Calling all PCB CNC Milling Experts

[Qiaozhi]

I have just acquired (secondhand eBay purchase) a CNC3020T CNC router engraving machine. After struggling with the Chinglish User Manual (followed by lots of Googling) I've eventually figured out the tuning parameters for the stepper motors, and the Mach3 software is now successfully controlling the machine. However, I still have a number of questions that I hope some of you can answer:

The best software I've found for converting Gerber files to G-code is FlatCAM (version 7), but the same questions will apply to any program used to create the isolation paths. I found that LazyCAM makes a lot of mistakes, and often gets the pad sizes wrong.

1) What size (diameter) and shape engraving bit do you use to mill out the PCB?
2) How deep should the cut be? (i.e. cut Z.)
3) What feed rate is best?

Also, as a side issue - have any of you tried to engrave a key fob? The machine came with several plastic, and a few metal, key fobs. But so far, every attempt has ended in a mess. Presumably there's some simple free software available to do this?

[Koala]

hope this helps

[Qiaozhi]

hope this helps

Thanks.

I already know about the pcb g-code plug-in for Eagle, but I'm not using that software for PCB design. However, the information provided is still useful.

It appears that he uses a 15 thou (mil) flat end-mill instead of the usual angled isolation bit. The main advantages are that it removes the criticality of Z-level touch-off, and doesn't affect the trace widths. This seems to be a reasonable idea, and I think I may have some end-mill bits in the box.

Recommended track spacing for pcb milling are 16 thou spacing (using a 15 thou tool) with an 18 thou trace size. This is claimed to provide good results.

There are still some questions unanswered, so does anyone else have any input concerning the Z-depth and feed rate?
Also, if anyone actually owns a CNC2030T, then what parameters do you use?

[Altra]

I use Kcam to convert gerber to gcode. It's not perfect. I still have to go in and edit the gcode mostly the z axis.
Kcam is also fading due to the popularity of mach3 . The author hasn't done any updates for three years.

Here's a free one

http://www.ofitselfso.com/LineGrinder.php/


I bought this controller and software licence, but have not tried it yet. It does isolation conversions

http://www.planet-cnc.com/index.php?page=hardware

For cutters I use something like these
http://www.ebay.com/itm/10-Pcs-Flat-...item1e950d91f9

[greylourie]

Found this page with some mach3 info for his 3020.
http://www.planetpointy.co.uk/cnc-3020-adventures/

And another guy using emc2, plus other possibly interesting features he found like unlocking the software based spindle speed control.
http://www.planetpointy.co.uk/cnc-3020-adventures/

[Qiaozhi]

I use Kcam to convert gerber to gcode. It's not perfect. I still have to go in and edit the gcode mostly the z axis.
Kcam is also fading due to the popularity of mach3 . The author hasn't done any updates for three years.

That's a pity. I took a quick look at Kcam, and it seems fairly comprehensive.

Here's a free one

http://www.ofitselfso.com/LineGrinder.php/

Unfortunately some of the links on that page are broken, and the zip file containing the binary executable is corrupted. (Tried to decompress it on both Windows and Linux with the same error.)

I bought this controller and software licence, but have not tried it yet. It does isolation conversions

http://www.planet-cnc.com/index.php?page=hardware

This appears to be a potentially good solution to the old PC / parallel port issue.

For cutters I use something like these
http://www.ebay.com/itm/10-Pcs-Flat-...item1e950d91f9

These look exactly like the ones I have. 60 degree engraving bit with the same plastic case and blue sheath.

What I'm really interested in knowing, is what Z depth do you set in the G-code for the isolation routing? The default setting in FlatCAM is -0.002 thou (0.05mm), but this seems awfully tiny, and causes the bit to just skim over the surface. I did try the flat-end bit, but the result was not good. In the end I went back the engraving bit, and increased the Z depth to 5 thou (0.127 mm) with better results. Although I found that the depth of cut varied across the PCB, so I'll need to flatten the sacrificial (spoil) board.

[Qiaozhi]

Here's a free one

http://www.ofitselfso.com/LineGrinder.php/

That's a pity. I took a quick look at Kcam, and it seems fairly comprehensive.

Unfortunately some of the links on that page are broken, and the zip file containing the binary executable is corrupted. (Tried to decompress it on both Windows and Linux with the same error.)

Update: There is a slightly different URL than the one posted by Altra, which contains all the images and a good zip file. Here it is -> http://www.ofitselfso.com/LineGrinder/LineGrinder.php

[Qiaozhi]

Found this page with some mach3 info for his 3020.
http://www.planetpointy.co.uk/cnc-3020-adventures/

This guy's CNC machine is the same as mine. Even the front panel of the controller box is identical, but the rear panel is different. On mine, the 4 separate connectors are replaced by a Centronics-type.

Depending on which Chinglish User Manual you look at, the Ports and Pins settings seem to be different. The one in the above link actually does match my particular setup, although this is the first time I've seen numbers quoted for the Step Pulse and the Direction Pulse. The Mach3 default values are set to zero. Perhaps that's why the machine was going mental with the velocity at 1200 mm per min, and acceleration at 300 mm per min. In the end I reduced these values to 120 and 20 respectively. I'll report back later about what happens when I adjust the motor tuning to match the settings on planetpointy.com. One thing that seems odd though, is the Velocity setting range is shown as 1 to 5us, but the number entered is 10.

Examining his "Early PCB Attempt", I suspect he did two isolation passes on the board.

[Altra]

One trick you need to do. Is draw your traces and pads oversized, this compensates for what the cutter removes. Lets say a through hole resistor pad is 60mils. I make them 85-90 mils. In the "Early PCB Attempt" you can see the pads and trace are under sized. See attached photo of pid motor controller board, I made recently. Most of the pads were drawn at 90mils, but after cutting they are close normal.

[Qiaozhi]

For cutters I use something like these
http://www.ebay.com/itm/10-Pcs-Flat-...item1e950d91f9

In your link above, the photo shows a 60 degree engraving bit. But to me it looks like the tip has an angle of about 30 degrees. Also, in this youtube video -> http://www.youtube.com/watch?v=TYAfNTvgTak (very close to the start) it recommends using a 20 degree V-shaped bit. Clearly the angle does refer to the end of the bit.

So now I'm confused.

[Altra]

The Chinese sellers don't alway use the right photos.

If you look at post 7 in this thread. I uploaded a photo of the actual bit that I use.

http://www.geotech1.com/forums/showt...&highlight=cnc

Using a 20 degree bit may make sense because you can cut deeper than nessesary without making a wide cut.
Cutting deeper will compensate for low spots on the pcb. For $10 each you can buy a set 20 and a 60 degree.
While learning you will break a few bits, so it won't hurt to have extras.

I found that PCB material is not uniform in thickness, plus warping and bowing. So depth of cut is the biggest challange.

There are people working on different solutions, I am using a floating head spindle which is the best. But here are some software
solutions

http://www.cnczone.com/forums/pcb-mi...-software.html

http://www.youtube.com/watch?v=r-l7I...MH25g&index=27

Last, there are no rules, only Youtube and a few blogs. It is what ever method you make work.

[Qiaozhi]

The Chinese sellers don't alway use the right photos.

If you look at post 7 in this thread. I uploaded a photo of the actual bit that I use.

http://www.geotech1.com/forums/showt...&highlight=cnc

I sort of suspected that would be the answer.
And thanks ... I'd totally forgotten about that very interesting thread.

Using a 20 degree bit may make sense because you can cut deeper than nessesary without making a wide cut.
Cutting deeper will compensate for low spots on the pcb. For $10 each you can buy a set 20 and a 60 degree.
While learning you will break a few bits, so it won't hurt to have extras.

My engraving bits are 30 degree V-shaped, and I've eventually calculated all the necessary parameters for the CNC3020T machine. The result looks quite acceptable, and I didn't have to oversize any of the tracks or pads. The layout used 15 mil tracks and 10 mil spacing.

I found that PCB material is not uniform in thickness, plus warping and bowing. So depth of cut is the biggest challange.

Yes, I've found the same thing.

I'll post my calculations later.

[Altra]

My engraving bits are 30 degree V-shaped, and I've eventually calculated all the necessary parameters for the CNC3020T machine. The result looks quite acceptable, and I didn't have to oversize any of the tracks or pads. The layout used 15 mil tracks and 10 mil spacing.

In theory the software should calculate the tool offset. So drawing oversized traces and pads would not be necessary. I may have my tool diameter set wrong in Kcam, which is causing the under cutting. I've got my setup and method working so well, that I have not tweaked it lately. So it's time to take another look.

[Qiaozhi]

Typical copper clad board (1oz) has a copper thickness of 1.37 mil (35um) and a board thickness of 60 mil (1.5mm).
I have 30 degree V-shaped bits available.

Clearly, given a particular V-shaped bit, and a fixed copper thickness, there is a limit on the minimum isolation path width than can be achieved.

Using some simple trigonometry:

where , z = depth of cut, and

Hence, for a 30 degree V-shaped bit,

The minimum recommended space between copper features (for 1oz copper) is 3.5 mil (89um). In this case

Therefore:

In other words, you need to make a Z-cut of 6.53 mil to achieve an isolation path width of 3.5 mil.
A more practical value for the path width is 10 mil (0.39mm), which requires a Z-cut of 18.66 mil (0.73mm).

For a 60 degree V-shaped bit, the depth for 10 mil isolation is 8.66 mil (0.34mm).
Likewise, for a 20 degree bit, the figure is 28.36 mil (1.16 mm), which is getting close to the overall thickness of the PCB.

Conclusion: A 30 degree bit is preferred for general PCB milling, and provides the best control of isolation path width. A 20 degree bit would be better for finer features (such as SMD) if the router is up to the task.

For the CNC3020T machine, I have the Mach 3 tuning parameters set to 400 steps per mm, velocity at 120 mm per minute, acceleration at 30 mm/sec/sec, step pulse = 0us, and dir pulse = 0us. In the General Logic Configuration menu, Motion Mode is set to Exact Stop.

[Altra]

Your math is impressive.

I changed my tool diameter to 6 mils. I had it set too small. See attached photo of 44 tqfp test.