need is a ball-nose bit. I think you can probably use a much bigger diameter; at least 1/4".

Hey read below

I just ran some black walnut and I used a .375 2 flute endmill. Perfect cut!
I use a .125 drop on each pass, which is proably too small, but it comes out so fine all I need is a light sanding.

Can you change up to a larger bit? Maybe the diameter is so small that it tears rather than shaves.

Quote:

---

Originally Posted by dustincowell

Hi,

I'm experiencing some bad "fuzzing" (roughness) when doing 2D profile cutting and need some advise.

Here's a run down on my setup and settings...

CNC: Probotix Fireball V90 - probostep motor upgrade, anti backlash nuts x/y drive nuts, 40V power supply upgrade, CNC USB software
Router: DeWalt DWP611 router
Collet: Precise Bits Dewalt 611 Precision-Grade Collet
Milling bit: Precise Bits - 1/8 in. dia. DeepReach 2-flute Fish-tail End-mill, 1.125 in. max DOC, 3.0 in. OAL (solid submicrograin carbide)
Dust collection: 1 HP Central Machinery (Harbor Freight) dust collector
Software settings: Pass depth 0.0625 in, feed rate 40 IPM, plunge rate 10 IPM
Router RPM: Appoximately 18-20k (setting 5 on the router, out of 6 speeds)
Wood: 13/16ths Poplar and Soft Maple

I am cutting the wood all the way through and leaving 4 thin tabs (one on each side) of the designs I am cutting. I started with poplar and then heard maple doesn't "fuzz" like poplar and has a tighter grain, so I tried some soft maple, but then experienced the same results. I've also tried changing the router RPM and feed rate with the same results.

I am wondering if I need to try some "rock" maple (hard maple) or another type of wood? Perhaps it is still possible to mill poplar or soft maple with different settings and not experience fuzzing? I have also questioned changing to a 2 HP dust collector as I noticed my 1 HP dust collector doesn't quite get all of the dust and chips. Could it be dust and chips left in the path of the passes that is causing the bit to mill like this? Am I using the wrong type of bit for the type of wood and cutting I am doing? Any other ideas for what could be causing this? Any ideas or suggestions would be greatly appreciated! I'm not sure what to try next.

I'm also attaching some photos so you can see what I'm talking about.

Thanks!

Dustin

Attachment 223520

Attachment 223522

Attachment 223524

Attachment 223526

Attachment 223528

---

I get absolutely perfect, totally fuzz-free cuts in maple and mahogany by using G.W. Schultz 1/2" carbide end mills, 2 and 3 flute categories.
I run them in my manual Bridgeport clone at anything up to the max RPM the spindle will go to, which in this case is about 3K. I take up to full 1/2" width
cuts in hard maple at depths of cut as much as 1/2". At less aggressive cuts I can of course make deeper (Z axis) cuts. Finishing passes of .1 inch at full depth of cut
are amazingly smooth and easy. Always read the grain of the wood and cut appropriately. Never permit the cutter to be prying chips up and out of the workpiece as this
will lead to chunks being knocked out. This isn't metal, and must not be cut like metal.

MOST common end mills are NOT sharp enough for wood. This is why I specify G.W. Schultz carbide and also the Ultratool brand. They are two I have found
that give the required cut surface characteristics.

http://www.practicalmachinist.com/vb...limb_conv1.jpg

You WANT to climb mill when it comes to milling wood.

- - - Updated - - -

Attachment 266326

use two toolpath as Gerry mentioned..

the first make as climb milling, and leave really just a little on climbmilling don't chips the wood..

at finish pass use the conventional and that little pass wont pull the splinters out..

the reason for this because the first climbing pass will ""bend"" fibers ... as you go against these fibers with the finish that will smooth it out..
otherwise you get fuzzy always, you can find it when you stain or make wet a little the surface..
only way avoid fuzzy if oyu could go as you sharp pencil.. always down on grains.. of course it is not possible in the practical life.. but you can greatly minimize..

another thing is , those diagonal marks shows your bit also was resonating.. that also makes worst..

The finish quality shown in those pictures tells me that your cutter is nowhere near sharp enough for wood. Do as I suggested, get GOOD cutters like the ones I mentioned,
and your quality of cut will instantly become far better.

Here's an example of my own work. Actually there was no finish pass made at all. Not on the pickup cavities. It's cut to spec in the minimum number of cuts possible.

Attachment 266390

On mine i am using a brand new white side upcut bit and the surface of my peices just fuzes up on one side and looks really nasty even though it scrapes right off. I am using a random direction, cutting speed, and RPM if that makes a differenct. any advice?