CNC PCB mill for n00bs

Thank you Clay for your comments and your compliments. I am glad you could provide some input. You are really improving, I must say, based on those pics you posted. Well done. If you get a chance, try and post some more pictures of your work with a bit of a description relative to CNC. I think that could be a real benefit to those just starting out so at least they have some basic idea of feeds speeds and what you can expect to cut without issue. Think of all those broken tool bits you'd save during the first couple of weeks of operation.:smilewink:....:music_whistling:

One point you mention which I forgot is that these machines also have several versions including the electronics package so it hard to know what in fact you are ultimately receiving.

Michael, prior to purchasing, it might be worth while having a long conversation with Clay about his journey getting the same type machine producing acceptable results. I'm sure Clay can provide some great insight for you.

I hope you have good luck with this .:)

John

Tx 4 the tips. I posted on CNCforum but didnt get any response there yet.

Clay, your experiences will be invalueble to others whish to dive into Chinese CNCs. Maybe u could summerize what u learnt here, plus the DOs and DONTs of (Chinese) CNCs.

Unlike CNCZone forums we both are into DCS and u already know about chinese CNCs. I read threads as suggested and noted on youtube that u had problems with the ballscrews.

Since your positive about the chinese i am now seriously contemplating an order CNC 3040Z ballscrew-version. Whats putting me off is the parallel port. Yes, use an old computer.. but here in Holland the houses are literally pigeonholes. My hobbyroom is the size of the average American house' bathroom. So an extra computer/laptop.. its taking up valueble space.

Which bits are u using, forexample to make holes, and/or clear copper areas example, for the UHF plate?

BTW. UC100 is a parallel-USB interface adapter.

Pappavis

 

After considering price and size I decided to take a chance on a 3040 cnc. I also had a tight budget which, in the end, was the deciding factor.

 

I would definitely purchase again. Well worth the money in my opinion.

 

Clay

pappavis,

 

 

Do you speak Russian? I few months ago build CNC, can share knowledge, but I bad speak English.

Я могу читать и понимать очень мало слов. У меня была русская подружка ;)

grtz,

Michiel

the UC100 is essemntially a USB2parallel interface but it does more than that and requires a plugin to your control software. Looks like mach3 is supported to when I had a quick look.

The other thing is to get a pci parallel port card, you might have to run an old version of windows but not an old PC if using a parallel port. From memory...

As metalnwood says its more than a parallel port in fact I would not call the UC100 a USB to Parallel interface per say. Yes it's USB and has a DB25 on the other end, but it's not a parallel port to the computer. It's a microcontroller that handles sending pulses to the stepper. To use it you need CNC software that knows how to specifically talk to the UC100. That's either Mach3 or UCCNC.

Pappavis

Read my cnc thread

http://forums.eagle.ru/showthread.php?t=146467

It should answer a bunch of your questions.

Before you purchase keep in mind the limitations of these machines. My opinion is that for plastic and pc boards you should be able to make everything you need for the pit. As long as the seller doesn't try to rip you off!

I do agree with all Johns points regarding the faults these machines have but if you do things correctly you should be able to make it work.

Also search 3040 cnc at CNCZone and read as much as possible. There is some good info there.

Hi Clay, gadroc, John & lurkers :)

I took the plunge. I bought a Chinese "CNC 3040Z-DQ 3axis Router Engraver with limit switch with 1204 ball screw".

I read the forums as advised. I am scared sh*tless.. Its expensive!!

Total price=€889 to be shipped from Deutchland. The seller has his stock now on sea to the EU.

[edit]hopfully to receive it by 25-3-2016[/edit]

Software & controlling is still a problem. I consider to buy a TinyG USB controller for use with Chillipeppr & bCNC. Its supposed to be an alternative to the UC100 controller.

Questions;

1. Has any1 of u stuck a CNC USB Controller into the Chinese CNC machine? If so, which?

2. Does a TinyG controller work on other open source software, such as bCNC?

3. Can i use a UC100 controller on bCNC?

4. Which (free/open source) alternatives are there to Mach3?

5. FLATCam seems to be an Open Source alternative to CAMbam. I tried it on my laser cutter. Any1 als also have experience on FlatCAM?

6. Which engraving bits are best for PCBs? Carbide flute, tungsten..?

7. WHich bits are 'best' suited to milling woonden/perspex panels. Considering i might break a few..

8. other words of wisdom?

I ask here, coz maybe other guys on the ED forums also wanna build a pit, and buy a (Chinese) CNC. This way, we can share experiences, and concentrate it in one place.

Eventually.. later on i could do a small writeup / FAQ of my experiences and publish it here summarized as a single closingpost in this thread.

Hi Clay, gadroc, John & lurkers :)

 

I took the plunge. I bought a Chinese "CNC 3040Z-DQ 3axis Router Engraver with limit switch with 1204 ball screw".

I read the forums as advised. I am scared sh*tless.. Its expensive!!

 

Total price=€889 to be shipped from Deutchland. The seller has his stock now on sea to the EU.

 

Software & controlling is still a problem. I consider to buy a TinyG USB controller for use with Chillipeppr & bCNC. Its supposed to be an alternative to the UC100 controller.

 

Questions;

1. Has any1 of u stuck a CNC USB Controller into the Chinese CNC machine? If so, which?

2. Does a TinyG controller work on other open source software, such as bCNC?

3. Can i use a UC100 controller on bCNC?

4. Which (free/open source) alternatives are there to Mach3?

5. FLATCam seems to be an Open Source alternative to CAMbam. I tried it on my laser cutter. Any1 als also have experience on FlatCAM?

6. Which engraving bits are best for PCBs? Carbide flute, tungsten..?

7. WHich bits are 'best' suited to milling woonden/perspex panels. Considering i might break a few..

8. other words of wisdom?

 

I ask here, coz maybe other guys on the ED forums also wanna build a pit, and buy a (Chinese) CNC. This way, we can share experiences, and concentrate it in one place.

Eventually.. later on i could do a small writeup / FAQ of my experiences and publish it here summarized as a single closingpost in this thread.

I Congrats Pappavis.

I don't have a 3040 to add one to but the concepts are the same for all CNC milling machines. I've considered getting a 3040 to pair with the bigger gantry router. We'll see how well my gantry router does with 1/16" aluminum.

You need to understand the components involved here when we say "CNC" software. There are many tools which combine multiple aspects so it's hard to say what works with what without understanding the components.

CAD - Software used to design the object. This outputs a file which defines the shape via mathematical descriptions. (Example formats: STL, STEP, IGES....)

CAM - Software used to design the toolpaths and cutters which will be used to cut aways parts of stock to generate the designed shape from CAD. This outputs G-CODE which tells the machine how, when, where and how fast to move the machine axis to move the cutting head in the right way to cut the stock.

Trajectory Planner / GCode Interpreter - This component reads the g-code and make a plan taking into account limitations of the machine to how it will cut with the g-code. This planner will often modify speeds in order to make a smoother path or prevent motions which might damage the machine.

Motion Controller - This component takes the trajectory plan and turns it into electrical pulses which the stepper drivers need to move the machine. This component is very timing sensitive as the torque, and smooth action of the motors is dependent on a properly timed set of pulses.

GCode Sender - This is a tool which will transmit g-code to a trajectory / planner component which is not running on the computer.

Machine Control UI - Allows jogging of gantry, controlling spindle and other activities.

In terms of the products you've mentioned here is what they do:

UC100 - Motion Controller

UCCNC - Trajectory Planner, Machine Control UI

Mach3 - Trajectory Planner, Machine Control UI and it has a plugin that uses a parallel port as a motion controller

TinyG / GRBL - Trajectory Planner and Motion Controller

LinuxCNC - Trajectory Planner and has ability to use parallel port as a motion controller

bCNC - GCode sender, Machine Control UI

• You wouldn't need bCNC with Mach3, UCCNC or LinuxCNC as they read the GCode file right off the computer. Also bCNC supplies a Machine Control UI which is already incorporated into those products.
  
• You can't use bCNC with UC100 because neither has the trajectory planner.
  
• You don't need a UC100 if you use TinyG because TinyG as a motion controller built in.
  
• You can use a UC100 with Mach3 to replace it's built in parallel port motion controller.
  
• UC100 is not compatible with LinuxCNC
  

Unfortunately the open source tool chain for CAD/CAM is significantly lacking. There are tools out there, but they don't really compare to the commercial offerings. There are several free as in beer tools you can use.

SketchUp is a pretty popular CAD, but in my opinion is a horrible tool for solid modeling of mechanical components. Check out the OpenBuild forms for SketchUCam which is a CAM plugin to SketchUp.

While not open source, I use Autodesk Fusion360. It is a combined CAD/CAM system and is VERY powerful. There is a free tier of hobbiest you can elect to after the free trial. Just be aware if they cancel that tier you will have to port all your files.

I have not tried FLATCam, CAMBam.

Tools and speeds and feeds are several pages of discussions, and quite honestly I don't have them figured out yet ;)

I am scared sh*tless.

And so you should be. :P

I do hope you get a reasonably good machine that will perform as you would like it too. All I can suggest at this point is to start reading....:music_whistling: There is the Mach 3 manual which you need to read and understand before you do anything with your machine. You need to learn how to draw stuff...AutoCAD manual (read it). I use AutoCAD to draw my parts as you will want a .dxf file to import into your g-code conversion software. You do not need to draw them in 3D. That is going way overboard and entirely unnecessary. Your machine and the associated software will not cut it in 3d. Its actually referred to as 2.5D. Which brings me to CamBam. Buy it, use it. There is nothing else as good for beginners. Do the tutorials and read the manual.

This is the order of battle:

1. Draw part in AutoCAD LT ($1000.00) and then export dxf file.

2. Open dxf file in CamBam ($150) and assign cutting depths and tooling to cut the part. Generate g-code and send file to PC that is running Mach3.

3. Open g-code in Mach3 ($200.00) and set zero. Hit "Run" or whatever that big green button is called, and watch part being cut with finger on the e-stop button ready to shut down everything in case you run the spindle head against the side of the machine or whatever.

You should try and find an older PC with XP and a parallel port. It should be 100% stand alone with nothing else running on it. Not even virus protection and no internet connection. It will be 100% reliable if you do that. Opps...did I say 100%... Yup 100% reliable. Remember! Nothing else on it or running in the background... period. This machine must be used ONLY for running Mach3.

BTW...

****NEVER LEAVE YOUR MACHINE WHEN RUNNING...EVER**** (not even to take a piss)

. Its expensive!!

Not yet, but it will be. :music_whistling::megalol: You still have a crap load of extra crap to buy. (often called tooling and accessories) As you will soon learn, buying the machine is the least expensive part of this exercise. Check those threads I linked earlier. They have all the tooling and where to buy from in them. Clay can walk you through some of it I'm sure. You also need a dial indicator, some double sided tape and several collets.. You can waste money on trying other double sided tape but in the end there is only one to use. Again, look in the other threads for it.

Engraving v-bits are expensive and if you want a good job you will buy them. If you go cheap, you will soon see why your work piece looks like shit.

One last point. If the cables from you CNC controller to each of the stepper motors are not shielded, replace them with shielded cable. This is extremely important. The high speed spindle will generate all sorts of EMI and that will cause your motors to mover unexpectly when you cutting a work piece.

That all for now. I'm not allowed to post very much now a days. Doctors orders. I had the misfortune of having three heart attacks from Dec 20 to Feb 20. Actually, each one was on the 20th of the month. Pretty Fcked up if you ask me.

Good luck and I will keep an ear to the forum. (if I'm allowed) :music_whistling:

Warhog, if your suggestion is to spend $1150 on the cad/cam stuff then I would alternatively suggest a vectric product. http://www.vectric.com

It is both the cad/cam together and was really made for cnc routers. It ranges from cut2d at $149 to vcarve pro at $699.

These will do more or less anything you want on a 3 axis cnc router. Very easy to use and extremely popular with cnc router people.

Mr Burns, you and I will have to disagree on your last sentence :)

 

One CNC I built, using ballscrews on all axis was able to reposition to 0.01mm, or 0.0004". Thats all I bothered calibrating it to because thats what my dial indicator had.

 

Under load, < 0.1mm. Usually better to cut .1mm oversize and do a clean up cut to size around the profile .

 

If your machine is not rigid enough to give you the accuracy then the above step might help. If you cannot position with no load <1mm then something else is wrong :)

 

I met a guy who has something like the one the OP is looking at on ebay. It was using ballscrews and if they are your average ballsscres coming out of china then they should be OK for doing PCB's.

 

For myself, if the price was right I could get one for PCB only work knowing that the machine under the light load of doing a pcb would be ok. It would be similar to something I would build myself if it was for only that purpose. This guy who has one, when he puts it under load it vibrates like nothing and the piece of aluminium plate on the front of the gantry turns in to a soundboard amplifying everything. Not good to be around for a long time.

 

Edit, last sentence should read heavy load. IT can cut away lightly all day somewhat quietly but as an example, he cut a piece of aluminium for a motor mount and it took three hours, hard on the ears. I am now cutting all the parts for his new CNC machine, that three hour part is about 4 minutes on my larger machine.

I should qualify that, I am never going to get <0.1mm! :helpsmilie:although I have made it a little smaller and running it on aluminium runners and not copper pipe which flexed in the middle.

Warhog, if your suggestion is to spend $1150 on the cad/cam stuff then I would alternatively suggest a vectric product. http://www.vectric.com

 

It is both the cad/cam together and was really made for cnc routers. It ranges from cut2d at $149 to vcarve pro at $699.

 

These will do more or less anything you want on a 3 axis cnc router. Very easy to use and extremely popular with cnc router people.

I had considered the Vectric line of software way back when but as I'm a full time designer working with AutoCAD, it was what I already know and love. It was CamBam that made a big impression with me due to ease of use and cost. In fact I was using it for free for almost a year before I decided to buy it. As I recall the Vectric stuff didn't let you try it out properly before deciding if it was good for my application. That's why I didn't investigate it further.

But each to his own. Whatever you are comfortable using. I will say this however, for every part I make, a huge amount of time is spent in the drawing stage. It's so nessary to make sure your drawing will turn into a functioning part when all is said and done. So much thinking and drawing/redrawing or revising is required at this particular stage . I'm in the process of designing some replacement rudder pedals for the A10 and I have been at it for almost a week now, an hour or two each day. I've just scratched the surface of this project and its all drawn/detailed in AutoCAD to three decimal places of accuracy. The reason I mention this is that the drawing package you select needs to be what you are most comfortable using only because of the amount of time you will spend just drawing stuff.

I just remembered... CamBam also has drawing tools, somewhat limited but still quite adequate for drawing panels, to be sure.

I use CamBam on a daily basis. It seems to able to do everything I need to draw panels and pcb's. For someone that does not have cad experience I think it is great! Especially the way its layers work. Once you get used to the interface you can build everything on differant layers. Then you can select with objects regardless of their drawing layer to a machine operation. In the end I have a single file that contains all the parts but more importantly it has all the machining operations that need to done as well. So after all the drawings and MOP's (machine operation's is where the g-code will come from) are done I can select which MOP I want to run and it makes the g-code required.

It's line drawing tool could use some improvement but that might be something I haven't figured out yet.

Basic pcb's are doable but you will need something better to design boards with and then send it to CamBam.

Clay

Very nice work Clay. I guess I'm so in tune with AutoCAD nowadays that I don't see other drawing tools. But yes indeed, CamBam does a reasonable job at producing a panel drawing. That might be the best beginners scenario I've seen so far. There also appears to be enough people here on ED Using it who can assist others who are still struggling with learning it. Actually struggle may be to harsh as this is definitely one easy program to learn how to use.

Finally my CNC 3040Z-DQ has arrived from China-CNCrouter.

Overall, i am VERY HAPPY. But, let me report back in a few days again ;).

The machine is sturdy, all solid ball screws with limit switches built in. The controlbox has a parallelport for Mach3. Ofcoz I changed it to a TinyG USB controller :music_whistling:.

Setting up TinyG took me about >=3 days to figure out all the wires as my electronics knowhow is severly limited. I havent milled anything yet. Using a markerpen plotted a PCB onto wood. Before commiting to the real deal of PCB etching.

The machine was 95% pre-assembled. One only needs to hook up the printer cable, mount the Nema23 stepper motors, tighten some small screws and you're ready to go. Thats the theory. I am still learning about homing, limit switches etc.

The kit is quite complete coming with 4x drill bits, z-minimum probe, tools, reserve limit switches. After scratching my head,the limit switches are now also connected to TinyG. I have them setup for homing. Dont know how homing works yet, but will figure that out l8er.

My toolchain;

* FREE http://chilipeppr.com/tinyg . This is equivelant to Mach3.

* FlatCAM --> Converts GERBER-files to gcode.

* KiCAD for PCB designs.

So far i am happy :)

TODO:

* Write a small blog on howto get TinyG going + my experiences.

Looks like your making good progress! Please let us know how tinyG and chilipepper are working out for you. I have considered making that change as well but so far its "if it aint broke dont fix it".

Keep posting!

Clay

Yes, its very close to working. Took me <>4 days = 16 hrs of experimentation.

FYI. I bought a chinese CNC 3040Z-DQ with limit switches of ebay. Also, replaced the Mach3 parallelport for a Chillipeppr USB Motion controller. Its got Nema23 stepper motors.

VERY IMPORTANT accuracy settings;

Measurements $gun=0 (G21 millimiters)

Limit switches = NC (Normally Closed)

Motor 1,2, 3 Micro Steps=Eigth

Motor 1,2 Travel Per Revolution=4,1 mm/rev

Motor 3 Travel Per Revolution=2

Step Angle=1,8

Below. Try-out PCB etched into wood for Arduino Nano.

Non copper regions=0,2mm v-shaped bit.

Drill holes=0,8mm ball nose bit. (which bits do u use??)

Earlier failed test runs :P. Trying to reproduce a DirtyPCBs-version on my own machine.

Things to note;

1. Travels per revolution is VERY IMPORTANT!! Its influence for the scaling.

2. Stepper motors must be tightend very well, otherwise the ballscrews wil lwobble causing erratic patterns.

3. For this particular CNC, wire the limit switches all to GND, then per limit switch connect it to the relevent TinyG limit-switch.

4. To protect motors from damage set limit switches should be Velocity Max=400 mm/min. Yes its slow but thats a safe margin. On Z-axis set limit Min=homingand Max=Limit Only.

5. Emergency STOP button: easy peasy. Just plug it into the TinyG reset-pins.

6. I suppose ont can use a USB-based GRBL controller with Chillipeppr too. I bought a TinyG coz i wanted the best right from the get go.

TODO:

* Connect the Spindle to TinyG.

anyways, its an ongoing learning effort. Tomorrow maybe i will etch my very first real PCB.

I am kinda proud of myself. Got this far with only youtube, internet forums. The wife doesnt get it..

anyways, its an ongoing learning effort. Tomorrow maybe i will etch my very first real PCB.

I am kinda proud of myself. Got this far with only youtube, internet forums. The wife doesnt get it..

Awesome work so far. It's a very rewarding journey. My wife is never sufficiently impressed when I figure out how to build something either :lol:.

Main Thread updated with HOWTO info.

http://forums.eagle.ru/showpost.php?p=2689981&postcount=1

Small update.

I've been making a few PCBs on my Chinese CNC 3040Z-DQ machine.

What i learnt sofar;

1. The drillbits of 0,1mm quickly wears out to >=0,5mm :(.

2. Level surface of a pcb of 12x15xm is a challenge. The surface equality can differ upto 1,5mm.

3. Tuning the precion was/is a challgenge, espcially calculating revolutions per minute.

4. When CNC'ing one should generate 'non_copper' gcodes. That will create a empty circuit path.

5. Software. Lotsa FREE open source stuff available such as FlatCAM and TinyG.

6. Drillbits Using a brand new V-shaped drillbit 0,1mm gives best results.

UPDATE 23-6-2016

the below PCB was made.

Bit used=v-shaped 0,2mm tungsten carbide

carving depth=0,1mm (takes only copper away)

carve speed=280mm per minute

Track spacing=0,6mm

Track width=0,8mm

Gcode generator=FlatCAM 8.4 (open source)

FlatCAM CNC file used=xxxx_noncopper_paint_cnc.nc

Material=1,65mm thick copper plated board

IMPORTANT: The drill area was autolevelled using tinyG before start. Therefore less broken drillbits ;).

Settings of the CNC 304Z-DQ using a TinyG Motion Controller; [nema 23 steppers]

Motor X, Y & Z micosteps=eigth

Motor X, Y & Z stepangle=1,8

Motor X, Y travel per revolution=4,1

Motor Z travel per revolution=4,01

The result below:

Using TinyG's auto-levelling feature, small differences can be compensated therfore always milling exactly -0,1mm.