Elektroda.com
Elektroda.com
X

Search our partners

Find the latest content on electronic components. Datasheets.com
Elektroda.com

Milling PCBs designed at Eagle

malyjasiu 30486 41
This content has been translated » The original version can be found here
  • I decided to write this guide, because you can't find anything about it on the net (or I'm not doing a good job searching).
    There is a lot about some bizarre indirect methods using software that you don't know where to get. And this method is simple and effective.
    The guide is the end result of a whole pile of wasted tiles, but I do not regret it, I will reflect on chemicals :)
    To the point



    1. Download the pcb-gcode.ulp plugin from the Artsoft website (or from the attachment). http://www.cadsoftusa.com/downloads/ulps?language=en
    Works with Eagle version 5 and 6.
    2. Unpack and copy to Eagle / ulp directory
    3. Run Eagle, on Vista and 7 systems run as administrator.
    4. Not a word about design, I assume that we already have the board design ready - open it.
    5. Remove unnecessary layers from the PCB designed in the Eagle program, leave only the bottom, pads and vias (the guides will probably be useful).
    Of course, I assume that we mill the bottom side.
    6. Press file and select the run command - the window with ulp plugs will open (you can press the ULP icon on the main bar).
    7. Now select pcb-gcode-setup.ulp - this will allow us to set the milling parameters.
    8. In the Machine tab, set the units to millimeters, and go to the Generation Options tab.
    9. In the first Generation Options window, select the page to be milled. In this case we check Generate bottom outlines and Generate bottom drils, and we deselect Generate top outlines and Generate top drils. We also mark Mirror. We introduce parameters
    in the board window:
    show preview (optional), spot drill holes -0.254, minimum 0.00254 mm; Maximum - 0.01 mm; Step size - 0.127 mm. We do not use commas,
    only dots - American system.
    10. Machine tab. Z High - the height of the safe transport of the tool can be 5 mm. Z Up - how much the tool will lift when changing position without milling, we give 2 mm. With Down - how deeply it will mill the copper - I set it to -0.17 mm. You can set deeper, but such thin cutters are tapered,
    so they will widen the milled area and the board may not come out. We set the drill depth to -1.8 mm (it should be enough, if we had a thicker laminate, we set more). Drill dwell - 0.1 (time to stop the cutter in the hole in seconds). Position X and Y zero. Position Z 10.
    11. Mark GCode style tab Mach.
    12. Press Accept, and finish setting. We confirm OK and once again Accept. The rest of the parameters remain the default.
    13. Find pcb-gcode.ulp and click twice.
    14. In a moment, the program will generate two files placed in the same directory as the board project projekt.brd.
    These will be files: project.bot.drill.tap and project.bot.etch.tap. These are files already accepted by the Mach program. Preferably instead of dots in the middle
    put underscores in the names, because mach sees them right away.
    15. Now it would be good to check the board for errors. For this I used the older, free version of CamBam.
    Operation very simple, at least when it comes to the preview.
    If the honorable commission did not find any errors, we start milling the insert. Do not underestimate this check, especially if the distances between paths in the project are small. Then the adjacent tracks or pads can "merge" with each other. Then you have to correct the design.
    16. First, upload the project_bot_etch.tap file and install a 0.2 mm cutter. Where the G-code will start, you have to check it "dry".
    Usually it is near the lower left corner.
    We will set the cutter to "0" and continue as in Mach - reset all positions and start. The milling machine will replace the litter box with chemicals.
    17. When it is finished, pick up the tool so that it can be replaced with a drilling cutter. Then we set it to zero in the X and Y axes (the place where the program started milling).
    Reset the Z axis after a tool change. In order not to manually set the zero in the X and Y axes, you can add in the file projekt_bot_etch.tap
    (on the second line, the last nodes after the Z position, X00.0000 Y00.0000).
    When we have everything set up, upload the file projekt_bot_drill.tap and start. The milling machine will now drill all holes.
    Here is an example of a printed circuit board for Atmega_fusebit_doctor of my friend's manekinen (thanks),
    which doctor I'm about to do.
    The board is milled with a 0.2 mm cutter, flat face. Holes drilled with a 0.7 mm cutter. If you need to enlarge one of them, I will do it with a tiny hand drill.
    No problem if there are pilot holes. After the whole operation, smooth the tile with 1000 sandpaper to get rid of the hail on the edges of the paths.
    I took pictures and only realized that I hadn't checked the mirror option, so the board came out wrong - in the mirror. But now that the method is fine-tuned, I'm about to make a new plate. I just don't take a photo, because I gave the camera back. Mobile photos are not suitable for publication. The disadvantage of the method are the fields of unmilled copper remaining between the tracks. For now, I do not know how to get rid of it, maybe I will come up with something, then I will add a sequel.
    I just need to buy a laminate :) . All the supplies went to the experiments.
    In the attachment the CamBam program, which in the free version is already difficult to get. The author has withdrawn it from his site, he only has the paid versions there.
    In the second, a plug for Eagle.

    Milling PCBs designed at Eagle Milling PCBs designed at Eagle

    Cool? Ranking DIY
    Can you write similar article? Send message to me and you will get SD card 64GB.
    About Author
    malyjasiu
    Level 19  
    Offline 
    malyjasiu wrote 235 posts with rating 79, helped 32 times. Live in city Bydgoszcz. Been with us since 2007 year.
  • #2
    dudik56
    Level 15  
    I was just trying to mill the tiles and my friend's article fell out of the sky. It's a great idea to gather this information in one place.
  • #3
    kowal011
    Level 21  
    And let a colleague write how long it takes to mill an A5 formatted smd board? It's about the profitability of such a game. The preparation of the project takes the same amount and the execution itself (in time) is in my humble opinion inadequate to the final result.
  • #4
    Komar91
    Level 18  
    What program are you using to control the machine?
  • #5
    dudik56
    Level 15  
    Have you figured out the milling of tile contours? I mean some strange shapes and possibly inside a plate for mounting larger elements. Milling in a rectangular insert may be inefficient compared to other methods, but also milling some fancy contours in combination with drilling holes gives this method an advantage over other amateur methods.
  • #6
    malyjasiu
    Level 19  
    Buddy Kowal011: The time it takes to mill a tile depends on the speed of the machine. At a feed rate of 1300 mm / min, the plate presented in the photo was milling about 10 minutes. Drilling took about 6 minutes. Compared to etching, it comes out faster, please pay attention to the holes. I've done a lot of tiles in my life, but I've never been able to drill holes so cleanly by hand (even with a stand). A resistor is inserted into any plate, drilled anyhow. Worse with the integrated circuit. And in this PCB, the DIL stands are simply inserted. They fit perfectly.
    Komar91: prv
    dudik56: it is impossible to cut out the contours directly in one go, the ULP plug does not provide for this. But there are several ways to do this. The first is to design any shape in ArtCam. Then just cut it. Of course, how is ArtCam. You can do it in LazyCam, which is included with Mach3 with a full license, but I don't know how, because I don't use this program. I studied on ArtCami. You can also design a plate by hand in Eagle with only the contours to be cut drawn on the bottom layer. Set Z Down to the thickness of the laminate (e.g. 1.5 mm) and process with pcb-gcode.ulp into a cutting file according to the recipe given at the beginning. Looking at CamBam, we will see that the program will want to cut a double line, because it is supposed to make paths. But unnecessary pieces will fall off anyway. All you have to do is adjust the line placement to get the desired end result. And it's better to change to a cylindrical cutter, it will cut nicer. Clamping the insert on the milling table can be a problem, especially with a complicated pattern. Maybe double-sided adhesive tape? I still use a furniture board washer attached to the table, mainly due to drilling. And there is no problem with cutting a rectangle - I do it by hand - it's probably faster than making a g-code. As the board is attached to the sides with clamps, there are no problems with cutting the rectangle outline. I haven't tried any other figures yet.
  • #7
    1996arek
    Level 20  
    The design may be nice, but diligence is not. The paths are a bit crooked. Why has this happened?

    malyjasiu wrote:
    A resistor is inserted into any plate, drilled anyhow. Worse with the integrated circuit. And in this PCB, the DIL stands are simply inserted. They fit perfectly.

    Something. A colleague did not try. Even for a PCB made with a marker pen, the layouts fit perfectly. Not to mention thermotransfer. Drilling good holes is also not difficult. It all depends on your willingness and tools.
  • #8
    Jerzyczeka
    Level 17  
    A great tutorial, and the shape of the paths depends more on the rigidity and accuracy of the machine. I may have a silly question, but how do I open a pcb file in eagle? I have never done it and I just want to convert pcb files downloaded from the internet to gcode. All I see is a text file, no paths.

    best regards
  • #9
    kaytec
    Level 20  
    Thanks for the article. My first test:

    Milling PCBs designed at Eagle Milling PCBs designed at Eagle Milling PCBs designed at Eagle Milling PCBs designed at Eagle Milling PCBs designed at Eagle Milling PCBs designed at Eagle

    Board from mdiy.pl (component tester). A bit too deep in the corner, you can easily go to a depth of -0.05, there should be no problem with larger SMDs. I don't have a drill, but I already know I have to.

    From the problems, the code is generated in the minus of the X axis and about 20 mm in the plus in Y.
  • #10
    yogi009
    Level 43  
    Interesting topic, but for me it is rather a curiosity. Perhaps it makes a bit more sense with short bursts. Making precise paths and drilling (without a stand) holes for DIL and SIL housings is not a problem. It's a matter of training. Same as the quality of the soldering points. Looking at the photos I get the impression that the milling is too deep, but here I am a fanatic. In any case, chemical etching in my opinion gives better qualitative results. I do not know what the subject of precision of these cutters looks like, whether you can, for example, make 8-10 mils class paths and 4-6 mils intervals. In each installment, chemical etching certainly allows you to obtain such results, and with the use of the photochemical method, you may be tempted to go even "lower".
  • #11
    Komar91
    Level 18  
    And I have one more question: I followed the instructions from the first post and the program generated only the outline of the paths for me, and skipped the subtitles made on the top layer. I wanted to make a sample board for testing and choose unnecessary copper. Can anyone tell me how to set it up in this script? My example is attached. (I can't attach an attachment so I will paste a picture of the eagle Milling PCBs designed at Eagle )
  • #12
    sasii
    Level 10  
    dudik56 wrote:
    Have you figured out the milling of tile contours?

    Generate milling must be selected.
    Make the outline of the pcb board with a Milling layer
  • #13
    Lechito
    Level 12  
    I'm having trouble generating the top layer.
    In the settings, I select generate top outlines / drills, but it still generates only the bottom layer for me.
  • #14
    tomastom
    Level 11  
    Hello.
    Is there any Polish description of the CamBam program functions?
    best regards
  • #15
    Bartosz Lichtarowicz
    Level 12  
    Hello! He's been doing circuits on a machine I've built for some time. I used to make tiles even on a larger scale using the photo method. I had a digestion unit, the platesetter is still somewhere in the garage, etc ... At the moment, there is no way I'm going back to chemistry. Just as you need to practice with an iron and a marker pen, you also have to learn some things with the CNC. A colleague who has been making plates with thermal transfer for many years admitted that he has no chance, it is about speed, quality and repeatability. I am using Eagle and Pcb-Gcode for design. The machine mills, drills holes, cuts tiles and cuts masks for solder paste, although I prefer the latter to my colleague on a laser engraver if it is not to be thin alu. For precision, see the photos. If anyone has questions about pcb-gcode, I will be happy to help.
    Bartek.
  • #16
    Łokasz
    Level 16  
    Hello,
    I'm having trouble generating gcode. After performing the activities in accordance with the above instruction, only the * .bot.etch.tap file is generated for me, but the * .bot.drill.tap file for drilling is not generated. I am using eagle 6.1.0 and pcb g-code 3.6.0.4.
    Maybe someone has encountered such a problem and knows how to solve it?
    Thank you and best regards.
  • #17
    Bartosz Lichtarowicz
    Level 12  
    I have never had such a mistake. I'm using version 3.6.2.4 try to install a newer version again because it looks like something is missing. Alternatively, send me the eagle file, I'll check it at my place.
  • #18
    Łokasz
    Level 16  
    Hello,

    after installing the latest pcb gcode 3.6.2.4 it kicked Java errors. After installing Java, I am also unable to generate the code.
    I am asking for help in generating the files. The project is attached.

    A question to my friend Bartosz L. what are the eagle pcb and PCB g-code settings, that the path outline is made and the boards are so amazing! As for me, the effect is very good.

    Thank you in advance for your help and best regards
  • #19
    Bartosz Lichtarowicz
    Level 12  
    to Luke. I will not tell you anything about mistakes, you definitely have something dug up in your computer. The Eagle staff bow to your project. I recommend some courses that are full of online. I improved the project. In the attachments the result files, brd and pcb-gcode settings for this project, because it cannot be done once and for all. The settings are different depending on how we want to mill and what effects to achieve.
  • #20
    Oineh
    Level 20  
    I also had Java bugs, but only when I chose the show preview option. When I checked this, everything is generating nicely. I wanted to check this method when making pcb on aluminum supports.
  • #21
    maglo18
    Level 11  
    I did according to this tutorial, I will ask here. I arranged everything according to the guide. The paths of the upper and lower layers are generated correctly, but I have a problem with holes. As I look at the g-code of the holes, the positions are visible for each of them, the problem is that the cutter is lowered at the first and lifted up after the last hole, which results in the destruction of the plate. There is no pick up / drill for each hole. Has anyone encountered such a problem? I am using eagle version 7.6 and also tested version 6 without any changes. I generated my tiles and used by the author of the thread.

    Milling PCBs designed at Eagledrill ea..e.PNG Download (106 kB)
  • #22
    robo1973
    Level 15  
    Can you cut the plate with this plugin?
  • #23
    LA72
    Level 40  
    There is currently another interesting insert milling tool from Eagle.
    FlatCAM supports Gerber files that can be exported from Eagle without too much trouble.
  • #24
    madiz08
    Level 14  
    Hello
    I'd like to refresh the topic by asking a question about hole generation that has not been answered. As my colleague "maglo18" wrote, the paths are generated correctly, but the Gkod for the holes is incorrect. A great thing with generating paths, the tiles mill perfectly, but has anyone managed to properly generate the file with holes?
  • #25
    noel200
    Level 25  
    I always generate a file with holes without any problem. You have something wrong in the ulp setup file.
    And the contours and strokes are also great.
    You need to draw them on the milling layer with such a turquoise color and select the appropriate option in the ulp settings. Then the program generates an additional file. And we need the right cutters.
  • #26
    madiz08
    Level 14  
    I was about to give up with these holes looking for a different program, tried everything in ULP SETUP and nothing, finally running EAGLE as administrator and the board generated with holes. Due to the fact that the cutter is conical, I set the drilling to 0.1mm, which only causes a guide, and I countersink with a drill.
    Thanks for the answer because without it I would have given up and not deliberate
  • #27
    slawko_k
    Level 34  
    Hello.
    It also makes me wrong with the drilling file.
    However, running in administrator mode does not help.
    In addition, when I give a mirror, it makes me the wrong file from the blue layer, and when I uncheck the mirror, it does the right one, but it also reflects 0 of the machine to the bottom right corner.
    How to fix it ??
    Eagle 7.2 pcb 3.6.0.4
  • #28
    lukaszd82
    Level 30  
    Does the author have an idea what to do so that the holes are not moved in relation to the paths? For 3 tiles, there is always a shift of 1-3mm (always along the x axis), which disqualifies the tile. If I manually shift the wx dimension by spr, the tile comes out ok. But you have to set the shift by hand each time. Where does it come from, since both files are generated according to the same point. zero? I only change the tool and unfortunately it's crap ...

    When it comes to not generating a file for holes, you need to select "use simple drill code" in the Gcode Option tab. At least for me it is required.

    So far I have found a newer pcb-gcode 3.6.2.4
    I will include it in my CNC topic if it works.
    As if I will describe my fight with this topic here :)
  • #29
    k_party
    Level 2  
    If anyone is interested in a simple gcode generator from bmp. You can also properly scale the generated PCB image in my program and save the Gcode in the correct size.

    I have not used Eagl for a long time - because it is enough for me. The thread on how the program was created can be found on cnc.info

    I don't remember if you can provide links here. In any case, you can find it here: cnc.info.pl/program-bmp-to-g-code-t59454.html

    The program is completely free - that's why I'm putting it here. Maybe it will be useful to someone. It is useful to me very often.
  • #30
    neo62
    Level 16  
    And I have a question how to reset the drill after changing from the cutter? I mean height exactly. I dealt with the position in general with the command G28 X0 Y0 Z0. But the cutter and drill bit are of different lengths. How to do it?