[rdagger]

This is my 3rd sad attempt at milling pcb's. My first 2 looked like mashed potatoes. I'm using a Romaxx hs1 with a 60° vbit and I've been using millpcbs.com as a reference. I measured the runout on my Ryobi spindle at about .002. What steps should I take to address the whiskers?

[plasmator]

Is your spindle mount stable? Did you measure the spindle runout while mounted, or off the machine?

If everything is solid, you might play with different feeds and speeds.

[Kipper]

Is the cutter sharp....and turning in the right direction?

[rdagger]

The cutter is sharp and brand new although it is a cheap eBay purchase. I tried both a 60 and a 45. I assume the direction is correct because there is no way to change the direction on the Ryobi.

I measured the runout while the spindle was mounted on the machine. Is .002 bad?

The mount seems very solid. The Ryobi only has 1 speed but I will try to lower the feedrate.

[sch]

What rpm are you running the spindle at? Small bits need very high speeds.
For consideration, what sort of results would one get get running a 1" carbide
cutter at 20 rpm?

[rdagger]

My Ryobi TR45K only has 1 speed: 25,000 RPM at no load.

[chuck99z28]

Looks to me like its just too many ipm.
How fast are you traveling?
It looks like is just plowing through the copper.

[Jay C]

Not sure what you are etching into, but that doesn't look very level. What parameters are you using for bit size (assuming PCB-Gcode output). The bit isn't cutting the copper or PCB, it's tearing it. How old is the PCB material?

Also, the circles for the mounting holes don't look round. Do you have backlash in your axis? Have you successfully cut other materials?

[rdagger]

Here are my PCB-GCode settings:
isolation default .0001, maximum .0001, step size .006
etching tool size .005
z high .5, up .1, down -.005, drill depth -.07, drill dwell 1
Feed rates xy 20 ipm, z 10 ipm

I rushed home after work to try another pcb. I set the Mach3 feedrate to 20% instead of changing the values in PCB-GCode. I also bought some new PCB's. I was using old scraps for my first test. The results are better although it's still looking more like Picasso than a pcb. It got worse when I went to drill. It was going fine and then it just tore across the board.

[Jay C]

Try these settings:

Spot drill holes: -.005

Isolation
Default: .001
Maximum : .008
Step: .002

Tool size: .003

Z Down: -.003
XY Feed: 24
Z: 5 - too fast and you can snap the tip off of those V-Bits


Also, post a close -up/macro photo of the bit you are using ... the tip especially.

-Jay

[Jay C]

Oh, and post your G-Code so I can see what it looks like. That second photo looks like major backlash to me...the circles are horrid.

[rdagger]

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?

[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.