Page 1 of 3

downcut on plywood = fuzz

Posted: Tue Mar 08, 2016 3:56 am
by houndel
Hi!

My shapeoko3 is working like a hero since receiving a new controller: now I need to improve. Cuts in birch plywood have a very dense burr or fuzz where cut against the grain. I would love to get a better finish than this if possible. See image below:

Image

I'm using a new 1/8" down cut bit from ebay (drillman), feed rate 2500 mm/min, 24000rpm, 1.5mm stepdown. The program is set to conventional, not climb cut. The pocket has a profile cut at the end in the hope of cleaning it up- but as you can see it doesn't work when cutting against the grain.

Any suggestions on how to improve the cut?

Re: downcut on plywood = fuzz

Posted: Tue Mar 08, 2016 4:32 am
by WillAdams
Sharper endmill? (switch bits between roughing and finishing)
Leave less material for roughing clearance?
Change direction for finishing pass?
Spray finish and allow to dry between roughing and finishing?

Re: downcut on plywood = fuzz

Posted: Tue Mar 08, 2016 6:21 am
by DRobs86
I cut birch ply nearly every day. Im stuck at 30k rpm with my dw660. I usually go about 1300 mm per min at a 6.3mm depth of cut with an upcut. I usually just use a downcut if I want to run some engraving with the flat endmill, but I have just cut it profiles with it if I dont feel like changing

Why dont you try your 24k rpm with my feed and depth settings? Note that i dont have a shapeoko so use caution here.

Re: downcut on plywood = fuzz

Posted: Tue Mar 08, 2016 11:59 am
by Atonwa
If DRobs86 suggestions don't work here's another two things to try. I've found that all the birch ply I use is not created equal and I have more difficulty with the two big box stores than the cabinet shop and lumberyard I can get it at.

Option #1 and I'm sure you don't want to hear this is to look for the appropriate size compression bit that has downcut on the bottom and upcut on the top. This will give you the nice clean edge if you cut all the way through the plywood and the top surface will be mostly burr free. You'll have to take it in multiple passes.

Option #2 is using a 30 degree vbit to get through that top layer about .03 deep. Then change bits and proceed with the pocket. With the top surface broke and with a slight taper you won't get the edge burr. You will need to have homing switches to pick up your first starting reference point plus reset your z.

Unless you have a ton of plywood already I would also try picking up a piece from a true lumberyard and seeing the difference. Unless I'm in a hurry and they are closed its worth my time to pay a bit more per sheet for better stuff.

Re: downcut on plywood = fuzz

Posted: Tue Mar 08, 2016 12:42 pm
by Jimf
Some of the big box store ply is just really stringy. Had similar issues. Cleans up nice once you take a random orbit sander to it. I try to avoid the cheap ply but sometimes cost is a issue so I use it. I have to sand the faces anyway before paint so it isn't a that big of a issue for me.

Re: downcut on plywood = fuzz

Posted: Tue Mar 08, 2016 1:23 pm
by WillAdams
Another option is to use a chamfering or edge rounding plane or a file.

Re: downcut on plywood = fuzz

Posted: Wed Mar 09, 2016 2:20 am
by houndel
Thanks everyone for your suggestions.

I have just been sanding this off after cutting, but it would be great not to have to do this.

DRobs86 - will try your settings today. I've broken enough bits not to mind about doing it again :) The spindle I use is a 1.5kw chinese air cooled type from ebay, which so far is really solid with the option to change the RPM easily.

Atonwa - Thanks - I'll look into a compression cutter if I start doing more profile cuts. A friend who is a joiner recommended the same. Also will try the v bit method today.

Unfortunately this is the best ply I have found so far in Melbourne (AU), sourced from a cabinetry supplier. I might have to look around a bit more.

Will - I'll have a play with the direction of cuts and a couple of other endmills and post them.

Thanks again everyone!

Re: downcut on plywood = fuzz

Posted: Wed Mar 09, 2016 5:17 am
by houndel
A few tests to report back:

These were all cut at 1300mm/min, 24,000 RPM with a new 1/8" two flute upcut endmill.
https://dl.dropboxusercontent.com/u/34958944/6tests.JPG

Findings:

- Much better results, however my shapeoko 3 can only plunge 3mm - it jumps teeth even at 3mm depth.
- raster path works a lot better than offset to remove the pocket material.
- best settings seem to be ramp in to clear the pocket, with 0.5mm allowance for a spiral plunging profile path to clean up at the end. Both set a little faster at 1600mm/min to remove burning on entry. See below.

https://dl.dropboxusercontent.com/u/34958944/final.JPG

Still looks a little rough, and not a perfect profile but far less fuzz. The bit was probably a little dull by the time I got here from burning on entry when plunging at 700mm/min.

Re: downcut on plywood = fuzz

Posted: Wed Mar 09, 2016 11:36 am
by WillAdams
If you're having issues w/ the Z-axis, your belt-tension is probably too low.

http://www.shapeoko.com/wiki/index.php/Shapeoko_3#Belts

Re: downcut on plywood = fuzz

Posted: Wed Mar 09, 2016 6:41 pm
by Brian Stone
houndel wrote:A few tests to report back:

These were all cut at 1300mm/min, 24,000 RPM with a new 1/8" two flute upcut endmill.
I think that's too slow for the RPM. Consider the chip loading, assuming a 2-flute end mill: 1300/(24000*2) = 0.027 mm per flute... that's way too low. You should try targeting a chip load around 0.1 mm for a 1/8" end mill.

If you're using the Dewalt 611, drop the RPM to 16000 with dial set to 1. And bump your feed rate to 3000mm/min. That gives you a chip load of: 3000/(16000*2) = 0.09375 mm per flute. Use a modest step down of 0.5mm at first, and then increase the step down if you feel confident. Many fast-but-shallow passes are often preferable to a few slow-but-deep passes. It'll save your bits from dulling or breaking, and the reduced RPM will save your router.

Also, use Climb milling for this pocket to get the most cutting power for the money. There's no reason to use Conventional in this particular case.
- Much better results, however my shapeoko 3 can only plunge 3mm - it jumps teeth even at 3mm depth.
Are you jumping teeth or missing steps? If you really are jumping teeth, then your belt tension is too loose. If your motors are skipping steps when you push them hard, then could be your motor current is too low.