What causes whiskers

[chuck99z28]

If you're using the recent pcb g-code. It goes to the tool change z axis, before the tool change xy axis. That why it dragged over the board. You need to edit the code, find the place where it returns to zero for a trool change and change the order.

In pcb-gcode.ulp
At around like 276
rz(TOOL_CHANGE_POS_Z);
rxy(TOOL_CHANGE_POS_X, TOOL_CHANGE_POS_Y);

needs to be

rxy(TOOL_CHANGE_POS_X, TOOL_CHANGE_POS_Y);
rz(TOOL_CHANGE_POS_Z);

Its because you're your using z=0 as a tool change position.
Happens to me too.

[Jay C]

Here's the original code and a pic of the bit. I'll try your settings in the morning. If I change the tool change position z from 0 to .5, will that prevent my previous drill disaster?

I use 1" for my tool change position. Looking at the G-Code it's just a single line for each path. Looking at your results you have some combination of the following:
1. Severe run out at the spindle
2. Feed is too fast the bit isn't cutting it's tearing
3. Backlash the different thicknesses in your lines show the system is off in one direction. Multiple pass jobs would remove all of the copper.
4. The wrong etching bit. Copper is soft and tears, pulls, stretches.
So try these:
1. You said the runout is .002", that's half the width of your bit ... may want to double check that
2. Slow the feeds down to 10ipm or less to gauge any improvement
3. You need to do the square and circle test or use a DTI and check this in both axis. Have you cut anything else with this machine? Something is loose and it shows worse the smaller/finer you try to go.
4. You have an engraving bit meant for a different job. www.soigeneris.com has the Precise Bits without the high shipping or minimum order ... www.drewtronics.net has solid carbide V-bits that are very economical, but have a .001" tip and thus take more passes to get a wide isolation. I use them for tight SMD work which I haven't done in a while.

Also, I have run your gcode through an optimizer to shrink the amount of Z air moves.

-Jay

[Jay C]

If you're using the recent pcb g-code. It goes to the tool change z axis, before the tool change xy axis. That why it dragged over the board. You need to edit the code, find the place where it returns to zero for a trool change and change the order.

In pcb-gcode.ulp
At around like 276
rz(TOOL_CHANGE_POS_Z);
rxy(TOOL_CHANGE_POS_X, TOOL_CHANGE_POS_Y);

needs to be

rxy(TOOL_CHANGE_POS_X, TOOL_CHANGE_POS_Y);
rz(TOOL_CHANGE_POS_Z);

Its because you're your using z=0 as a tool change position.
Happens to me too.

Um, why would you do a tool change at zero??? At the very least if you are not going to change tools then set it to .01 Editing the code that outputs the Gcode is silly and will bite you one day.

[rdagger]

I took the Romaxx apart, cleaned and adjusted everything. I tried the new settings and it is worse now. I did some circle tests (5mm and 10mm radius) in pcb with the vbit and mdf with an end mill. They are not good. I also did another runout test on the vbit and it is much worse. If I'm reading it correctly, is it .006 (see pic)? btw I didn't zero the tester, the range is 1 to 1 the long way.

[Jay C]

Job one is to fix that backlash. I was under the assumption that the Romaxx didn't have any by design. Hopefully you are in contact with them or their Forum meambers to resolve that.

On a positive note, the edges of your copper look a lot cleaner

[eSilviu]

Here's the original code and a pic of the bit. I'll try your settings in the morning. If I change the tool change position z from 0 to .5, will that prevent my previous drill disaster?

could you send me the Eagle brd file?
I would like to try, and will post here the result

[rdagger]

I confirmed it is a hardware problem. The guys at Romaxx said they would fix it no charge even though the router is several years old. You can't beat that support.

[chuck99z28]

Um, why would you do a tool change at zero??? At the very least if you are not going to change tools then set it to .01 Editing the code that outputs the Gcode is silly and will bite you one day.

Off topic now sorry.
The tool change macro parks the spindle at zero on all three axis, I release the spindle and slide it up in the spindle mount, change the bit and slide it back down until the drill touches the surface of the work. Then restart the routine. I just use zero as the reference point, so I don't have to reset Z axis between every change.

[rdagger]

I finally got some time to work more on my PCB milling. The guys at Romaxx helped me fix the backlash issue (absolutely fantastic tech support). My last attempt is a big improvement considering I'm using cheap eBay engraving bits. I've ordered some proper bits from PreciseBits.com. I'm hoping to get even better results when I get them.

[Jay C]

I finally got some time to work more on my PCB milling. The guys at Romaxx helped me fix the backlash issue (absolutely fantastic tech support). My last attempt is a big improvement considering I'm using cheap eBay engraving bits. I've ordered some proper bits from PreciseBits.com. I'm hoping to get even better results when I get them.

It does look better, but the circles still look out of round to me. Did you have to send them your router for tuning?

[rdagger]

It does look better, but the circles still look out of round to me. Did you have to send them your router for tuning?

The circles I cut in wood look perfect. I'm not sure why those two 1/16" radius USB pads look a little off (It could be the cheap bits). I did end up sending them the router. I have one of their older machines and now it's like new.

[rdagger]

Here is my first real board. This is with 1 pass using a Think & Tinker 60° mechanical etching bit (.0050" tip). I leveled my MDF top and used carpet tape to hold the PCB. Here are my settings:
Default: 0.007
Maximum: 0.005
Step Size: 0.002
Etching Tool Size: 0.007
Z Down: -0.0045 (I'm using a sheet of paper above the PCB to zero the Z)
Feed Rates XY: 10
Feed Rates Z: 5

It's not perfect but the board works. I intentionally made the traces large. I'll try smaller on my next board. Thanks guys for all the help.