Gerber to GRBL: Current state of the art to mill PCB on desktop CNC?

[torch]

Background: I tinker for my own use, I don't make batches of things requiring multiple boards. I have made PCBs by etching in the past, but generally just dead-bug wire pre-drilled prototype boards.  I also tinker with 3D printing and now milling with a desktop CNC router, designing things in FreeCad. So why not step up my game and mill my own one-off boards?

The weapon of choice for designing the PCB layouts seems to be KiCad. I've downloaded the latest stable version (10.0.5) and reviewed some tutorials. I'm sure I will make some mistakes but think I can get the design part. Now researching how to get from design to actual PCB. There is a FC workbench called "Kicadstepup", but it seems oriented towards 3D printing an enclosure for the finished board rather than milling the copper traces. And all the tutorials I've found reference earlier versions of both FC and KC.

Realthunder has a linux console-only script called "fcad_pcb", but it's written for FC v0.17. The CAM workbench didn't even exist back then, AFAIK it is oriented around the old PATH workbench.

There's also a program called "Flatcam", which seems to be exactly what I want but again, all references are dated, there are some that suggest Flatcam is not compatible with current Python releases and the latest (Windows 64) release I can find is dated 6 years ago. Near as I can tell it's still looking for Python 2.7. 

At the moment, the only possible option I can see is to export the trace files from KC to FC and manually create toolpaths for each trace individually in the CAM workbench. Which seems rather a step backwards. So I'm looking for guidance from people with current knowledge and experience.

[langwadt]

So why not step up my game and mill my own one-off boards?

professionally made boards are so so much better, and so cheap that it is probably less that what it will cost you in worn out tools

[Doctorandus_P]

I mostly agree with langwadt. You can't compete with low cost professionally made PCB's with metalization, solder mask and silkscreen on both sides. And as a result, there is not much interest anymore in DIY milling PCB's.

But that said. There is nothing "wrong" with milling PCB's. It's relatively common for fast prototyping (You can have a new prototype in 15 minutes, instead of a day). I also once read about a radar installation (20GHz or so) where the milled prototypes worked, but the etched production PCB's did not. Apparently the root cause was signal reflections of the uneven sides of the etched tracks. One manufacturer that specializes in milling machines for PCB's is LPKF.

I've built my own CNC mill and one of the motivations was for quick prototyping PCB's, and for trying out "weird" things. The machine I built should be good enough to run a 0.2mm endmill between tracks, so I can also use "normal" design parameters for a regular fab. I even designed one PCB with milling in mind (bottom 100% GND plane, only GND via's). And then...

I have gotten flatcam to run on my previous linux box. Built a new PC about 3 years ago and after that I never bothered to even start flatcam. From what I remember, I had to fiddle around with one of the latest beta versions of flatcam. Older versions were not usable. flatcam also has a very convoluted user interface that I could not understand. Another problem with flatcam is that it left a big number of tiny dots of copper. (And other / more bugs). For things that should be simple you had to hunt around in 30 different menu's.

Tried to start flatcam just now (installed some 10 python dependencies, then got stuck on a "svg" for which I don't have an equivalent)

I've read someone being happy with "coppercam". But that's commercial and windoze only.

Maybe "pcb2gcode" is a usable program. It's a relatively simple file command line utility to convert files, but apart from that I never really tried it.

The machine I built runs on GRBL, and I have milled a few objects by using bCNC to control the machine. I quite liked the capabilities of bCNC (Such as DXF import, adding offsets and tabs, and more) but bCNC is also a bit primitive in other ways. And like flatcam it is also severely lacking in the maintenance department.

[torch]

I mostly agree with langwadt. You can't compete with low cost professionally made PCB's with metalization, solder mask and silkscreen on both sides. And as a result, there is not much interest anymore in DIY milling PCB's.

Not the news I wanted to hear, but kind of what I feared.     PCBway seems to sponsor half of YouTube these days, a sign of the times I guess. I can see the value of those services for those that are producing limited runs of niche products that don't warrant the investment to do it in-house. But I'm strictly a one-off home hobbyist. Everything I do is basically a prototype. None of it is SMD. The CNC router was acquired to support my metal working efforts; small, complex parts like a replacement timing gear for my wife's sewing machine. I just figured since I have it anyway...

I had a quick look at Coppercam. It does seem like what I'm looking for in terms of capability. I think. Not much documentation on their website, but there are a couple of YouTube videos with demonstrations. The pricing is rather steep for my anticipated usage but I may give the demo version a whirl just to try it out.

Thanks for your comments.

[elektryk]

I tried it https://copper.carbide3d.com/ but I still prefer photoresist film method or JLC...

[torch]

I tried it https://copper.carbide3d.com/ but I still prefer photoresist film method or JLC...

Interesting. Still a Beta according to their video, single sided only but looks dead simple to use. Except for the possible need to manually edit the g-code. I'll try that and see how it does.

[Doctorandus_P]

Last afternoon I spend a few hours to attempt: KiCad -> FreeCAD (KiCad StepUp workbench) -> CAM workbench. And this mostly failed.

(The way I understand The CAM workbench is not new, it's just a rename of the "PATH" workbench).

I can import the track geometry with KiCad StepUp, but it turns up to be a different object type in FreeCAD then I'm used to (From the "Parts" workbench instead of the "Parts Design" workbench), and I can't figure out how to manipulate those objects in a sensible way.

I've also been struggling with the setup of milling tools. I may be able to figure that one out eventually, but at the moment it still feels convoluted and confusing.

[torch]

Last afternoon I spend a few hours to attempt: KiCad -> FreeCAD (KiCad StepUp workbench) -> CAM workbench. And this mostly failed.

(The way I understand The CAM workbench is not new, it's just a rename of the "PATH" workbench).

My understanding is that while the workflow between the two is very similar, much of the underlying code was re-written. Macros, etc. that worked with Path are broken in CAM. However, I got into that after CAM came out and never used Path.

I can import the track geometry with KiCad StepUp, but it turns up to be a different object type in FreeCAD then I'm used to (From the "Parts" workbench instead of the "Parts Design" workbench), and I can't figure out how to manipulate those objects in a sensible way.

From what I've read, FC and KC use .step format to exchange files. Part WB, Assembly WB, etc. all work directly with solids, but Part Design does not. I assume if you want to use it in PD, you have to treat it like any other solid: import it, highlight it then create a body. PD will then create a new body with a "Base Feature" parametric version.

But I understood that CAM works just fine with step files too. Shouldn't need to import it into Part Design. That said, I've never tried it. I rarely import things into FreeCad. 

I've also been struggling with the setup of milling tools. I may be able to figure that one out eventually, but at the moment it still feels convoluted and confusing.

I struggled with that at first too, but I'm slowly getting the hang of it. It's hierarchical. Tool is at the bottom of the totem pole and just describes the tool itself. Tool Managers define how the tool is being used in a particular circumstance. It kind of make sense -- the same bit could be used to mill steel or aluminium but the speeds and feeds would be different. You can define a Tool Manager for use in aluminium and a second one for steel -- or in this case, copper-clad PCBs. At the top of the hierarchy is the operation, where you define the path the tool will take. And can override the default settings from lower tiers. 

Definitely designed by a committee.   

[ftg]

IMSAI guy just did a video about his Kicad to milled PCB workflow.
He seems to use FlatCAM.

[Doctorandus_P]

I have had success. Just drew a PCB on paper as a first test.

At first I tried get along with the FreeCAD CAM workbench. I managed to get some CNC vectors / G-code, but I had to add each track and pad manually to the list of things to be processed, so that was a no go.

While searching for tutorials, I (re) discovered the video from Mattias Wandel (A.K.A. "WoodGears"). He wrote a Python script with some help of AI and debugged it in 3 days, so it is a bit "rough", but I was curious so I cloned his repository and ran the script, and it created a G-code file. Looked promising...

Next step was bCNC. It did not start "immediately", and as it's mostly unmaintained I did not want to invest a lot of time in it, so I had a look at Candle. Cloned the candle repository, and compiled it (lots of errors about obsolete functions), but the compile did run to completion. and I could start up Candle.

This is the first time ever for me to install / run Candle, so I still have to get used to it. After experimenting a bit It looks like a quite usable program. So the next step in testing was to replace my milling spindle with a ballpoint pen and I ran the G-code which was generated by Mathias' script.

By default the script is configured to do 3 passes with a 0.2mm offset, and that is (mostly) OK for my machine.  It also removes the sections where there is not enough room for those three passes, and that is also promising.
For my test PCB I had to reduce "offset_distance" to get the script to route in between SMT pads with a 250um clearance, and that also worked as expected.

I also already discovered a few problems. Some pads of a THT connector are missing, and zone boundaries seem to be treated wrongly, and they get milled on both the inside and the outside of the boundary.

But overall, it looks quite promising.

At the moment the script only does single sided PCB's.

There is no licensing mentioned in Matias' repository at all. It seems obvious he want to share it, but the legalese is messy.

Links I used:


https://github.com/Matthias-Wandel/Gerber2nc
https://github.com/Denvi/Candle

[torch]

I have had success. Just drew a PCB on paper as a first test.

At first I tried get along with the FreeCAD CAM workbench. I managed to get some CNC vectors / G-code, but I had to add each track and pad manually to the list of things to be processed, so that was a no go.

While searching for tutorials, I (re) discovered the video from Mattias Wandel (A.K.A. "WoodGears"). He wrote a Python script with some help of AI and debugged it in 3 days, so it is a bit "rough", but I was curious so I cloned his repository and ran the script, and it created a G-code file. Looked promising...

I watched that video as part of my research. As you say, it looks a bit rough, but may be an option. Your findings on using FC CAM pretty much concur with what I thought -- doable one track or pad at a time. Seems ridiculous. Unless we're both missing something. The one advantage I can see about using FC is that the model will already be loaded, ready for enclosure design.

I have Candle. The latest (which as you say, is not particularly current) came on an SD card along with some sample .nc files included with my machine. It is current enough to require Python 3.x (significant in a moment). I've used it and found it a reasonable useful controller. The other really popular one -- and is currently maintained -- is UGS (Universal G-code Sender). Also requires Python 3.x. A few more bells and whistles compared to Candle, but ultimately both get the job done.

I don't use either one. Both require a computer to be tethered to the CNC router as they are directly sending the G-code line by line. As I said earlier, my principle use is milling aluminium parts -- lots of flying metal chips. Not good for the computer! Not something SWMBO wants in her house! I do have an old WinXP laptop I was wiling to sacrifice as a dedicated controller, but it won't run Python 3.x. I did manage to find an older version of Candle compatible with Python 2.x, but it has some bugs.

Ultimately, I settled on an "Off-line controller" -- a stand alone device. It's touch-screen, so no keyboard to trap swarf. I can send the .nc or .ncg file via wifi to the controller out in the shop (it has a primitive web server). It can store up to 11 macros for things like probing. In the shop, I can do all the essentials like zeroing out the axis, select files, start/pause/stop, adjust speeds and feeds on the fly, etc. Rather like a 3D printer. It doesn't offer a live graphical display of the tool path, but it does show live numerical display of the axis.

It's also an example of my level of electrical engineering expertise. Or perhaps more accurately: lack of expertise; I know just enough to be dangerous.  But I did manage to figure out the controller has a 5v UART interface and the machine has a 3.3v RXD/TXD + a 5v supply. And they both can handle 115200 baud at the common 8N1 pattern.

So I dug out a suitably sized piece of perboard, an AMS1117-3.3 mounted on a little board with a TO220 through hole adapter, an 8-pin 2 x 4 IBC socket and an Adafruit 4 channel I2C compatible level converter and started soldering in jumper wires. Housed it all in a 3D printed enclosure designed in FreeCad.

It is this very circuit that I chose as my first foray into KiCad. I spent 3 or 4 hours last night working on this and am now at the point of starting the actual PCB layout. Along the way I learned how to change the default SMD footprint of an AMS117-3.3 by selecting a TO-220 footprint instead. I learned how to add an Adafruit library because the default doesn't include their products. I learned how to search out and download a specific level converter board created by a third party from Github and install that because Adafruit neglected to include that particular product in their library.

My old way was definitely faster! 

[Doctorandus_P]

I really like PC connectivity in my CNC machine. Recently I bought a brand new Mobo + Memory for building a LinuxCNC machine. Chips are an issue, but by putting the PC in a closed box and a bit of filtering it's not a huge deal.

You can very likely run Linux on your old XP laptop. Linux comes by default with Python pre-installed. Trying out linux is as simple as downloading an image, putting it on an USB stick and then booting from the USB stick. This does not install anything on the PC, so you can just try it out so see how it works. I'm running Linux Mint myself, and it's also a good beginners distribution. It "just works" without having to fiddle with a lot of things.

Here in the EU, it's also very easy to second hand PC's for small prices (Starting around EUR 100). Very often this is "ex office" equipment that just gets replaced every 3 or 4 years. Such PC's have a lot of life left in them. My own PC (Ryzen 5600G) is now 3 years old (I think), and I plan to use it for another 10 years or so.

Yesterday I looked a bit at forks of the Wandel script. Axolito added support for mirroring and bottom layer milling. both hwelch-fle and gasparini added support for command line parameters, but I get completely lost in the gasparini branch. It claims to use "python best practices". but adds a makefile (Yuch) installs some "virtual environment thing", and after "compiling" (which it goes though without trouble) I can't figure out where the final program is or how to start it. Gasparine also just slapped a MIT license on Mathias' code (Original code does not have a licence at all) And this is also quite dubious. Apparently there are 9 forks, but I can only link to 4 of them on gitlab. Confusing.

Are you capable of (or interested in) a bit of Python programming? I am thinking myself of figuring out what is going wrong with the zones, and adding support for the (oval) pads that are now missing. But my mind is chaotic and slow, so no promises.

More important for me is to upgrade my CNC machine. It's still running on an STM32F103C8T6 (Blue Pill, from when those were still real). And F103 is deprecated in the GRBL-hal branch. Too small, too old. I have already bought some Teensy 4.1 boards (With Ethernet) a few years ago with the intention of putting GRBL-Hal into it. But I am very good at procrastinating.

Also: With ethernet, you can put a long cable on your CNC machine. You can put it in a cellar, in the attic or in a shed, and still keep an eye on it with a camera.

KiCad is good. I've been using it for over 10 years now. I mostly draw schematics, have not ordered many PCB's yet. But I also do use the PCB editor for footprint placement on one-off projects that I build on matrix board. For those I do the footprint placement and ratsnest optimization, maybe draw a few tracks too, but certainly not all of them. When soldering on matrix board, you can have many "layers" of wiring I do use 0.2mm enameled wire for soldering such boards. Much easier to work with then with wire you have to strip the insulation off of.

[torch]

IMSAI guy just did a video about his Kicad to milled PCB workflow.
He seems to use FlatCAM.

Interesting. He's got almost the same CNC machine as I and his laptop appears to be running Win 10 or 11. So clearly it's possible to run Flatcam on a modern OS.

[torch]

I really like PC connectivity in my CNC machine. Recently I bought a brand new Mobo + Memory for building a LinuxCNC machine. Chips are an issue, but by putting the PC in a closed box and a bit of filtering it's not a huge deal.

The one advantage of using the PC as a controller is the ability to generate a mesh to accommodate a warped surface. Not an issue when milling aluminium parts but a potential issue when creating a PCB trace.

You can very likely run Linux on your old XP laptop. Linux comes by default with Python pre-installed. Trying out linux is as simple as downloading an image, putting it on an USB stick and then booting from the USB stick. This does not install anything on the PC, so you can just try it out so see how it works. I'm running Linux Mint myself, and it's also a good beginners distribution. It "just works" without having to fiddle with a lot of things.

My exposure to Linux is limited to things like computer routers rather than as a PC operating system. But from the outside looking in, it appears to me that there is no such thing as "Linux". There are a whole raft of contenders for the title with names like "Ubuntu" and "Wine" and "Fedora". Some things run on one, but not another. Then there's the whole issue of drivers and hardware compatibility. I love the idea of Linux but it seems a daunting challenge to make a go of it.

Are you capable of (or interested in) a bit of Python programming?

I have very limited C+ programming skills. And very limited skill in the Arduino variant. Never tried Python.

Also: With ethernet, you can put a long cable on your CNC machine. You can put it in a cellar, in the attic or in a shed, and still keep an eye on it with a camera.

When I renovated my current home 30 years ago, I ran CAT 5e into every room of the house (but not the shop) from a 24 port hub. Very leading edge. Shortly thereafter WiFi 2 was released and the cables quickly became redundant. Now the only cables in use run from the fiber bridge to the router and from the router to the television. The shop has a Wifi extender.

KiCad is good. I've been using it for over 10 years now.

It looks very powerful. Any problems are likely PEBKAC.

[Doctorandus_P]

Congratuations. That is a relatively nice little router  (shown @09:10) . It's definitely a lot better then the EUR 400 things with the unsupported round guideways. This one has proper (although thin but that does not matter much) supported linear rails on it's X, Y and Z axis, and ball spindles on all motors too. I just also watched the earlier review from IMSAIGUY.

The thing I built is 80kg of steel. but something like this would be around the minimum I would dare to recommend to buy for a "beginner". And for around EUR 600 it's still quite affordable. (Cheaper routers can barely be called toys.)

https://www.lunyeecnc.com/products/lunyee-3020-nova-cnc-router

Anything you can do to improve stiffness in a router like this will improve milling results. The simplest you can do is:

• Remove the spindle motor.
• Set the Z axis in it's lowest position.
• Put the spindle motor back, with the "highest plausible" position in it's (round) bracket.

He is using an older version of Flatcam though: @06:46 Flatcam 2024.04 Version Date: 2024/04/15 And the title bar of Flatcam also shows it's a BETA version.

Concerning "linux", yes there are a lot of versions (called "distributions") but nearly all are based on different mixes of the same (preconfigured) software. And software is quite interchangeable between different distributions. With Linux, most software can be directly installed by your OS (which also handles updates). You don't have to go to the internet and find software on some website. The differences are mostly offloaded to the people who do the "packaging" of the software. And for starting, it's not something you have to worry about much. If you're ever curious to have a look at it, I recommend (again) Linux Mint. It's very friendly towards beginners. Just create an USB stick and boot from it. It's that simple to get started. But for a more serious evaluation, a complete install is a lot better.[/list]

[torch]

He is using an older version of Flatcam though: @06:46 Flatcam 2024.04 Version Date: 2024/04/15 And the title bar of Flatcam also shows it's a BETA version.

Sadly, I think it's the latest version. And a fork.

From what I can tell, Flatcam was available through bitbucket.org, which now only displays a zip of the repository. However, I did find an archive of the original on github (https://github.com/sasodoma/flatcam-archive). At the bottom of that page, he provides the original bitbucket links to each of the installers -- and oddly enough, those still function even though they're no longer listed on the bitbucket page. So I downloaded the FlatCAM_beta_8.994_x64_installer.exe using that bitbucket link.

The changelog suggests the last Flatcam release was 8.5 in 2019. I'm not sure what happened after that, but as we all know, the world changed in 2020. If the developer was one of the casualties, then may he rest in peace. Someone else picked it up and released a series of beta forks from 8.991 to 8.994 in 2024. Nothing since then that I have been able to find.

Anyway, it seems to have installed on Win 10 successfully. I haven't tried doing anything with it yet, but it opened without crashing.

[torch]

Ok, now what's wrong with this picture?



Actually, I know what's wrong with the picture, I just don't know why, if it's something I screwed up importing it into the library or a bug in the library. I don't think it matters ultimately since the footprint is correct.

NEVERMIND. I figured out how to edit and rotate the 3D model.

[Doctorandus_P]

In the screenshot of your KiCad 3D view, on the top there is: "Board outline is missing or malformed. Run DRC for a full analysis." And that is a quite important message. It means that KiCad does not know how big you PCB is, and the 3D viewer just guesses some dimensions based on where footprints are. To fix it, first select the "Ege.Cuts" layer and then use PCB Editor / Place / Draw Rectangles to draw a rectangle on that layer. The lines on Edge.Cuts must also form a "perfect shape", with no gaps, overlaps or lines crossing each other.

Concerning Flatcam...
Even if I had a version that starts up and "sorta works", I'm not sure I would want to continue with it. From what I remember, it's workflow is overly convoluted (especially tool management) and the generation of milling vectors also made weird errors. Combine that with the lack of maintenance and the overall complexity of the program, and it is beyond what I can manage.

https://bitbucket.org/marius_stanciu/flatcam_beta/src/Beta_8.995/

On gitlab, there are some 180 versions of flatcam. I had a short look at one of them (https://github.com/ProgLuis/FlatCAM9NeoS2) This one has received some updates this year, and the (translated (Spanish? Portugese?) introduction promised some modernization of the code. The install instructions are setting up some sort of "virtual environment" thing. I also saw that in Gerber2nc_gasparini. This seems to be an extra layer to make python more complicated. https://docs.python.org/3/library/venv.html ... But also: If it can run a specific python version, and also install packages for that python version and handle all the dependencies of the python script in that environment, then it may be a useful thing. But for me it smells like an extra layer of glue for people who are to lazy to keep their program code up to date.





The script from Mathias Wandel is also not perfect, but it's relatively simple and making some modifications is in the range of programming skills that I can manage.

[torch]

In the screenshot of your KiCad 3D view, on the top there is: "Board outline is missing or malformed. Run DRC for a full analysis." And that is a quite important message. It means that KiCad does not know how big you PCB is, and the 3D viewer just guesses some dimensions based on where footprints are. To fix it, first select the "Ege.Cuts" layer and then use PCB Editor / Place / Draw Rectangles to draw a rectangle on that layer. The lines on Edge.Cuts must also form a "perfect shape", with no gaps, overlaps or lines crossing each other.

I think the issue was the level shifter intersected the main board. Two objects occupying the same space at the same time. Once I rotated the level shifter board properly the error went away. 

I'm playing with that Beta of Flatcam right now. A bit confusing as the interface appears to have evolved since whatever version was being used in the video I watched. That said, once the tools are sorted it seems pretty straightforward. (I say that now, without actually having milled anything yet...  )

[Geoff-AU]

Timely thread!  I have slowly been setting up a Lunyee 3018 Pro Max and have milled a bit of wood so far.  One of the things I bought it for was rapid prototype or one-off PCBs.  I know I can order professional boards but CNC is a fun skill to learn  (I also want to engrave anodized aluminium front panels for projects so the enclosures look nice).

So far just been playing with FreeCAD and bCNC.  I have it set up with an Odroid N2+ connected via USB so the linux-based softwares will be of interest - FlatCAM looks great.

[Doctorandus_P]

Congratulations with your new machine, but the 3018 Pro Max is a very different machine from the 3020 Nova. It's the difference between a very low budget gadget to play with a bit, and a machine that is fairly decent. IMHO, if you can't afford the Nova, then it's better to save up some more money instead of buying that other one.

Another significant limitation of the "pro max" is the spindle motor. Putting an ER collet holder on a thin motor axle is very wobbly and causes a lot of chatter.

But still, for PCB's and 0.2mm endmills, cutting forces are very low, so you may still be able to get some usable results with it. Backlash is probably the biggest problem. You can possibly fix that by putting a pulley on the X and Y axis and then use some cord and two weights to pull the backlash in the same direction. (There are also constructions with double nuts and springs in between, or with adjustable double nuts).

[torch]

I had (well, still have. In a box) a 3018. Lots of videos out there with people using them to engrave PCBs. Let's face it, you don't need a Bridgeport to engrave 1/2 a millimeter of copper. It might even lightly engrave aluminium if the cuts are shallow and feed rate slow enough. Use cutting fluid and stick to T6061-T6. It's probably the most forgiving aluminium alloy for a beginner with a table-top CNC router. 

Backlash is definitely a problem though, even with spring loaded "anti-backlash" nuts. I drilled and tapped the flanges of mine for M4 set screws, two per nut, so they maintain the distance between the two halves rather than relying on a spring. Manually adjust out the backlash without excessive drag and lubricate the screw with machinist's way oil. Lock the adjustment with a locknut or thread locker. Makes a world of difference.

[Geoff-AU]

3018 Pro Max

I misspoke, it's the Pro Ultra I have (X-axis linear guide).  The Nova has all 3 axes on linear guides and a better motor so yes I'm sure it would do a much better job.  I got the Ultra on a pretty good promotion. I also bought the 10W laser option (and a pair of real laser safety glasses for $250) as I'm keen on doing some laser engraving and at the price of the CNC I don't trust any safety measures they've taken.  If I get into machining more then yes its shortcomings will quickly become evident.  The motor is pretty "meh".

[elektryk]

3018 PRO with plastic Z Axis Assembly is really frustrating due to absolute lack of stiffness.
https://www.eevblog.com/forum/mechanical-engineering/cnc3018-upgrade-it-or-replace-it/msg6153811/#msg6153811

I could do only PCBs with really big clearances.

[torch]

3018 PRO with plastic Z Axis Assembly is really frustrating due to absolute lack of stiffness.
I could do only PCBs with really big clearances.

I strongly suspect the bigger problem is excessive backlash. The "anti-backlash" nuts are pathetic, even with the spring compressed to maximum. I modified mine with manually adjusted setscrews. The holes are just about perfect for M4 screws: