Converts G0/G1 GCode commands to G2/G3 (arc) commands and back again. This can greatly compress most GCode files and potentially improve quality by preventing planner starvation. It is especially useful when streaming over a serial connection (OctoPrint, Pronterface, Slicer Direct Printing), but has some potential advantages in other cases too depending on your firmware and board.
This software was designed for 3D printers but should also be useful in other cases.
In order for ArcWelded gcode files to work on your printer, arcs must be enabled. If these gcodes aren't enabled, the arc commands will be skipped, resulting in a mess. I plan to add instructions for detecting whether or not arc gcodes are enabled in the future.
Most gcode visualizers do NOT correctly display G2/G3 commands. This will cause the output to look like a mess, but it does NOT mean the ArcWelded GCode commands are incorrect or broken. It is likely that they will print just fine provided arc commands are enabled within your printer's firmware.'
Here are some common visualizers that do NOT support G2/G3 commands:
- Cura
- PrusaSlicer
- Slic3r
- Slic3r PE
- SuperSlicer
Here are a few that DO support G2/G3 commands:
- Simplify3D
- OctoPrint's built in 2D GCode Viewer
- PrettyGCode plugin for OctoPrint
- ncviewer.com - Note that this viewer has some issues with embedded thumbnails. It sometimes renders certain gcodes as arcs or circles as well, which can cause confusion. You can click on odd looking arcs and check out the gcode. If it's not a G2/G3, it's just a rendering bug.
Installation is a simple matter of downloading and extracting the latest release. You can find all of the releases here, with the latest release on top. Simply scroll to the bottom of the release and download the proper archive for your OS.
The archive will contain two folders:
- bin - Here you will find the two console applications: ArcWelder and ArcStraightener. Just copy these to your local machine and you can run them from the command line, from a script, or directly within most slicers. See the sections below for instructions on how to use these applications.
- lib - This folder contains pre-compiled ArcWelder libraries that can be integrated into applications. The GcodeProcessorLib library has functions for parsing gcode, tracking the printer's state and position, as well as several other goodies. The ArcWelder library (requires GcodeProcessorLib) contains the core welding algorithm.
From the repository root, create a build directory, generate makefile, and build:
mkdir build
cd build
cmake ..
make
The resulting console application is located in build/ArcWelderConsole/. You might want to create the build directory out of the repository, or make git ignore it, to avoid a dirty tree.
This is a multiplatform console application that can be used to run the ArcWelder algorithm from a command prompt. Binaries are available for Windows, Linux, Raspbian, and MacOs. See the [installation][#installation] section for information on how to download the console application.
Once ArcWelder (or ArcWelder.exe for Windows) is downloaded and copied to your machine, you can execute it in the following form:
{Path_To_Arc_Welder} {Options_Parameters} {Source_Path} {Optional_Target_Path}
Overwriting the source file
If you want to overwrite the source file, no target path is needed. For example, if you are running the Windows version from the root of your C drive and want to weld a file called C:\thing.gcode, you could run the following command from the terminal:
C:\ArcWelder.exe C:\thing.gcode
That will replace thing.gcode with a welded version of the file.
Creating a new file
If you want your original file preserved, you can specify a target path.
Windows example:
ArcWelder thing.gcode thing.aw.gcode
Linux/Raspbian example:
./ArcWelder thing.gcode thing.aw.gcode
That would create a new file called thing.aw.gcode and would leave the thing.gcode file alone.
You can also supply a path for the source and target gcode files:
ArcWelder c:\my_gcode\thing.gcode c:\my_gcode\arc_welded_files\thing.aw.gcode
Note: You may need to enclose the paths in quotes, for example, if there are any spaces.
The console program will output all of the options with the following command for Windows:
ArcWelder --help
Run the following command to view the current version, which is very useful for debugging purposes, or if you submit a github issue:
ArcWelder --version
ArcWelder has good defaults for most applications, but occationally you may want more control. Many options are available that might be helpful depending on your situation.
ArcWelder uses the TCLAP Templatized C++ Command Line Parser for implementing the arguments, and I've been most impressed with it.
For some printers, sending a G90 or G91 command also changes the E axis mode. This is required for any printer running Marlin 2+ or a fork of Marlin 2, for Smoothieware, and for Prusa Buddy Firmware (Prusa Mini). Do NOT add this flag if you are running any other firmware. If your firmware is not on this list but requires this parameter, please create an issue, and I will update the documentation.
- Type: Flag
- Default: Disabled
- Short Parameter: -g
- Long Parameter: --g90-influences-extruder
- Example:
ArcWelder "C:\thing.gcode" -g
ArcWelder is able to compress line segments into gcode by taking advantage of the fact that a bunch of tiny line segments can, when viewed from a distance, approximate a curve. However, a true curved path will never match up exactly with a bunch of straight lines, so ArcWelder needs a bit of play in order to create arc commands. The resolution argument tells ArcWelder how much leeway it has with the original toolpath to make an arc. Increasing this value will result in more compression, and reducing it will improve accuracy. It is a trade-off, but one that most slicers implement anyway in order to prevent too many tiny movements from overwhelming your firmware. In fact, ArcWelder can produce toolpaths that are more accurate than simply merging short segments together, making it less 'lossy' than slicer resolution settings.
The default resolution is 0.05mm, which means your toolpaths can deviate by plus or minus 0.025mm. In general, this produces excellent results and toolpaths that are indistinguishable from the originals with the naked eye. For extremely high precision parts, you may decrease this value, but this will reduce the amount of compression that can be achieved.
Values above 0.1 are not recommended, as you may encounter overlapping toolpaths. When using values above 0.1, I recommend you use a visualizer that supports arcs before running your print.
- Type: Value (millimeters)
- Default: 0.05 (+- 0.025)
- Restrictions: Only values greater than 0 are allowed.
- Short Parameter: -r=<decimal_value>
- Long Parameter: --resolution-mm=<decimal_value>
- Example:
ArcWelder "C:\thing.gcode" -r=0.1
This parameter allows you control how much the length of the final arc can deviate from the original toolpath. The default value of 5% is absolutely fine in most cases, even though that sounds like a lot. The key thing to remember here is that your firmware will break the G2/G3 commands into many small segments, essentially reversing the process, so the path length in your firmware will match the original path much more closely.
Originally, this setting was added as a safety feature to prevent prevent bad arcs from being generated in some edge cases. However, since then a new error detection algorithm was added that makes this unnecessary. In some cases, especially if your resolution parameter is large (above 0.1), this setting can be used to fine tune the generated arcs, so I left this setting in as is. 99+% of the time, no adjustments will be necessary here.
- Type: Value (percent)
- Default: 0.05 (5%)
- Restrictions: Only values greater than 0 (0%) and less than 1.0 (100%) are allowed.
- Short Parameter: -t=<decimal_value>
- Long Parameter: --path-tolerance-percent=<decimal_value>
- Example:
ArcWelder "C:\thing.gcode" --path-tolerance-percent=0.10
Allows you to control the maximum radius arc that will be generated with ArcWelder. This was added as a safety feature to prevent giant arcs from being generated for essentially straight lines. ArcWelder does have built-in detection to prevent colinear lines from being turned into arcs, but slight deviations due to the precision of the gcodes (usually fixed to 3 decimal places) can cause arcs to be generated where straight lines would do. Typically no adjustments are necessary from the defaults, but you can adjust this value if you want.
- Type: Value (decimal, millimeters)
- Default: 9999.0mm
- Restrictions: Only values greater than 0.0 are allowed.
- Short Parameter: -m=<decimal_value>
- Long Parameter: --max-radius-mm=<decimal_value>
- Example:
ArcWelder "C:\thing.gcode" --max-radius-mm=1000.0
This option allows G2/G3 commands to be generated when using vase mode. This is an experimental option, and it's possible that there are some unknown firmware issues when adding Z coordinates to arc commands. That being said, I've gotten pretty good results from this option. At some point, this will be enabled by default.
- Type: Flag
- Default: Disabled
- Short Parameter: -z
- Long Parameter: --allow-3d-arcs
- Example:
ArcWelder "C:\thing.gcode" --allow-3d-arcs
This option allows G2/G3 commands to be generated when for travel moves (moves without any extrusion). In general, most travel moves will not be converted for the average 3D print. However, for plotters or CNC, or certain slicers that perform wipe actions while retracting, this feature can be useful. This is an experimental option.
Note: When using the allow-travel-arcs option, you will see separate statistics for the travel move conversion, or a message indicating that no travel moves were converted.
- Type: Flag
- Default: False
- Short Parameter: -y
- Long Parameter: --allow-travel-arcs
- Example:
ArcWelder "C:\thing.gcode" --allow-travel-arcs
Not all gcode has the same precision for X, Y, and Z parameters. Enabling this option will cause the precision to grow as ArcWelder encounters gcodes with higher precision. This may increase gcode size somewhat, depending on the precision of the gcode commands in your file.
Important Note: This option used to be the default, but in some cases I've seen files with unusually high precision. If it gets too high, the resulting gcode may overrun the gcode buffer size, causing prints to fail. For that reason, this option has been disabled by default. I've only seen a few cases where this happens, and it's always been due to custom start/end gcode with extremely high precision. See the Maximum Gcode Length section for more details.
- Type: Flag
- Default: Disabled
- Short Parameter: -d
- Long Parameter: --allow-dynamic-precision
- Example:
ArcWelder "C:\thing.gcode" --allow-dynamic-precision
ArcWelder outputs fixed precision for X, Y, Z, I, and J parameters. 99% of the time the default of 3 decimal places is just fine. If you need (want) more or less precision, you can alter this value.
Note: that when combined with the --allow-dynamic-precision argument, this represents the minimum precision. It will grow if ArcWelder encounters gcode commands with a higher precision.
Important Note: Some firmware isn't capable of executing gcodes that are too long. Increasing the precision will produce longer gcodes. See the Maximum Gcode Length section for more details.
- Type: Value (integer decimal places)
- Default: 3 (3 decimals, example: 1.001)
- Restrictions: Allowed values are 3, 4, 5, or 6.
- Short Parameter: -x=<integer_value>
- Long Parameter: --default-xyz-precision=<integer_value>
- Example:
ArcWelder "C:\thing.gcode" --default-xyz-precision=5
ArcWelder outputs fixed precision for the E parameter (extruder travel). 99% of the time the default of 5 decimal places is what you want. If you need (want) more or less precision, you can alter this value. In general, I do not recommend a value below 3 or above 5.
Note, that when combined with the --allow-dynamic-precision argument, this represents the minimum precision. It will grow if ArcWelder encounters gcode commands with a higher precision.
Important Note: Some firmware isn't capable of executing gcodes that are too long. Increasing the precision will produce longer gcodes. See the Maximum Gcode Length section for more details.
- Type: Value (integer decimal places)
- Default: 5 (5 decimals, example: 1.00001)
- Restrictions: Allowed values are 3, 4, 5, or 6.
- Short Parameter: -e=<integer_value>
- Long Parameter: --default-e-precision=<integer_value>
- Example:
ArcWelder "C:\thing.gcode" --default-e-precision=3
Important: Do NOT enable firmware compensation unless you are sure you need it! Print quality and compression will suffer if it is enabled needlessly.
Some firmware does not handle arcs with a small radius (under approximately 5mm depending on your settings), which will appear flat instead of curved. If larger arcs appear flat, it's likely that G2/G3 is disabled. See this closed issue for more details, including some illustrations showing what firmware compensation does to your gcode.
This applies to Marlin 1.x (but NOT Marlin 2), Klipper (can be fixed by changing settings), and a few others. If you notice small radius arcs that print with a flat edge, you may need to enable firmware compensation. Note that compression may be reduced (perhaps drastically) when firmware compensation is enabled.
This feature is just a workaround, and the best solution will always be to either upgrade your firmware, which is especially important for people running Marlin 1.x or forks, or to adjust your arc interpolation settings (Marlin 2.x and above, Klipper, and others). If you absolutely cannot upgrade your firmware, this may be your only options.
There are two arguments that need to be added to enable firmware compensation:
This is the default length of a segment in your firmware. This setting MUST match your firmware setting exactly. 99% of the time this setting should be 1.0 for firmware compensation to work.
- Type: Value (millimeters)
- Default: 0 (disabled)
- Restrictions: Only values greater than or equal to 0.0 are allowed. If set greater than 0, min-arc-segments must also be set.
- Short Parameter: -s=<decimal_value>
- Long Parameter: --mm-per-arc-segment=<decimal_value>
- Example:
ArcWelder "C:\thing.gcode" --mm-per-arc-segment=1.0 --min-arc-segments=14
This specifies the minimum number of segments that a circle of the same radius must have and is the parameter that determines how much compensation will be applied. This setting was inspired by the Marlin 2.0 arc interpolation algorithm and attempts to follow it as closely as possible. The higher the value, the more compensation will be applied, and the less compression you will get. A minimum of 14 is recommended. Values above 24 are NOT recommended. In general, this should be set as low as possible.
If ArcWelder detects that a generated arc would have fewer segments than specified, it will reject the arc and output regular G0/G1 codes instead. It's possible that a single arc will be broken into several G2/G3 commands as well, depending on the exact situation. Note that ArcWelder will never increase the number of GCodes used, so it is limited by the resolution of the source gcode file.
- Type: Value
- Default: 0 (disabled)
- Restrictions: Only values greater than or equal to 0.0 are allowed. If set greater than 0, mm-per-arc-segment must also be set.
- Short Parameter: -a=<integer_value>
- Long Parameter: --min-arc-segments=<integer_value>
- Example:
ArcWelder "C:\thing.gcode" --mm-per-arc-segment=1.0 --min-arc-segments=14
If you need to enable firmware compensation because you notice that small arcs appear flat, I recommend you start with the following settings:
ArcWelder --mm-per-arc-segment=1.0 --min-arc-segments=14
This should produce much more rounded small arcs. However, in some cases you will want more detail (again, at the cost of compression, which reduces the effectiveness of ArcWelder), increase --min-arc-segments up to around 24. I don't recommend going higher than this since you will start to get lots of uncompressed gcode in areas that need it.
This feature allows ArcWelder to abort an arc if the extrusion rate changes by more than the value set here. Note that a setting of 0.050 = 5.0%. This option especially useful for prints using Cura's Arachne engine, but is also useful for regular prints. Set this value to 0 to disable this feature.
- Type: Value
- Default: 0.05 (5.0%)
- Restrictions: Only values greater than or equal to 0.0 are allowed.
- Short Parameter: -v=<decimal_value> (0.05 = 5.0%, 0 to disable)
- Long Parameter: --extrusion-rate-variance-percent=<decimal_value>
- Example:
ArcWelder "C:\thing.gcode" --extrusion-rate-variance-percent=0.025
Some firmware has a problem with long gcode commands, and G2/G3 commands are some of the longest. You can specify a maximum gcode length to prevent long commands from being generated, which will reduce compression by a tiny amount.
Non-zero values less than 31 are not allowed.
- Type: Value
- Default: 0 (no limit)
- Restrictions: Can be set to 0, or values > 30.
- Short Parameter: -c=<integer_value>
- Long Parameter: --max-gcode-length=<integer_value>
- Example:
ArcWelder "C:\thing.gcode" --max-gcode-length=50
This setting allows you to control the type of progress messages the ArcWelder console application will display. There are three options:
SIMPLE - This is the default setting. Here is a sample simple progress message:
Progress: 21.9% complete - Estimated 35 of 45 seconds remaing.
FULL - This will show a much more detailed message, which is useful for any applications that which to scrape the detailed progress messages. Here is a sample full progress message:
Progress: percent_complete:100.00, seconds_elapsed:0.01, seconds_remaining:0.00, gcodes_processed: 4320, current_file_line: 4320, points_compressed: 2092, arcs_created: 81, arcs_aborted_by_flowrate: 59, num_firmware_compensations: 0, num_gcode_length_exceptions: 0, compression_ratio: 2.27, size_reduction: 55.96%
NONE - No progress messages will be shown.
- Type: Value
- Default: SIMPLE
- Short Parameter: -P=<SIMPLE|FULL|NONE>
- Long Parameter: --progress-type=<SIMPLE|FULL|NONE>
- Example:
ArcWelder "C:\thing.gcode" --progress-type=FULL
When set, ArcWelder will log to the console. This can be used to track down issues, or to figure out exactly what ArcWelder is doing.
Important Note: Setting the log level could cause a huge amount of data to be outputted to the console, and will cause ArcWelder to be slow. I recommend you redirect the console output to speed things up if you use the DEBUG, VERBOSE or NOSET log levels.
- Type: Value
- Default: INFO
- Short Parameter: -l=<NOSET|VERBOSE|DEBUG|INFO|WARNING|ERROR|CRITICAL>
- Long Parameter: --log-level=<NOSET|VERBOSE|DEBUG|INFO|WARNING|ERROR|CRITICAL>
- Example:
ArcWelder "C:\thing.gcode" --log-level=DEBUG
It's easy to integrate ArcWelder with most slicers.
There is no way to plug the ArcWelder console application into Cura. Fortunately there is a plugin in the marketplace that integrates ArcWelder into Cura, developed by FieldOfView, so no worries there!
Note that if you are running Marlin 2, a fork of Marlin 2, Prusa Buddy (Prusa Mini), or Smoothieware, enable the 'G90 Influences Extruder' setting. See the G90 Influences Extruder section for more info.
If you are running Marlin 1 or any fork of Marlin 1 (Prusa Firmware for Mk2/Mk3, for example) or Klipper, you might consider enabling Firmware Compensation. This is dependent on your firmware settings, but in general you will want to set MM Per Arc Segment to 1.0 and Min Arc Segments to 14 to enable firmware compensation. Setting either to 0 will disable this. See the firmware compensation section for more info.
There are slight differences between these different slicers, but fortunately the method for integrating ArcWelder is the same.
- Put the ArcWelder binary somewhere on your PC and copy the full path (see the installation section above). For example:
C:\ArcWelder - Select 'Print Settings'.
- Depending on which slicer your are using, you may have to enable 'Advanced' or 'Expert' mode (PrusaSlicer requires this at least).
- Select the 'Output options' sub menu.
- In the 'Post-processing scripts', add the following command (your path to ArcWelder may be different):
c:\ArcWelder.exe
That will run ArcWelder on each sliced print with the default parameters.
- Save your settings changes.
- Slice a test file and open it, checking for the ArcWelder header at the top, which should look like this:
; Postprocessed by [ArcWelder](https://github.com/FormerLurker/ArcWelderLib)
Now you should be good to go!
There are some parameters you might want to add. For example, if you are using a printer running Marlin 1.0 or a fork of Marlin 1, you may want to enable firmware compensation. Here's an example of that:
{path_to_arc_welder_here}\ArcWelder.exe --mm-per-arc-segment=1.0 --min-arc-segments=14
See the firmware compensation section for more info.
If you are running Marlin 2.0, a fork of Marlin 2.0, Smoothieware, or Prusa Buddy (for the Prusa Mini), you will want to add the --g90-influences-extruder like so:
{path_to_arc_welder_here}\ArcWelder.exe --g90-influences-extruder
See the G90 Influences Extruder section for more info.
- Edit your current process settings.
- Click on the Scripts tab.
- Add the following command (your path to ArcWelder may be different) like so:
c:\ArcWelder.exe "[output_filepath]"
Important Note: The quotes around the [output_filepath] tag are CRITICAL! Omitting these will lead to intermittent issues depending on your gocde path and file name. Also, DO NOT hard code an output path or file name. Simplify3D will automatically replace the token [output_filepath] with the path and file name of our output file.
- Now click 'OK' to save your settings change, load and slice a file, and save it somewhere. Open it up and verify that the ArcWelder header appears at the top of your file. It should look like this:
; Postprocessed by [ArcWelder](https://github.com/FormerLurker/ArcWelderLib)
Now you should be producing welded files directly from Simplify3D!
There are some parameters you might want to add. For example, if you are using a printer running Marlin 1.0 or a fork of Marlin 1, you may want to enable firmware compensation. Here's an example of that:
c:\ArcWelder.exe --mm-per-arc-segment=1.0 --min-arc-segments=14 "[output_filepath]"
See the firmware compensation section for more info.
If you are running Marlin 2.0, a fork of Marlin 2.0, Smoothieware, or Prusa Buddy (for the Prusa Mini), you will want to add the --g90-influences-extruder like so:
c:\ArcWelder.exe --g90-influences-extruder "[output_filepath]"
See the G90 Influences Extruder section for more info.
This is the opposite of ArcWelder. It will find any G2/G3 commands and replace them with G1 commands. This is useful for testing firmware settings and generally seeing what the firmware is doing with your arc commands.
The latest version includes several implementations of the arc interpolation algorithms from several different firmware types and versions. This tool can be extremely useful for tracking down firmware issues when running G2/G3 commands.
Once ArcStraightener (or ArcStraightener.exe for Windows) is downloaded and copied to your machine, you can execute it in the following form:
{Path_To_Arc_Straightener} {Options_Parameters} {Source_Path} {Optional_Target_Path}
Alternatively, you can put the source and (optional) target path first:
{Path_To_Arc_Straightener} {Source_Path} {Optional_Target_Path} {Options_Parameters}
Important Note: By Default, ArcStraightener will process your gcode using the latest version of Marlin 2's arc interpolation algorithm using the default firmware settings. See the --firmware-type and --firmware-version parameters for information about supported firmware types and versions.
Overwriting the source file
If you want to overwrite the source file, no target path is needed. For example, if you are running the Windows version from the root of your C drive and want to weld a file called C:\thing.aw.gcode, you could run the following command from the terminal:
C:\ArcStraightener.exe C:\thing.aw.gcode
That will replace thing.aw.gcode with a welded version of the file.
Creating a new file
If you want your original file preserved, you can specify a target path.
Windows example:
ArcStraightener thing.aw.gcode thing.gcode
Linux/Raspbian example:
./ArcStraightener thing.aw.gcode thing.gcode
That would create a new file called thing.gcode and would leave the thing.aw.gcode file alone.
You can also supply a path for the source and target gcode files:
ArcStraightener c:\my_gcode\thing.aw.gcode c:\my_gcode\arc_welded_files\thing.gcode
Note: You may need to enclose the paths in quotes, for example, if there are any spaces:
ArcStraightener "c:\my_gcode\thing with spaces.aw.gcode" "c:\my_gcode\arc_welded_files\thing with spaces.gcode"
You can get a full list of parameters using the --help argument like so:
ArcStraightener --help
This will also show you what firmware types and versions are available.
Run the following command to view the current version, which is very useful for debugging purposes, or if you submit a github issue:
ArcStraightener --version
ArcStraightener has settings that represent the arc interpolation settings for the firmwares that are implemented. The parameters accepted vary by firmware type and version. ArcStraightener will not accept any parameters that will not work with the selected firmware and version. It can also provide a list of available settings and the defaults by firmware type and version.
ArcStraightener also uses the TCLAP Templatized C++ Command Line Parser for implementing the arguments.
The following arguments apply regardless of the firmware type and version selected.
Currently there are 5 different firmware types available: MARLIN_1, MARLIN_2, REPETIER, PRUSA, SMOOTHIEWARE
- Type: Value
- Default: MARLIN_2
- Short Parameter: -f=
- Long Parameter: --firmware-type=
- Example:
ArcStraightener "C:\thing.aw.gcode" --firmware-type==MARLIN_1
Use this argument to specify the firmware version. Not all versions are supported. To see a list of available versions for each firmware type, use the --help argument. Note that the LATEST_RELEASE parameter does not always point to the most recent version, but rather the most recent stable release. Also, the PRUSA firmware version V3_11_0 is not yet released, but was added assuming new arc interpolation parameters from the roadmap will be included.
Note: You may need to specify the firmware-type argument to choose the appropriate firmware version.
- Type: Value
- Default: LATEST_RELEASE
- Short Parameter: -V=
- Long Parameter: --firmware_version=
- Example:
ArcStraightener "C:\thing.aw.gcode" --firmware-type==MARLIN_1 --firmware_version==1.1.9.1
Prints all avaliable settings and defaults for the provided firmware type and version. When using this parameter, all other valid parameters will be ignored.
Note: Supply the --firmware_type and --firmware_version to see the defaults and supported settings. When printing firmware defaults, you don't need to supply a source file location.
- Type: Flag
- Short Parameter: -p
- Long Parameter: --print-firmware-defaults
- Example:
ArcStraightener --print-firmware-defaults --firmware_type=MARLIN_1 --firmware_version==1.1.9.1
The different firmware types and versions all support different arc interpolation settings. See the Print Firmware Defaults section for info on how to discover what paramaters a specific firmware version supports, as well as the defaults.
Sets the firmware's G90/G91 influences extruder axis behavior. By default this is determined by the firmware's behavior.
- Type: Value
- Default: Set By Firmware Type and Version
- Short Parameter: -g=<TRUE,FALSE>
- Long Parameter: --g90-influences-extruder=
- Example:
ArcStraightener "C:\thing.aw.gcode" --firmware_type=PRUSA --firmware_version==V1_1_9_1 --g90-influences-extruder=TRUE
Note, in the example above, the default behavior of the prusa firmware is overridden by the argument.
This is the default segment length for arc interpolation. Depending on the implementation, arcs could be longer or shorter than this value.
- Type: Value (millimeters)
- Default: 1.0
- Short Parameter: -m=<decimal_value>
- Long Parameter: --mm-per-arc-segment=<decimal_value>
- Example:
ArcStraightener "C:\thing.aw.gcode" --mm-per-arc-segment=0.5
This is the maximum length an arc segment can be. Similar to --arc-segments-per-r, but is used in different firmware. This has replaced and has a slightly different meaning than --mm-per-arc-segment in newer versions of Marlin 2.0.
- Type: Value (millimeters)
- Default: 1.0
- Short Parameter: -d=<decimal_value>
- Long Parameter: --max-arc-segment-mm=<decimal_value>
- Example:
ArcStraightener "C:\thing.aw.gcode" --max-arc-segment-mm=0.5
This is the maximum length an arc segment can be. Similar to --max-arc-segment-mm, but is used in different firmware.
- Type: Value (millimeters)
- Default: 0 (disabled)
- Short Parameter: -i=<decimal_value>
- Long Parameter: --arc-segments-per-r=<decimal_value>
- Example:
ArcStraightener "C:\thing.aw.gcode" --arc-segments-per-r=0.5
This is the Minimum length an arc segment can be. Similar to -min_arc_segment_mm, but used for different firmware.
- Type: Value (millimeters)
- Default: 1.0
- Short Parameter: -n=<decimal_value>
- Long Parameter: --min-mm-per-arc-segment=<decimal_value>
- Example:
ArcStraightener "C:\thing.aw.gcode" --min-mm-per-arc-segment=0.5
This is the Minimum length an arc segment can be. Similar to --min=mm-per-arc-segment, but used for different firmware.
- Type: Value (millimeters)
- Default: 1.0
- Short Parameter: -b=<decimal_value>
- Long Parameter: --min_arc_segment_mm=<decimal_value>
- Example:
ArcStraightener "C:\thing.aw.gcode" --min_arc_segment_mm=0.5
The minimum number of segments within a circle of the same radius as the arc. Can be used to increase detail on small arcs. This is a the same as --min-circle-segments setting used in some firmware versions.
- Type: Integer Value
- Default: 24
- Short Parameter: -r=<integer_value>
- Long Parameter: --min-arc-segments=<integer_value>
- Example:
ArcStraightener "C:\thing.aw.gcode" --min-arc-segments=24
The minimum number of segments within a circle of the same radius as the arc. Can be used to increase detail on small arcs. This is a the same as --min-arc-segments setting used in some firmware versions.
- Type: Integer Value
- Default: 72
- Short Parameter: -a=<integer_value>
- Long Parameter: --min-circle-segments=<integer_value>
- Example:
ArcStraightener "C:\thing.aw.gcode" --min-circle-segments=24
The number of segments that will be interpolated using a small angle approximation before true sin/cos corrections are applied. A value less than or equal to 1 will disable this feature. Note that enabling this can cause visible interpolation errors, especially on arcs with a very large radius. Disabling this setting could cause performance issues on slower hardware.
- Type: Integer Value
- Default: 24
- Short Parameter: -c=<integer_value>
- Long Parameter: --n-arc-correction=<integer_value>
- Example:
ArcStraightener "C:\thing.aw.gcode" --n-arc-correction=8
The number of segments per second. This will produce a constant number of arcs, clamped between mm-per-arc-segment and min-mm-per-arc-segment. Can be used to prevent stuttering when printing very quickly. A value less than or equal to 0 will disable this feature.
- Type: Integer Value
- Default: 0 (Disabled)
- Short Parameter: -s=<integer_value>
- Long Parameter: --arc-segments-per-second=<integer_value>
- Example:
ArcStraightener "C:\thing.aw.gcode" --arc-segments-per-second=24
I'm not 100% sure exactly what this does, but I believe it attempts to limit the drift in the arc path to this value in MM. When I know more I will update this description. This currently is only used in Smoothieware. Set to 0 to disable.
- Type: Value (millimeters)
- Default: 0.01
- Short Parameter: -e=<decimal_value>
- Long Parameter: --mm-max-arc-error=<decimal_value>
- Example:
ArcStraightener "C:\thing.aw.gcode" --mm-max-arc-error=0.25