# GCodeClean hits v1.0.1 🎉

**URL:** <https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995>\
**Category:** Software\
**Tags:** gcode\
**Created:** [May 7, 2022, 7:05am UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995 "2022-05-07T07:05:46Z")\
**Posts on this page:** 20\
**Page:** 2

<div class="post-metadata">

**Author:** ![md8n](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/md8n/32/28197_2.png) [@md8n](https://forums.maslowcnc.com/u/md8n)\
**Post date:** [July 31, 2022, 1:48am UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/21 "2022-07-31T01:48:03Z")

</div>

I’d like to see that run through GCodeClean. I’d really appreciate a sample of the code if you’re willing to share.

---

<div class="post-metadata">

**Author:** ![md8n](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/md8n/32/28197_2.png) [@md8n](https://forums.maslowcnc.com/u/md8n)\
**Post date:** [July 31, 2022, 1:51am UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/22 "2022-07-31T01:51:06Z")

</div>

I’ve had the convert `G1` with +ve z-axis values to `G0` for some time now. But I have noticed that they’re doing -ve to +ve transitions on the z-axis with other motion as well. Now that’s kinda normal for many scenarios, but it seems they’re doing it a lot. So I’m in the process of tweaking the `G1` to `G0` conversion to make it better able to handle these transitions.

---

<div class="post-metadata">

**Author:** ![jonatpridesleap](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/jonatpridesleap/32/6639_2.png) [@jonatpridesleap](https://forums.maslowcnc.com/u/jonatpridesleap)\
**Post date:** [July 31, 2022, 1:48pm UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/23 "2022-07-31T13:48:29Z")

</div>

> [@mooselake](#):
>
> GCodeClean may have become very interesting to Fusion 360 free users

pardon my ignorance but im curious as to what GCode Clean does. I am a F360 user but am not sure what GCC actually does and how it would be helpful to me.

---

<div class="post-metadata">

**Author:** ![md8n](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/md8n/32/28197_2.png) [@md8n](https://forums.maslowcnc.com/u/md8n)\
**Post date:** [July 31, 2022, 3:43pm UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/24 "2022-07-31T15:43:51Z")

</div>

For the ‘free’ tier of Fusion360 it was changed to emit only `G1` codes instead of a combination of `G1` and `G0` codes. Depending on what you’re using the GCode with, `G1` can be a lot slower than `G0`.

Among other things GCodeClean cleans up this behaviour, converting positive z-axis valued `G1` back to `G0` commands.

There’s other tricks as well, although it’s mainly about making sure of ‘better’ GCode

---

<div class="post-metadata">

**Author:** ![mooselake](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/mooselake/32/6218_2.png) [@mooselake](https://forums.maslowcnc.com/u/mooselake)\
**Post date:** [July 31, 2022, 3:59pm UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/25 "2022-07-31T15:59:26Z")

</div>

In case md8n doesn’t jump in (edit: I see we overlapped) there’s a good description on [github](https://github.com/md8n/GCodeClean)

Short answer, it can make your gcode run faster, optimize moving up out of the material being cut, and optimizing how arcs are sent to the controller. Plus it makes gcode look prettier. Try it on some small jobs and something other than your stash of precious walnut, and see what it’ll do for you. I like to cut the same 5-10 minute job multiple times when tweaking parameters, while timing them and looking to see if cut gets screwed up fwiw, although a before/after test or two should be enough for GCC.

Sorry if this is too long, I tend to overexplain. While I tried GCodeClean on a normal (non-Maslow, an old 6"x9" Zenbot Mini) cutting job (number blocks for the grandkids) it really got interesting when I started doing diamond drag engravings (on a non-Maslow machine) with a CAM program that used G1 for plunges retracts, GCodeClean converted the retracts to G0 and saved me a fair amount of time. While these gadgets and handle a high XY speed I was concerned about fast Z moves (probably unnecessarily…) whacking the diamond into the workpiece and cracking it loose from it’s mount. Normally I’d just do a test to failure, but these things are relatively expensive. One peculiarity of the bits is they’re spring loaded, and the cutting pressure is controlled by increasing the spring compression, which normal people would call depth of cut, and the required compression was around 5mm for the bit and material I was using. The machine was spending an awful lot of time moving down and then back up, GCodeClean cut the retract time to almost nothing and came close to cutting job time in half. Ideally it would rapid until the bit almost touches, slowly plunge until the diamond contacted the surface, and then speed up, but that’s way to specialized for a general purpose utility and is opposite of how you’d use a spinny cutting bit.

I’m a big fan of G2/G3 arcs instead of short line segments. Besides a significant increase in gcode file size, and in the number of characters that have to be fired across the serial interface (at least for grbl like controllers, not an issue for, say, LinuxCNC), and (although I haven’t looked) could improved the lookahead of the movement planner. They also have the potential of executing arcs with step sized segments, making them as smooth as the machine can possibly go. GCodeClean will convert line segments to arcs which also made it very attractive

I’ve been interested in optimizing travel moves for a long time, admittedly not enough to take off my retired hat and trying to do it myself. Many CAM programs (3DP slicers are very bad at this) generate pretty stupid hopping around gcode, a lot of wtf moves instead of keeping travel lengths between cuts short. Adding this to GCodeClean is pretty exciting. My mental picture of the ideal optimizer breaks every file into an array of cuts, all with beginning and ending XYZ coordinates with a feed rate and then ordering them while maybe reversing direction (gets into climb/convention issues) to give the fastest cutting file. Less straightforward when you start thinking about depths of cut, you don’t want to cut the Z-10 paths before you cut the Z-1 paths above it, for example. The more common technique and easier technique seems to be breaking gcode into blocks separated by Z moves and then doing something like a TSP solution between blocks.

---

<div class="post-metadata">

**Author:** ![mooselake](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/mooselake/32/6218_2.png) [@mooselake](https://forums.maslowcnc.com/u/mooselake)\
**Post date:** [July 31, 2022, 4:06pm UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/26 "2022-07-31T16:06:47Z")

</div>

Sure, although the files I’m using lately are in the 60K to 150K line range. I’ll see if one will zip up small enough to attach. I’ll see if I can run them through 1.0.5 and see what happens although there may be some honeydo’s in the way today. I recently dropped a FluidNC/ESP32 controller into the machine (it was using an uno/cnc shield so fitting it was painless) and have been cutting what may become a table lamp with pine trees around the base and an elk over them (clipart that came with VCarve…) to give it a good test.

I’ve been doing some googling about arcs and rotary axes but not finding anything useful. The closest was a short comment on Haas’s site that said they only do arcs on linear, not rotary, axes. Hmm, vectric offers both raster scan and waterline cutting, wonder what that might do. I’ve only been using raster.

---

<div class="post-metadata">

**Author:** ![dlang](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/dlang/32/859_2.png) [@dlang](https://forums.maslowcnc.com/u/dlang)\
**Post date:** [July 31, 2022, 4:39pm UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/27 "2022-07-31T16:39:02Z")

</div>

gcode (as produced by many programs) can be very inefficient, making lots of  
tiny moves, lots of up and down moves in one place (useful for drilling, but not  
for anything else), etc. GCodeClean goes through your gcode and writes a version  
out that produces the same result (within a very small error margin), but  
optimizes it.

For the Maslow, which normally operates on the scale of ~1/100 inch, CAD/CAM is  
happy to do things on the scale of 1/10000 inch, and when doing corners, will  
split a corner into hundreds of lines of gcode, each moving the bit just a tiny  
bit. When cutting wood, this results in burning of the wood at the corner as the  
CNC machine takes more time to parse each line of gcode and the resulting  
movement may be less than the resolution of the machine.

GCodeClean detects such tiny movements and removes them (among other things but  
this is an easy example)

David Lang

---

<div class="post-metadata">

**Author:** ![jonatpridesleap](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/jonatpridesleap/32/6639_2.png) [@jonatpridesleap](https://forums.maslowcnc.com/u/jonatpridesleap)\
**Post date:** [July 31, 2022, 7:42pm UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/28 "2022-07-31T19:42:13Z")

</div>

Thanks for the explanantions everyone.

I actualy use the paid version of Fusion so I probably have never encountered this particular problem with it. However, I absolutely can see this being a problem with other CAM packages and see now why GCC was developed. When I used to send out work to a cabinet builder to cut, he hated receiving designs that contained splines for a similar reason. His CAM would break a spline into 1000’s of straight lines. At best it would take 10x longer to cut. At worse it would start fires.

Anyway, when I stop doing commercial work with Fusion and I flip back over to the free version then I will need this solution so thanks for putting it together!

---

<div class="post-metadata">

**Author:** ![mooselake](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/mooselake/32/6218_2.png) [@mooselake](https://forums.maslowcnc.com/u/mooselake)\
**Post date:** [July 31, 2022, 9:01pm UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/29 "2022-07-31T21:01:45Z")

</div>

GCodeClean really doesn’t like my 4th axis Vectric gcode. VCarve recommends center 0 for rotary jobs, so all Z values are positive, forgot about that. It kind of defeats the whole purpose of zclamping. A seems to work OK, but it quit about 24K in. I tried to attach a zipped copy of the 130K line gcode file, but it won’t upload, gets to 100% and gets an error message “Sorry, an error has occurred.”, also tried with the faceplant trick of renaming it to dot zipp, that failed the same way, as did the raw gcode. Here’s a [google drive link](https://drive.google.com/file/d/1bOP4mW7JI60vsbCLC4jxrT4zJMsRcosN/view?usp=sharing) that might work

---

<div class="post-metadata">

**Author:** ![md8n](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/md8n/32/28197_2.png) [@md8n](https://forums.maslowcnc.com/u/md8n)\
**Post date:** [July 31, 2022, 11:39pm UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/30 "2022-07-31T23:39:02Z")

</div>

OK - Got that downloaded, I’ll start exploring it soon

---

<div class="post-metadata">

**Author:** ![md8n](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/md8n/32/28197_2.png) [@md8n](https://forums.maslowcnc.com/u/md8n)\
**Post date:** [July 31, 2022, 11:48pm UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/31 "2022-07-31T23:48:04Z")

</div>

> [@jonatpridesleap](#):
>
> see now why GCC was developed

It was developed because of this:

 ![IMG_20200508_154227_HDR](https://canada1.discourse-cdn.com/flex031/uploads/maslowcnc/original/3X/2/9/29519a85be6337ff48bc7b3520a674148c156fb2.jpeg)  
That’s a 15 hour carving of a 15MB, 486K lines GCode file (to be honest I broke it into 15 files to carve).  
Now with the current version of GCodeClean that’s reduced to a GCode file that is 3MB and 106K lines of GCode

---

<div class="post-metadata">

**Author:** ![jonatpridesleap](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/jonatpridesleap/32/6639_2.png) [@jonatpridesleap](https://forums.maslowcnc.com/u/jonatpridesleap)\
**Post date:** [July 31, 2022, 11:52pm UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/32 "2022-07-31T23:52:58Z")

</div>

486k…… I … I thought that was a file size….

---

<div class="post-metadata">

**Author:** ![md8n](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/md8n/32/28197_2.png) [@md8n](https://forums.maslowcnc.com/u/md8n)\
**Post date:** [July 31, 2022, 11:54pm UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/33 "2022-07-31T23:54:01Z")

</div>

Well … in a way it is 😉

---

<div class="post-metadata">

**Author:** ![md8n](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/md8n/32/28197_2.png) [@md8n](https://forums.maslowcnc.com/u/md8n)\
**Post date:** [July 31, 2022, 11:57pm UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/34 "2022-07-31T23:57:12Z")

</div>

I used estlcam to generate the GCode from an SVG file. estlcam did an awesome job of path matching, but it generally generated line segments that were around 0.1mm long. With my maslow only processing around 10 lines of GCode per second that meant my actual feed rate was reduced to 1mm/s, so I needed a way of reanalysing GCode to take a more efficient approach (within tolerance limits).

---

<div class="post-metadata">

**Author:** ![md8n](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/md8n/32/28197_2.png) [@md8n](https://forums.maslowcnc.com/u/md8n)\
**Post date:** [August 1, 2022, 5:29am UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/35 "2022-08-01T05:29:34Z")

</div>

# GCodeClean gets travelling v1.1.0 🚎

This is the first step towards doing file splitting and ultimately travelling path optimisation. So it gets a jump as a major point release to v1.1

[Release v1.1.0 - Identify Travelling · md8n/GCodeClean (github.com)](https://github.com/md8n/GCodeClean/releases/tag/v1.1.0)

---

<div class="post-metadata">

**Author:** ![md8n](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/md8n/32/28197_2.png) [@md8n](https://forums.maslowcnc.com/u/md8n)\
**Post date:** [August 18, 2022, 12:00am UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/36 "2022-08-18T00:00:05Z")

</div>

# Need to get .net 6 for building GCodeClean yourself?

It’s now super easy on Ubuntu 22.04 (latest LTS of Ubuntu)  
[.NET 6 is now in Ubuntu 22.04 - .NET Blog (microsoft.com)](https://devblogs.microsoft.com/dotnet/dotnet-6-is-now-in-ubuntu-2204/)

> **[Microsoft and Canonical announce native .NET availability in Ubuntu 22.04...](https://ubuntu.com/blog/install-dotnet-on-ubuntu)**
>
> .NET and ASP.NET are now natively available on Ubuntu hosts and container images. Ultra-small container images prebuilt from Ubuntu packages are available.

---

<div class="post-metadata">

**Author:** ![md8n](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/md8n/32/28197_2.png) [@md8n](https://forums.maslowcnc.com/u/md8n)\
**Post date:** [September 6, 2022, 5:11am UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/37 "2022-09-06T05:11:01Z")

</div>

# For Future Me To Do

GCodeClean runs on .net - not the old .net Framework that only ran on Windows, but the newer .net (formerly known as .net core) that runs on absolutely everything. .net 7 is about to go RC1 (Release Candidate 1) which means it is on the path to a final release.

For several years now ‘performance’ (by all measures) has been a 'first-class feature` for each .net release, .net 7 features an absolute tonne of performance improvements. But one that caught my eye is this one: [performance improvements in .net 7 - Native AOT](https://devblogs.microsoft.com/dotnet/performance_improvements_in_net_7/#native-aot)  
(warning that’s a very very long blog that just covers some of the performance improvements)

Native AOT - means ‘Ahead of Time code generation, Native to OS and processor’. For GcodeClean this would mean having a single file, the executable itself, that’s compiled specific to a given OS (and processor) and would likely equal a drop in file size of 90%

I’m particularly keen on seeing what impact this would have for GCodeClean on Raspberry Pis.

But also, if there’s anyone wanting GCodeClean to run on Macs please let me know. With .net 7 it would be practical for me to start doing Mac specific builds again for the releases.

---

<div class="post-metadata">

**Author:** ![TimS](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/tims/32/17329_2.png) [@TimS](https://forums.maslowcnc.com/u/TimS)\
**Post date:** [September 11, 2022, 4:51am UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/38 "2022-09-11T04:51:08Z")

</div>

I’ll be downloading v1.0.1 this weekend and testing it for you. Any options you need feedback on?

---

<div class="post-metadata">

**Author:** ![md8n](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/md8n/32/28197_2.png) [@md8n](https://forums.maslowcnc.com/u/md8n)\
**Post date:** [September 12, 2022, 12:00am UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/39 "2022-09-12T00:00:33Z")

</div>

Not really anything specific - I’ll be very interested if someone gets it up and working on their own Raspberry Pi (or Mac), and the usual is if you get an ‘interesting’ result from it reprocessing a file.

The only new ‘feature’ as such does not require any new switch. At the end of each cutting section GCodeClean will emit a comment with data about that section. This is a precursor to file splitting and then travelling optimisation.

---

<div class="post-metadata">

**Author:** ![md8n](https://yyz1.discourse-cdn.com/flex031/user_avatar/forums.maslowcnc.com/md8n/32/28197_2.png) [@md8n](https://forums.maslowcnc.com/u/md8n)\
**Post date:** [December 12, 2022, 1:07am UTC](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995/40 "2022-12-12T01:07:22Z")

</div>

# GCodeClean goes to v1.1.2

[Releases · md8n/GCodeClean (github.com)](https://github.com/md8n/GCodeClean/releases)

This is a first step in getting GCodeClean on .net 7 - plus I also replaced the library I was using for the console (terminal) behaviour to something a little newer.

Getting the build working for ARM (Raspberry Pi) with Native AOT (see above) looks to be a little tricky - so you won’t find a pre-built binary for that yet. I may revert to cross-gen compilation for the Pi stuff (so not a single file, and quite a bit bigger) but we’ll see …

[Previous page](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995.md?page=1)

[Next page](https://forums.maslowcnc.com/t/gcodeclean-hits-v1-0-1/17995.md?page=3)