Help please, shallow DOC sucks noodles... LOTS OF PICS!

[Propaganda]

OK, so when I set a DOC at .008" the copper burrs like a guy from the Tropic of Cancer when he is in the Arctic. WTF. See picture #1.

My specs...

Router - 20K, 5 mils of runout
Feed - 15 IPM
Bits - V carve carbide, 60 or 20 degrees - examples on eBay
Material - FR4 .05oz

Now when I do a DOC of .020" no burrs form and the results are fantastic. Picture #2, 5, 6, 7

However, I need to mill a board with thin and tight traces. Picture #3, 4


The copper clad is bolted down to a piece of MDF from there I can raise and lower the corners until the clad is flat to about .003ish. Sometimes I can see a bow (a lift) in the clad, but that does not effect the results seemingly.

The only thing I can think of is ditching the china bits and going with a drewtronics bit. IDK, Do you guys have and advice for about how to get those darn little burrs from forming so I can use a shallow DOC of .008"ish.

-Str

[powerr]

yes i would try different bits. i have heard good things about drewtronics but have yet to try them. i use precisebits 60 and 90 degree bits using .035 to .025 doc.
what kind of machine are you using? does it vibrate bad when the machine is running? did you measure runout with router running? the only reason i ask is when i was dialing my machine in, the gib was loose on the x axis causing vibration and ended up with traces that look like that.

Rob

you making a wireless RGB controller?

[Propaganda]

Run out was measured by turning the spindle manually. There is an attached picture of the machine I am running. It's decently solid, but I will heed your experience and recheck the bearings, etc for stiffness.

Now, that I sat in my chair watching Futurama for a few minutes I remembered when I cut some MDF the other day and I had odd results, so more than likely the machine needs cleaned and tightened up.

you making a wireless RGB controller?

Yes, yes I am. Good eye on that.

[neilw20]

It looks like the tip of your cutter is moving around when not supported deeply in the material.
1. Is the tip perfectly sharp?
2. Can you get less overhang on the cutter?
3. Try a slower feedrate.

[M250cnc]

You may have the tip of the cutter overloaded with the copper at a shallow depth.

Copper is a very gummy material.

Cure is a V bit or very shallow slow ramp in maybe with cutting oil smeared on board with a depth of cut at least double the copper thickness

To prove, check thickness of of board with and without copper if copper is 0.008 thick then that is the likely cause.

Phil

[Jay C]

If you want to try the Precise Bits, avoid the minimum shipping fee and buy them from Jeff at www.soigeneris.com I started with the Drewtronics bits and they work great, but I liek that the PB have a stop collar that allows me to swap bits without having to touch off for etching, drilling, and then milling.

-Jay

[powerr]

Hello propaganda. your machine looks fairly solid from what can be seen. i know it sounds kinda scary but recheck your run out with the router running. it may be introducing some vibration at full speed.

I like playing with rgb led and dmx stuff my self. when i saw your board that was the only thing i could think of.

Rob

[eSilviu]

OK, so when I set a DOC at .008" the copper burrs like a guy from the Tropic of Cancer when he is in the Arctic. WTF. See picture #1.

My specs...

Router - 20K, 5 mils of runout
Feed - 15 IPM
Bits - V carve carbide, 60 or 20 degrees - examples on eBay
Material - FR4 .05oz

Now when I do a DOC of .020" no burrs form and the results are fantastic. Picture #2, 5, 6, 7

However, I need to mill a board with thin and tight traces. Picture #3, 4


The copper clad is bolted down to a piece of MDF from there I can raise and lower the corners until the clad is flat to about .003ish. Sometimes I can see a bow (a lift) in the clad, but that does not effect the results seemingly.

The only thing I can think of is ditching the china bits and going with a drewtronics bit. IDK, Do you guys have and advice for about how to get those darn little burrs from forming so I can use a shallow DOC of .008"ish.

-Str

I use the same bits as you (cheap chinese V bits) with a cheap dremmel (russian) clone. Generally, my results are better than yours, and only a few are worse.
In my case:
1. rotating the bit in collet helps to get clear cuts (some trial and error before starting the real PCB are needed)
2. 15krpm, and 250mm/min offer best results
3. FR4 fiberglass + epoxy is the worst PCB I ever milled. I prefer other cheap PCB based on resin and paper. Chinese V bit will be used in about 2 meters of linear mill (based on my experience)
4. 0.1 to 0.15mm deep makes a good cut. Yours seem like 0.2mm - too dip
5. used V bits are resharpened to wider diameter with a simple diamond file.

[Propaganda]

thanks guys for the tips I will them out.

Can you get less overhang on the cutter?

what does that mean?


Using oil did not help, although it did cut down of dust.

I clamped down a dial gauge to the table and the other to the side of the router and there was about .001" or less of movement due to vibration of the router. IDK is that good?

In the mean time I was lucky to have had a 10 degree cutter so I ran that so I can move along with my electronics project. The pic is the result. I still had to cut .015" deep. And the very tip did break and I had to retouch off in the middle of milling. The result came out great. However, I will still try those tips in for future projects, I know I can get it right.

[BobWarfield]

You know one thing that's kind of interesting about this kind of cutting is the effective diameter varies with the depth of cut, just like with a ballnosed endmill.

Just for kicks, I plugged in the two depths in my G-Wizard calculator as though we were using a 2 flute endmill instead of a 60 degree engraving cutter.

When you are cutting at 0.008" depth of cut, the effective diameter (which you can figure out with the Chamfer tool in G-Wizard) is only 0.0092 for a 60 degree tool. So if we plug that in with a 0.008" depth of cut and a 0.0092" width of cut on a 0.0092" diameter 2 flute endmill, cutting in copper, it wants all of 20K rpm and more, and a feedrate on the order of 8 or 9 IPM.

Now if you plug in that deeper 0.020" cut, your effective cutter diameter is now 0.023. So after plugging in those parameters we get a 20 IPM recommended feedrate, which is a heck of a lot closer to the 15 IPM that you're using.

Just sayin'

It'd be interesting to slow down to 8 IPM with the shallower cut and see how that works.

Cheers,

BW

[powerr]

i would try some different bits. I like the precise bits 60 and 90 degree bits.
.001 should not be that bad. the also make precision collets for routers might want to check them out.

Rob

[Propaganda]

Those calculations are rather interesting. I think at on time I did a feed of 8IPM, but silly me I did not document my experiments this time around. sigh

The next board I run will be a revision of the board I just milled, prob in a few weeks. So that will give me time to tighten up the machine. Also, I think I am going to make a vacuum jig to eliminate that .008" rise in the middle of the board, which is necessary when I am able to mill .008ish deep.

You know what, I do have the precise collect set, and even with that I get a runout of .005"!