Using a Cheap Desktop CNC With 2.5W Laser for PCB Drilling and Milling Capabilities

Hi
I've taken the plunge / route (apologies) and obtained a cheap desktop CNC machine (very cheap). Yes I know all the negatives that will be forthcoming, perhaps deservedly, but at the price I paid which unbeknown at the time included a 2.5W Laser, I can at the very least automate my Christmas card list with aplomb. If only I had a pet shark...... (Austin Powers is on....)

Following on from associated posts regarding PCB construction vs China, I do have the capabilities to chemically create boards with relative ease, but hand drilling is not too much fun. From reviews I am under the hopeful impression that I can feed in the necessary file(s) and have it drill for me. Reviews also suggest that it can mill PCBs too, but whether or not it can to any useful extent, and I have no reason to disbelieve the +/- reviews on such, all I really care about is drilling as far as PCBs go (but seriously contemplating getting a shark as a secondary purpose).

I'm also hopeful that once I figure it all out I can route/cut holes in plastic to accommodate switches / buttons / displays / anything not requiring a simple drill bit. Again nothing suggests this is outside its comfort zone. Clearly at the price it has limitations which may prove to be insurmountable but at worst you can expect a burned balsa card come December.

It is in kit form, arrived well packed and gives a very, very good first impression.
If anyone is interested in how this progresses, perhaps to landfill, I'm more than happy to document the good and bad with pictures where appropriate.

I'm in a win/win situation though. As a total novice in CNC-ing, even if it does end up in landfill I expect to break even as it will have kept me out of the pub for an appropriate cost..

RegardsPSNo. 6 on leader board..yes!Once I automate my creative abilities and have my automatons build more automatons watch out! Have fun whilst you still can.

That's interesting to read, can you post a link to the kit that you purchased? A photo or two would be interesting and I would be keen to see how well it performs once you have carried out some trials.  The only CNC machine I've been involved with was 12' high and could machine the engine block for a passenger liner!
Don't forget that from the April issue (published next month) we revert to our maiden magazine title of 'Practical Electronics' and the current (March) issue is the final one for EPE.

Hi AlanI'm a subscriber so I won't miss an issue. Will miss the name though.....I built the machine today, which was pretty straight forward but there are a couple of things to watch out for. I'll document in another post along with details of where I bought etc.
I haven't installed the software but using the hand held controller I confirmed all axis and spindle works. That's a good start methinks.Regards

HiI bought my machine herehttps://www.amazon.co.uk/Upgrade-Version-Engraver-Controller-Extension/dp/B07GJBY9DT/ref=pd_sbs_60_3/261-9169228-7267153?_encoding=UTF8&pd_rd_i=B07GJBY9DT&pd_rd_r=35480709-3a78-11e9-8ff4-4bd596040a30&pd_rd_w=Knjmc&pd_rd_wg=fEtmk&pf_rd_p=18edf98b-139a-41ee-bb40-d725dd59d1d3&pf_rd_r=CVGAK5ZPR58VNTY0JNT3&psc=1&refRID=CVGAK5ZPR58VNTY0JNT3The review at the bottom was a strong deciding factor for me and is quite accurate. I would add to that the following (based on my experience):It is very well packaged and it will take much longer than twenty minutes to assemble.
The instruction sheet provides a link to my.pcloud.com to download software etc. Many similar products there but after downloading all things relevant I discovered they were all pretty much the same.When assembling the table mounts on to the runners, be careful and align the mounts correctly on the runners (mounting holes to the outside edges). Guess who didn't and had to disassemble the base to rectify. Also, insert the T-nuts for the vertical pillars before completing the base.I agree completely that you should go to Screwfix or similar and obtain M5 x 16mm Cap Heads for attaching the table to mounts. If not, have fun.....I too had issue in mounting the X-Axis motor. If doing this again I would first check and adjust the mounting holes before doing anything else. I had to widen all holes with a 3mm bit and "wiggle", with one hole needing quite a bit of "adjustment".The controller board doesn't have any cover. I will probably put it in a box or the like at some point. Three stick on heatsinks were provided but no instructions as to where they should go, but this is rather obvious. If in doubt use your grounded fingers to find out..<s>
The wiring from board to motors is connectorised and whilst they supplied ty-wraps to keep things neat, I preferred to use spiral wrap as this makes a far better job.It comes with a hand held controller which seems to be Arduino based. It can control the mill manually and load files from a Micro-SD card (supplied). The controller board can connect to a PC to be controlled by the supplied software but I haven't got around to that yet.
I haven't tried the Laser module which came with protective glasses (awaiting delivery of a shark), but I clamped an old bit of PCB and using the hand controller and supplied bit, I lowered the bit until it just touched the surface, lowered a further "0.1" on the Z-axis then moved about a centimeter back / right / forward / left and ended up back where I started. Without stopping I did the same again and it went over the previous trace. No competing trace so that suggests to me repeatability.I wish to stress that I am completely new to any form of CNC activity and I appreciate I have a lot to learn regarding such. The supplied documentation for the software is not what you could call comprehensive but it does provide a starting point.
Next thing, now that it works, is to remove each bolt in turn and coat with blue Loctite.
I am impressed with it, especially considering the price, and I think it will earn it's keep. Since obtaining it I have saved about a third of the purchase price already by staying away from the pub..<s>

Pictures during construction. Note that whilst I have "workshop" facilities I chose to build this on a table as I figured most hobbyists would do so. No special tools were needed as all keys were supplied, but a decent set-square is recommended.

HiThis morning I tried to connect to a PC...
It's a good job we all consider messing with anything even slightly technical fun...The "supplied" software consisted of:-CH340 Driver - This chip is known to be a bit temperamental (focus on mental) at timesCandle 1.1.7 - This is the software to control the CNCLaserGRBL2.9 - This is the software to control the Laser cutterAlso included was Xloader to update the controller board to "latest" if required. Documentation suggested that the controller needed to be updated to work with the version of Candle supplied but there didn't seem any way to establish what was already installed.
Installed the driver which seemed to have no issues. I then ran Candle and after selecting the correct Com Port (in my case Com 3) the software did appear to acknowledge such but I could not connect nor control.I took this as a sign that I needed to update.Running Xloader and following instructions I attempted to upload the Hex. This failed and Xloader just hung. I tried a few times, even swapping the supplied USB lead for a known good one but I couldn't get either Xloader nor Candle to talk.
I discovered the console window in Candle (which was minimised) partially hidden by the "jog" controls. Jog allows you to move the bit x/y/z manually. Opening this up I could see the responses which indicated that Candle could not communicate with the CNC board.I searched for an updated CH340 Driver but Windows told me I had the latest installed. Searching around the web indicated that I have the latest everything, however I could not connect.I found the reason, which isn't documented anywhere I looked. The CNC comes with a hand held controller that allows you to manually control the CNC and you can even load a file with it using it's MicroSD. This is a good thing as milling machines have a habit of making a bit of a mess in operation and I personally would not want my laptop too near one depending on what it is doing at the time.If the hand held controller is plugged in, then your PC will not connect. Once I unplugged, Xloader ran first time and when I ran Candle it connected straight away. I can now control the CNC with the supplied software.In my searches it appears that the controller board and everything to do with the CNC is quite generic and open source, which I like as I can change anything I wish if I want to.
I'm going to look for software to convert Gerber to G-code, and there are a fair few choices out there. If anyone can recommend anything I'm happy to try.I have certainly learned a lot messing with this and confidence in the machine is still high. Of course I haven't actually done anything with it yet and I cannot comment on reliability, but as mentioned earlier a lot seems generic so I'm sure if I blow something up getting spares / replacements won't be too hard.A couple of things I didn't mention earlier. The supplied mains lead is a US style plug with adapters for UK/EU. It is a generic figure-8 lead and I binned mine and used one I had already fitted with a proper UK fused plug.
Whilst pretty much everything is included to get you up and running, spanners to tighten / loosen the collett are not included but everyone will have suitable ones in their toolboxes.It came with 10 x 20-degree V-Cut bits. These are very sharp and can be slightly tricky to remove from their case. I'm sure you can guess how I know these are very sharp....Regards

HiHuge smile on my face.Today I did my first test on a PCB and I call it a success.First off, creating G-code from Gerber proved a bit tricky. I obtained various bits of software off of the web. Some seemed to generate the code, some looked like it would mill the way I wished but holes didn't line up, some just didn't run. Possibly a lot of this was my fault or PC fault.However TINA which is one of the programs I use, does have an option to generate G-code but being a complete novice re CNC it was very much trial and error. I had created a test circuit in TINA about 5cm square. Not wanting to damage anything or inadvertently set it to do something it didn't like, I set it so that the X/Y zero was near the corner of my scrap PCB and the Z zero a mill or so above. Settings for both milling and drilling would, I hope, do little more than trace out where things would go rather than proper milling / drilling.Armed with the supplied 20 degree V-cut, within a few minutes my board was done. A clear mill had been produced with holes exactly where they should be (well had I a drill in the chuck and had I set it to properly mill / drill).Based on this I have confidence that this cheap machine will mill / drill PCBs to meet my needs and I have no doubt it will make swift work of any cases I wish to attack. I prototype mainly with THD with a smattering of SMD so I am unlikely to be able to comment on milling out tracks for TQFP or the like so I can't say if it would be suitable for that, but for me and my needs this will easily drill holes for boards I have chemically produced or mill / drill the PCB for me.No idea about reliability yet...I hope this is of interest.Regards

Chip, you said "If anyone is interested in how this progresses, perhaps to landfill, I'm more than happy to document the good and bad with pictures where appropriate. "You've already pretty much done that here, but I'll get Max to contact you about expanding it into a full article.  As one who has always made his PCBs the old smelly way, and spent hours drilling holes (in most of the boards, anyway) I'd seriously look at getting something like this.  Many thanks for posting.  

Hi DavidThe above are just comments on my progress, but I would be happy to produce a document if there is interest to include things to check / rectify first (happily not a lot really). I did take photographs at every stage.
Things I'm learning now are track width versus depth of cut. If using V-cut blades  then the deeper you mill then the wider the cut (at surface) and if your track width is too narrow / cut too deep then you run the risk of milling into your track. In my initial PCB test I didn't care about that, I just wanted to see if it would follow instructions and how well. I was clearly cutting too deep in my test but I stress that I had not set anything up to anything but a guess as I just was eager to see if it would follow the code created and it did.
A friend of mine does know a lot about CNC and I'm hoping he can advise on which is the most suitable bit for which application I'm likely to encounter, and to also recommend suitable spindle speed / feed rates. I see a lot of experimentation coming up
This won't allow you to take a block of metal and turn it into the engine for the QE2, but for the "light cutting" use as I intend and also for engraving front panels then so far it appears more than capable.Biggest pain other than X-axis motor and table mounting was software. I have a few PCB design applications (TINA produces workable G-code) but I have been trying lots of other freeware to convert Gerber to G-code with limited success. One application likes the Gerber from one design package but can't cope at all with that from another. Guess who tried the problematic package first..... That was a few hours kept away from beer so my actual cost of this machine is rapidly falling..
Regards

HiI'm glad there is never anything on TV as it allows me time to scour the web for software and play.CNC machines use G-Code to control the machine and unless your software produces such directly then you will need software to convert your Gerber (or DXF/SVG) to G-Code.Currently I'm trying out the following free software I've found, and this list of available software is no means exhaustive.PCBConverterFlatCAMCarbide3D - Note that this is a free web service offered by Carbide 3DInkScape - Note this is a graphics program that can save in many formats including  SVG / DXF. I will possibly use this for engraving front panels or such like. Save as SVG/DXF then convert to G-Code with FlatCAM or some other software
Once I start producing working G-Code I'll then experiment with the type of bits and depths etc.Regards

HiJust discovered Inkscape can export directly to G-code.Attached is a very quick and rough picture on some scrap PCB (non copper side) using a non standard font. Please note that I have not yet figured out best settings etc, this and previous are just play time. Since engraving this I washed the board and cleared away the swarf which left a much smoother trace than shown.
Regards

HiToday I created a simple schematic in TINA and exported as G-code. The board is about an inch square and was cut into a piece of scrap PCB that I've been messing with. The component in the middle / bottom is an 8-pin DIP and the whole thing took a couple of minutes to mill. Note that I did not ask it to drill any holes as I didn't have any wasteboard underneath.
Bear in mind that this is really my first attempt at milling so I am finding my feet but thought it quite encouraging.I used the supplied 0.1mm 20-degree V-cutterTrack width and pads in TINA were as my default (off hand 0.5mm tracks I think).It isn't perfect, but a good first attempt.Where the copper isn't milled all the way through could be due to a number of factors including uneven thickness of copper, board not flat, board flexing (possibly due to clamps) or even just depth of cut.I believe the controller board can accept Z-probing which would help to eliminate the above but I haven't explored that yet. Probably will once I gain more confidence in it's use.
With a bit more experimentation I'm sure this will meet my needs
If there is a more fun way to waste a Thursday lunchtime I don't know of it.Regards

FYIThe PCB layout it came from

HiRather than keep using that scabby bit of PCB that's been hanging around my garage for ages I did the following tests on a shiny new piece. The "clamps" that came with the CNC are just bolts with a large square washer and wing-nut, that slot into the table. In these tests I used mini-C-channel cut and drilled appropriately that holds the PCB firmly along two sides without interfering with the machine
First test was with a 0.1mm 20 Degree V-cutSecond was with a 0.1mm 45 Degree V-cutThird test was with a 0.8mm End MillTrack widths were 0.5mm and pads were default size for the component. Mill depth was 0.09mm. Again I didn't ask it to drill as I know that's no issue.
Apologies for the picture quality, my wobbly hand.As you can see the V-cuts were quite successful but the end mill needs a lot more work. It chomped it's way through all it met <s> I think the depth of 0.09mm was a tad deep as in places the track width when cut with the V-cut's gets a bit thin. Perhaps 0.08 or 0.085mm would be the ideal depth. Typically for the PCBs I use the copper layer is only around 0.03 - 0.04mm thick, so the deeper the V-cuts the wider the gap at surface level which could eat into the track. Settings can negate this though.
I am sure if I tweak settings, track width versus depth of cut etc then things will improve, but for now, for my needs it looks like the 0.1mm 20 Degree V-cut will meet my milling needs, cutting to a depth of 0.08mm with a 0.5mm track width.Note the above was all done with TINA exporting the G-code directly. If converting Gerber to G-code I may get different results.I'm 100% sure that this "cheap" CNC will drill all I ask of it and I'm pretty sure that for my PCB needs it will mill too. Rarely do I need exceptionally thin tracks which this CNC may struggle to mill, but if I do I still have my etching capabilities for such.
If I were to chemically produce these test PCB's, from deciding that what was on my PC is good to being ready for drilling, by the time I printed on to transparency, exposed and etched etc it would have realistically taken me an hour anyway. This took two and a half minutes to get to the same stage with no messing around with chemicals. I concede that the chemical process would be pretty much any size and complexity of board (within reason) and if multiple boards were being made then I could easily expose more whilst some etched etc. It would not take one hour per board. To mill a more complex board would obviously have taken a lot longer and I can only mill one board at a time.This won't make my chemical capabilities redundant, far from it. It will without question be used to drill all such boards though. This will dramatically cut time. When I print the transparency I will simultaneously export the Gerber/G-code for controlling the drilling process. Of course zero-ing the X/Y axis and board alignment on the table will be paramount for such but not that hard to do.
For modest boards and certainly any one off or prototype, being able to create in minutes with no mess is a huge plus and a "no-brainer". For PCB work you could certainly use it on a desk or the like as there is only minimal mess, but remember to wear a P3 dust mask!
Next up is trying it out to cut holes in plastic. Reviews / sales docs claim it can cut / mill 6mm softwoods but that won't remain to be seen as I just need it to cut plastic a millimeter or two  thick.I've not done anything with the Laser yet but the shark keeps giving me a wary look anytime I go near.....RegardsLeft to right: 20d V-cut, 40d V-cut, 0.8mm End Mill

Thank you very much for sharing your progress with CNC. I'm definitely going to have to look into getting something like this when I can see having some time to use it.

HiWhat I learned today.Laptops are lazy little things. They go to sleep at an unreasonable time without care nor consideration for those around them...Today was time for hole cutting. I discovered Carbide3D has a free download called Carbide Create which you can use to create shapes and generally make all sort of setting / tool changes. Obviously earmarked for their products but will generate g-code for any machine. Quite easy to use, rarely needed to go to the "Help" pages.With a piece of scrap plastic (front panel) around 2.5mm ish thick secured to the bed (with clearance below to allow the bit to pass through and not touch bed) I did a few manual plays with an assortment of end mills etc I have quickly amassed. Spindle speed, feed rate etc were all experimented with and I think for this little machine it is best not to ask it to cut a shape in plastic all at once, instead make multiple passes increasing the depth each pass. In Carbide Create this depth per pass can be set (as I'm sure other applications can do too).I created a simple rectangle, saved and opened up in Candle (CNC software supplied with machine). Zeroing the X/Y/Z appropriately I then set it off on it's task.Off it went, making deeper and deeper cuts each pass and all was going good. Well too good until it stopped without obvious reason. Turned out that my lazy laptop, which of course was running sans AC decided it was time for a nap thereby shutting down comms ports amongst other things. This resulted in no instructions being sent and a complete halt to the proceedings.I have attached a picture of where we got to before bedtime (ignore the large scuffs / cuts, result of various tests) and you can see that if it had finished it's task, with only a little bit of deburring etc I would have had a reasonable shape cut out. I measured the internal dimensions, compared these to what I asked and I'm not complaining. I asked for 30mm x 20mm and got 30.3mm x 20.2mm back (I couldn't get my calipers fully inserted though as the hole wasn't complete). Certainly good enough for me.
I did notice that those little heatsinks that I mentioned before were getting seriously hot. As I was doing this indoors I had a vacuum cleaner handy disposing of debris and a quick reroute of it's nozzle soon cooled things down. I'm guessing that perhaps some of those that may have had reliability issues may not have appreciated heat vs silicon. I will perhaps fit a fan or the like to assist, or be lazy (like my laptop) and just keep the Dyson to hand.Regards

HiNow I know why aliens like probing things... It is the height of good fun......
Candle (software that came with the machine) has a Z-Probe function. If you connect your work to Ground (0V) and the spindle / bit to A5 on the controller board using appropriate wires, when "probing" the Z-Axis the CNC will automatically detect when the bit touches the PCB. Very cool.What's even cooler is that in Settings / Console you can enable Height Mapping. Once enabled you can then create a height map of your work. Once selected there are a few settings to be made such as size of work area, how many points to be probed X/Y etc then off it goes. At selected points the CNC probes the Z-Axis and creates a map of the board height at each point probed This can be quite time consuming depending on board size and number of
points to be probed. In the photo below you can see the map with nine
probe points overlaying the contour. It took approximately two and a
half minutes to probe and you can see that there is a difference in
height over the board of more than the depth I wish to mill.If you then tell it to use this map it automatically takes the height of the board into consideration when milling the PCB and you can see the Z-Axis adjusting to compensate as you mill.
In the pictures below in which I've been experimenting with settings etc on some PCB, you can see very acceptable results using a 0.1mm 60 Degree V-cut with a slow feed rate of 25mm/min cutting to a depth of 0.06mm. Default pad sizes for components and a 0.5mm track width. I held the board up to the light for another picture and you can see clean cuts. Without the height map I would have needed to increase my depth of cut or risk some areas not being milled at all. Of course increasing depth means a wider cut which could eat into track width.I fitted a fan to the unit which connects to the 12v pins of the controller board and this keeps those heatsinks pretty cool when the motors are running. Definitely a recommended addition. I was just using croc clips and jumpers to connect to the probe points but I'll probably make up something a bit more permanent. I also bought a set of Step Clamps which are a far better idea than the supplied bolts and washers for holding the work in place.
I'm still experimenting with this but I can certainly say it will mill / drill / cut everything that I need it to.
Regards

HiDid some further tests using various V-cut bits and trace widths.This time I routed a track between IC pins. Tracks were 0.5mm in width with one track starting at 0.4mm then dropping to 0.2mm in width. Yes, I was having a laugh and didn't expect much.
Board was height mapped before each cut using 0.1mm 10/20/30/45/60 Degree V-cuts at a depth of 0.06mm. I didn't spend too long on the mapping but obviously the more you probe the more accurate your milling will be. I was more interested in comparing how the bits performed.
Without question, for me and this setup, my best results were obtained with the 60 Degree V-cut. The 10 Degree basically shredded everything it touched which could be due to the modest speed (max 10000rpm). V-cuts like high spin rates.I have attached two pictures showing the 60 Degree cut. It cleanly routed the 0.5mm between IC pins and it did do the 0.4mm track but although the 0.2mm track is almost invisible having been almost milled away completely, it is still there as confirmed with a multimeter. I was astounded by this.
I don't need to go smaller than 0.5mm and if I did I could perhaps do so chemically.Regards

Nice series of posts the Mr Chip Fryer, on each post you made I was going to comment, but on subsequent posts I saw you got there already
I've done the same - I bought a similar CNC machine (probably the same design, looks like it) specifically for doing PCBs. Patch antennas for satellite comms, as part of my day job.Funnily enough it was just this afternoon that I was out buying flexible tubing to attach to the machine, as I am not a fan of FR4 dust in the lab. It really does rate up there with asbestos as a bad dust to be generating, FYI.
I was going to write an article on this device but instead will just post a link to your posts, you've done a great job there!
If you get bored of CNC machining stuff, go get yourself a 3D printer. Similar price, brilliant performance. https://m.gearbest.com/3d-printers-3d-printer-kits/pp_1845899.html?wid=1433363. I'll be covering it in the magazine if you don't get there first!
Regards,
Mike.

Dear MikeThanks for the kind words and sorry for my tardy reply as business commitments can keep me away from more fun pursuits.
I would first like to take the opportunity to say how much I enjoyed your articles in EPE. Very informative.
Since my last post I've actually created my first board from start to finish on the machine. It milled, drilled and cut out the PCB from blank stock. Admittedly it is rather basic but small steps as they say. It's just a few header connections surrounding a RF module I use, but I have learned a LOT about CNC and G-code in the process.Totally agree about FR4. I fashioned a small frame that sits on a workbench and I then ty-wrap the nozzle of my garage vac to it. It allows me to position the nozzle pretty much where I want irrespective of cutting tool. Cheapo vac so it isn't HEPA filtered but better the dust away from me than on me. Of course I strongly recommend a proper P3 mask too. I got one with replaceable filters from Screwfix for under £20. Barely know I'm wearing it which causes the postwoman some concern.......
Now that my confidence has grown I will probably use the CNC bits obtained cheaply online for experimenting and invest in proper bits from more reputable sources. Looking at the points of some of mine you couldn't tell they were all supposed to be the same tool...:)Next experiment is to up the feed rate. Not so much when milling the tracks but finding a good trade off between depth and feed when cutting the board. At present I haven't went deeper / faster than 0.4mm using a 1.0mm end cut chipper with a feed of 25mm/m.I did notice a problem with the machine though. In the Z-Assembly there are two stabilising pillars aside the lead screw. The assembly has inserts that the pillars pass through. Depending on what it's doing, the vibration can loosen these inserts and they drop out. This of course destabilises the assembly. This could be my problem though as I liberally applied graphite (obtained from an aircraft carrier) along all rails, rods and runners to lubricate. Graphite gets everywhere and without question is now on the outer edges of these inserts. I'll get around to cleaning it up a bit some time.I found that my Y-axis motor gets much noticeably warmer than any other. When creating a height map it gets too hot to comfortably touch despite the X and Z-axis doing far more work. I have a couple of 30mm fans so these will probably join the small blower I fitted earlier, to cool the steppers.Got to have broken even by now on the purchase price versus keep-out-of-pub...:)Below is a picture of the board before being rinsed and attacked with a wet-block to get rid of swarf and burrs.Not had a chance yet to play with the laser, but I will get around to it once I figure out a reason to use it :)Thanks for the link to the 3D printer. I've really only seen the ones available in shops such as Maplin etc plus of course I've read about others, but they were all too expensive for what would be for me a hobby purchase. The ones advertised for £150 upwards (from China) I didn't really look at, mainly for the same reasons as not looking at these CNC machines until now. Having first hand experience of what these CNC's can do I may look deeper into 3D. If you do write an article please send me a link as I'd be keen to read more.Regards

HiWork commitments have kept me away from this but I have recently:-Fitted fans to all stepper motors (in addition to the blower at the heatsinks)Connected the body of the drilling motor to "A5" with a semi-permanent crimp and and added a Croc Clip to the 0v for height mapping (I kept forgetting to disconnect the clip on the bit before energising the motor...).Ran wires for Z-Axis end stops but haven't yet got around to fitting any.I'll forward photo's later but included here are two of 0.1mm 60-degree V-Cutters.
The first is Chinese and you typically get five or ten in a pack.The second is from a well known PCB supplies company in the UK, and for the cost of this single bit you could get quite a lot of the Chinese ones indeed.
I've only used the Chinese ones so far (documented above) as they are so cheap it doesn't matter if they break. I have had OK results with them but I'm keen to see the difference the UK sourced one makes. I will probably cry though if it snaps....Apologies in advance if the photos don't appear in sequence correctly as I still haven't figured out the trick in posting them here.
Regards

Chinese 0.1mm 60 Degree V-Cut

UK Sourced 0.1mm 60 Degree V-Cut

Well I'm shedding tears.....My own fault. The purpose of milling is to create isolation. If you have isolated something then there is no electrical path. I milled an area using a Chinese bit then swapped over to my expensive UK bit to mill the same circuit for comparison (elsewhere on board). I performed a "Z-probe" but stupidly the probe took place over the area previously milled and you can guess the rest..I'm going to fit a big STOP button to it.

HiBeen traveling so haven't been able to play until recently. Not sure if anyone is following my attempts but this is my latest update re PCBs.I have been using TINA to directly export the G-Code and this did provide acceptable results but it did require me to become familiar with G-Code if I wanted to tweak certain parameters. Previous attempts at exporting Gerber and then converting to G-Code had limited success.I tried using FlatCam (free) which is quite a powerful piece of software, and although it would open and allow me to manipulate the Gerber files created in TINA, when I tried to open the Excellon files (drills) they were completely wrong in terms of size and positioning. I tried scaling etc to no avail.I have now found out why I had this trouble. I use Metric measurements and had set FlatCam to such. That's fine when opening the Gerbers however if set to Metric and opening the Excellon (drill) files the problem occurs even though the files were created in "metric" TINA. If I open the Excellon files in imperial measurements (i.e. keep FlatCam Excellon set to inches) then everything aligns up (yes, I do mean I open "metric" contours and "imperial" drills on the same sheet).FlatCam allows me far greater control over the machining process. I can make many tweaks, add in text or shapes and a whole raft of other features can be utilised before creating the G-Code. Now that I have figured out the drill issue I have to say I'm impressed with it.So far I'm having good and repeatable success using the following when milling tracks:-Tool = 0.1mm 30-degree V-Cut (set diameter to 0.15 as this is the approx diameter when at depth)Z-Depth (cut) = 0.0933mm in two passes of 0.04665mmX/Y Feed rate = 100mm/minZ Feed rate = 79.9998When Z-Probing the more you probe the better your results but as I minimum I probe 4mm grids. The more points in your grid the longer it takes to probe but it can be very worthwhile.When cutting I use a 1.49mm End Cutter and usually run four passes at 0.45mm with a X/Y feed of 50mm/min. I could probably run higher but I'm in no hurry <s>I will attach a couple of pictures later.Regards

Chip,Glad to hear that you are still going at it. I've got this bookmarked so I can follow...

HiA little later than promised due to travel.I mentioned earlier that I made some modifications and bought some extras. First thing was to fit a small blower to keep the heatsinks cool. This is strongly recommended. I had various blowers / fans kicking around so used them, but they are so cheap to buy you should do so too.

I also fitted fans (roughly) to the stepper motors themselves and one day I'll do a better job

Fan fitted to top of Z-Stepper
Don't know why but this picture has rotated 90 degrees left..! It shows the fan on top of the stepper. The coiled red & black wires are for a Z-Limit switch I've yet to fit. The brown wire is on a spade crimp tightened up against the motor body which provides a connection for Z-Probing. When the drill is inserted it makes electrical contact with this wire via the body. The "splatters" on the wall behind are from the last person that displeased me.
This picture shows my Z-Probe ground wire (and a reminder to connect it). With this connected to the PCB the Z-Probing is a breeze. You can see the fans fitted to motors too.
It is essential to hold the board firmly in place whilst working. I strongly recommend the use of step-clamps and I bought two sets made by Proxxon. These clamps allow you to clamp pretty much anything you wish.Proxxon Step-Clamps holding the PCB and a piece of waste-board firmly to the bed. Note the Ground probe clipped to one of the clamps. When the bit touches the copper the Z-Probe circuit will complete informing the controller of the height at that point.Looking down on the table.I like to print an actual size copy of my circuit and cut it out. I then use it to ensure  the mill won't foul against the clamps and to align the X and Y axis (zero X/Y).
Plenty of room around the intended circuit.Manually moving the mill to the bottom left corner. Once in the correct position the "Zero X/Y " button is pressed and sets the X/Y Zero to these coordinates.Next is to Zero the Z-axis. Moving the print away the Z-Probe button is then pressed (make sure ground is connected to the clamps first). This slowly lowers the mill until it touches the copper and then stops.Z-Axis Zero. Once the Z-Probe has completed simply press the "Zero Z" button and the controller now knows at what height the copper is.One all zeroed it is recommended to create a Height Map. More on this in a follow up post, but briefly it moves across the board in a grid like manner Z-probing to establish a "map" of the board height at each probe. The board will not be completely level and the thickness of the copper can vary. These factors can and do affect the depth of cut. Mapping helps eliminate problems due to such.Once mapping is complete and is in use it is time to cut. I recommend the use of a good quality cutting oil for a few reasons. It will keep the mill cool as it works (especially if using Fibreglass), it will help to clear the swarf from the bit, and importantly it will help prevent the swarf flying around. Unlike when perhaps drilling some metal, I make a puddle over the entire area. I have a bottle of Clarke's cutting oil which I think is around a litre. This will last me for a very long time. Afterwards I use a paper towel to clear up the mess. The next few pictures illustrate.
A nice big deep puddle
Milling complete. You can see the swarf.
Drilling in progressWhen you complete the milling and insert drills you then need to re-zero the Z-axis. I manually move the head slightly outside the pattern (maybe 0.1mm), Z-Probe and then set the Z-Zero. I then open up the height map and use it. This needs to be done after every tool change. If you don't move the bit slightly outside the pattern there will be no circuit to make when probing as you will have isolated your board from the remaining PCB. This results in broken bits. Guess how I know :)After drilling it is time to cut the board. In this example I will leave tabs on each side and then break it out afterwards but you can simply cut it out completely if you prefer.
Cutting almost complete.Look at all that swarf that is being held in suspension by the cutting oil. Without the oil an awful lot of this would be slung into the air and that is not a good thing especially if using FR4.
Don't know why it has rotated again, but this is it after a wipe with a paper towel and a going over with my vac.Snapped out and just needing to be deburred.To make this board, after clamping it to the table it took around forty minutes or so to probe and create the height map. During this time I could go and do something else more fun (and did). The milling took another forty minutes or so and again once started I left it to get on with it. The drilling needs your attention as you need to change bits and rezero and for this board it took around half an hour or so. Once drilled the cutting took around fifteen to twenty minutes to complete. That makes around two hours to create from beginning to end.In my next post I'll document a bit more of zeroing etc and include some more photo's.Regards

HiFollowing on from before.Using TINA I created my PCB layout and exported as Gerber, then opened up the files in Flatcam before exporting as the G-code necessary for the CNC to operate.One nice touch in Flatcam is that it informs you of the milling distance in your design i.e. how far the mill will travel to complete. This will surprise you. One of those 70mm x 100mm boards had nearly 5 metres of milling within....Anyway, the nice touch is that this allows me to keep note of how much milling each bit has done and will form a record for reference. The bit I have been using is now just showing signs of wear after over 25m of milling. I have to admit that I don't know if it was brand new when I started to track it or not. However as they are around 50p each from China it isn't a concern but nice to know when I can expect to change bits.I keep separate bits/records for FR1 / FR4 etc.Once I have completed within Flatcam it is exported as G-code and opened up using Candle (controller software supplied with CNC).The next few pictures reference the board in the preceding post.
G-code opened up in Candle. The bottom half of the main window documents each line of our generated code.
In the top right hand corner you will see the "State" window and in here we find the Work Coordinates and the Machine Coordinates. These are populated by the controller upon power up and by and large don't mean very much to us yet.Beneath this we have the "Control" window which allows us to do things as set x/y/z and probe etc.Then we have the "Jog" window which gives us manual control over the x/y/z motors to move the bit.
As mentioned in previous posts we need to zero x/y/z axis. First make sure the bit will clear the board and clamps during travel (adjust Z to increase height if required) then using the "Jog" controls we move the mill to the appropriate position for X and Y. As the bit moves you will see the coordinates change to reflect current positions. Once at the desired position we then press the Zero X/Y button in the Control window. This now sets the Work coordinates to x=0, y=0, z= whatever.
Zero x/y completed. Note the change in coordinates from before.Next is to Z-probe to find out at what height the copper begins. Pressing the Z-probe button will slowly lower the mill until it comes into contact with the copper (making the circuit as explained above) automatically stopping once reached. Simply press the Zero "Z" button now and you have zero'd all three axis.
The above shows that since we switched on, we have moved the Machine coordinates from initial position by a considerable amount. As this is where we want the project to start, the work coordinates were zeroed giving us our "Home" position. During the milling operation this zero position will be returned to after each stage has complete.Although we could start the cutting process now we wouldn't get much success unless very lucky, as there is no guarantee the board is perfectly flat or the copper is of even thickness. To overcome this we create a height map. This sends the machine off to probe the board in a grid pattern mapping the height as it goes.If we scroll down from the "Jog" window we come across the Heightmap window. If we click the create button we get a window like the following.

Near the bottom of the main window we see Heightmap Settings. In here we set the borders and other probing requirements. Clicking Auto sets the borders to that of the opened project, but you can manually set to suit.Next we need to set the Probe Grid X and Y. With the cheap FR1 boards I have been practicing with I have been getting good results by probing every 4mm ish. My X is 58.18mm so dividing that by 4 gives me 15 (or near enough). My Y is 83.18mm which then gives 21 (or near enough).Once these X/Y details have been entered we can start the process by pressing "Probe". The CNC machine will now probe the board, in our example every 4mm ish, showing results as it goes until it has covered the entire area. Depending on size of board and amount of probing this can take some time. The software gives an estimate of how long this will take but is just a rough estimate whilst probing. Milling and drilling estimates are quite realistic though.
Mapping complete. We can see a graphic representation of height at each probe point.Once mapping is complete we need to save the file (File>Save As filename.map).Next is to use the Jog controls to raise the mill to a safe height above the board to allow for travel back to the home position.The name of our saved map should now be populated in the Heightmap window, if not click Open and choose the saved map.You may need to toggle "Edit Mode" to close out the Heightmap Settings window and return to G-code.
 If we scroll down to the bottom of our G-code we can see we have 29,232 lines of code to control the milling of our tracks. If we then click the "Use Heightmap" checkbox the software automatically makes adjustment for height at each point based on our newly created map.

We now have 30,335 lines of code after Heightmap inclusion.We can now click "Send" and the CNC will go off and mill our board. Don't forget to include a puddle of oil on top <s>As the milling gets underway we will see progress graphically over our "board" with the lines turning grey as they get milled. Also the lines of code will scroll indicating status of each command. Once complete the mill will stop and return to the Home position.
This board took 47 minutes to mill and during which you can pretty much leave it to get on with it whilst you do something else.Next we would drill the board by loading the appropriate file(s) remembering to undertake a new Z-probe after each tool change, then re-loading and using our heightmap.After the holes are drilled we would then cut-out the board, again after Z-probing after tool change etc.Regards

Hi

I mentioned above that I am using step-clamps made by Proxxon to secure the
work. However sometimes, depending on the size of your work that may not be
possible as the clamps would interfere. In those cases, and I believe it is a
very popular way to do it, I secure the PCB to the waste board using double
sided tape. I find that Tesa tape provides a very strong grip.

I secure the PCB to the board with tape, then use the step-clamps to secure
the board. I usually find I can get one clamp to make contact with the PCB so I
use that when probing.

PCB secured to board by tape with one step-clamp in contact

I find it very helpful when applying the tape to let it overlap, that way I
have something to grip when removing it.