QtPlasmaC

Installation instructions are available from here.

Following these instructions will yield a machine with the current stable branch of LinuxCNC (v2.9) on Debian 12 (Bookworm).

Follow the instructions from the Updating LinuxCNC on Debian Bookworm section from here.

A package installation (Buildbot) uses prebuilt packages from the LinuxCNC Buildbot.

Add the GPG keys and add the repository to the sources list to suit the Debian version.

The below stanza would add the 2.9 Bullseye repository.

A run in place installation runs LinuxCNC from a locally compiled version usually located at ~/linuxcnc-dev, instructions for building a run in place installation are available from here.

QtPlasmaC requires the selection of one of following three operating modes:

Only one of either Float Switch or Ohmic Probe is required. If both are used then Float Switch will be a fallback if Ohmic Probe is not sensed.

If Ohmic Probe is used then Ohmic Probe Enable is required to be checked on the QtPlasmaC GUI.

Breakaway Switch is not mandatory because the Float Switch is treated the same as a breakaway when not probing. If they are two separate switches, and there are not enough inputs on the breakout board, they could be combined and connected as a Float Switch.

Refer to the Heights Diagram diagram for a visual representation of the terms below.

where: o = overrun, a = acceleration in units/s² and v = velocity in units/s.

Metric example: given a Z axis MAX_ACCELERATION of 600 mm/s² and MAX_VELOCITY of 60 mm/s, the overrun would be 3 mm.

Imperial example: given a Z axis MAX_ACCELERATION of 24 in/s² and MAX_VELOCITY of 2.4 in/s, the overrun would be 0.12 in.

On machines that will utilize an ohmic probe as the primary method of probing, it is highly recommended to install a switch on the floating head as a backup means of stopping Z motion in the event of ohmic probe failure due to dirty surfaces.

LinuxCNC provides two configuration wizards which can be used to build a machine configuration. The choice of these wizards is dependent on the hardware used to control the machine.

If the user wishes to use a Run In Place installation then prior to running one of the following commands they will need to run the following command from a terminal:

If using a Package installation then no additional action is required.

If using a parallel port, use the StepConf wizard by running the stepconf command in a terminal window or launching it using the Application -> CNC -> StepConf Wizard desktop menu entry.

If using a Mesa Electronics board, use the PnCconf wizard by running the pncconf command in a terminal window or launching it using the Application -> CNC -> PnCConf Wizard desktop menu entry.

If using a Pico Systems board, this LinuxCNC forum thread may be helpful.

The machine specific settings are not described here, refer to the documentation for the particular configuration wizard that is being used.

There are LinuxCNC forum sections available for these wizards:

StepConf Wizard

PnCconf Wizard

Fill in the required entries to suit the machine wiring/breakout board configuration.

QtPlasmaC adds two pages to the LinuxCNC configuration wizards for QtPlasmaC specific parameters, the two pages are QtPlasmaC options and User Buttons. Complete each of the wizards QtPlasmaC page to suit the machine that is being configured and the user button requirements.

Note that PnCconf options allow user selection of Feed Override, Linear Velocity, and Jog Increments, whereas in StepConf these are automatically calculated and set.

The THCAD screen will only appear if a Plasma Encoder is selected in the card screen. The the dedicated section on Mesa THCAD for more information.

When the configuration is complete, the wizard will save a copy of the configuration that may be loaded and edited at a later time, a working QtPlasmaC configuration will be created in the following directory: ~/linuxcnc/configs/<machine_name>.

The way the newly created QtPlasmaC configuration can be run from the terminal command line slightly differs depending the way LinuxCNC was installed:

For a package installation (Buildbot):

For a run in place installation:

After running the above command LinuxCNC should be running with the QtPlasmaC GUI visible.

ONLY WHEN this criteria is met should the user proceed with the QtPlasmaC initial setup.

If any Qt dependency errors are encountered while attempting to run the QtPlasmaC configuration, the user may need to run the QtVCP installation script to resolve these issues.

For a package installation (Buildbot) enter the following command in a terminal window:

For a run in place installation enter the following command in a terminal window:

The following heights diagram will help the user visualize the different heights involved in plasma cutting and how they are measured:

Click on the Parameters Tab to view the CONFIGURATION section which shows the user settable parameters. It is necessary to ensure every one of these settings is tailored to the machine.

To set the Z axis DRO relative to the Z axis MINIMUM_LIMIT, the user should perform the following steps. It is important to understand that in QtPlasmaC, touching off the Z axis DRO has no effect on the Z axis position while running a G-code program. These steps simply allow the user to more easily set the probe height as after performing the steps, the displayed Z axis DRO value will be relative to Z axis MINIMUM_LIMIT.

If the machine is equipped with a float switch then the user will need to set the offset in the CONFIGURATION section of the PARAMETERS tab. This will be done by running a "Probe Test" cycle.

A quick method to move to QtPlasmaC from PlasmaC (loaded on top of either AXIS or GMOCCAPY) is to use the plasmac2qt conversion program, which will attempt to create a new QtPlasmaC configuration from an existing PlasmaC INI file. This program will convert the user’s parameters, settings, and materials from the previous PlasmaC configuration and create a new QtPlasmaC configuration directory in the ~/linuxcnc/configs directory.

This methods will keep the original PlasmaC config as a backup with _plasmac and a time stamp appended to the directory name.

To run the plasmac2qt conversion program, use the following instructions:

For a package installation (Buildbot) enter the following line in a terminal window:

For a run in place installation enter the following lines in terminal window:

The following screen will be displayed:

Leave this blank if it is not used/required.

After filling in the appropriate entries, press CONVERT.

This method to move to QtPlasmaC from PlasmaC (loaded on top of either AXIS or GMOCCAPY) is to use a configuration wizard to create a new configuration. This method then allows changing of the base machine configuration at a later date via the configuration wizard, provided that the base INI and base HAL files have not been edited.

This method requires that the user take note of all HAL pins used in the existing config so they can be entered into the configuration wizard. Any custom HAL commands will also need to be noted and added manually to either the custom.hal file or the custom_postgui.hal file which will be created by the configuration wizard.

After using the wizard, the user can then run a conversion program (cfg2prefs) to convert the parameters, settings, and materials from the previous PlasmaC configuration to the new QtPlasmaC configuration. This tool should be used immediately after the user has created a new QtPlasmaC configuration.

Prior to running this conversion program, it is mandatory that the user have both an existing PlasmaC configuration and a new QtPlasmaC configuration. This program will overwrite the existing QtPlasmaC preferences and materials files, and should be used with caution if it is not being run on a new QtPlasmaC configuration.

The program will create a time-stamped backup of the original preferences file and the existing materials file (if it exists).

It will read the existing <machine_name>config.cfg, <machine_name>_run.cfg, <machine_name>_wizards.cfg, and plasmac_stats.var files and write them to an existing _<machine_name>.prefs file. It will also copy the <machine_name>_material.cfg file to the existing QtPlasmaC configuration.

To run the cfg2prefs conversion program, use the following instructions:

For a package installation (Buildbot) enter the following line in a terminal window:

For a run in place installation enter the following lines in terminal window:

Select the INI file of the old PlasmaC configuration, select the INI file of the new QtPlasmaC configuration, then press CONVERT.

The plasmac HAL component has a built in lowpass filter that if used is applied to the plasmac.arc-voltage-in input pin to filter any noise that could cause erroneous voltage readings. The lowpass filter should only be used after using Halscope to determine the required frequency and whether the amplitude of the noise is large enough to cause any issues. For most plasma machines lowpass is not required and should not be used unless it is required.

The HAL pin assigned to this filter is plasmac.lowpass-frequency and is set to 0 (disabled) by default. To apply a lowpass filter to the arc-voltage, the user would edit the following entry in the custom.hal file in the machine’s configuration directory to add the appropriate cutoff frequency as measured in Hertz (Hz).

For example:

The above example would give a cutoff frequency of 100Hz.

Contact bounce from mechanical relays, switches, or external interference may cause some inconsistent behavior of the following switches:

Due to the fact that the software is capable of sampling rates faster than the contact bounce period, it is possible that the software may see contact bounce as several changes in input states occurring in a very small time period, and incorrectly interpret this as a very quick on-off of the input. One method of mitigating contact bounce is to "debounce" the input. To summarize debounce, it requires the input state to be stable at the opposite state of the output state for consecutive delay periods before changing the state of the output.

Debounce delay periods can be changed by editing the appropriate debounce value in the custom.hal file in the <machine_name> config directory.

Each increment of delay adds one servo thread cycle to the debounce time. For example: given a servo thread period of 1000000 (measured in nano seconds), a debounce delay of 5 would equate to 5000000 ns, or 5 ms.

For the Float and Ohmic switches this equates to a 0.001 mm (0.00004") increase in the probed height result.

It is recommended to keep the debounce values as low as possible while still achieving consistent results. Using Halscope to plot the inputs is a good way to establish the correct value.

For QtPlasmaC installations, debounce is achieved by using the HAL dbounce component which is a later alternative to the original debounce component. This new version allows for the loading and naming of individual debounce instances and is compatible with Twopass HAL file processing.

All four signals above have an individual debounce component so the debounce periods can be catered individually to each input. Any changes made to these values in the custom.hal file will not be overwritten by later updates of QtPlasmaC.

The default delay for all four inputs is five servo thread periods. In most cases this value will work quite well. If any of the inputs do not use mechanical switches, it may be possible to either reduce or remove the delay for those inputs.

If debounce is required for other equipment like home or limit switches etc. then more dbounce components may added in any of the HAL files without any regard to the signals listed here.

Mechanical relays and switches usually require a minimum current passing through the contacts for reliable operation. This current varies with the material that the contacts in the device are made from.

Depending on the specified minimum contact current and the current drawn by the input device there may be a need to provide a method to increase the current through the contacts.

Most relays using gold contacts will not require any additional current for reliable operation.

There are two different methods available to provide this minimum current if it is required:

Schematics are shown at contact load schematics.

More information on contact switching load can be seen on page VI of the finder General Technical Information document.

If using a Mesa card, the input resistance of a 7I96 is 4700 Ω (symbol R)(always consult the product manual associated with the revision being used as these values sometimes vary between revisions), giving a contact current of 5.1 mA (symbol I) assuming a supply voltage (symbol U) of 24 V (I = U/R)
[In the US, the letter V is commonly used as a symbol (Voltage) and as a unit (Volt).]
.

As an example, the typical relay used in a Hypertherm Powermax 65 plasma cutter (TE T77S1D10-24) requires a minimum contact load of 100 mA @ 5 VDC which will dissipate 0.5 W (P = I * V). If using a 24 VDC power supply this would then equate to a minimum current of 20.8 mA. Because there is less current drawn by the Mesa input than is required by the relay there needs to be an increase in the current.

The resistance can be calculated using R = U_s / (I_m - I_i) where:

Using a 7I96 with an input current of 5.1 mA gives a calculated value of 1529 Ω ( = 24 V / (.0208 - .0051) A). This could then be rounded down to a commonly available 1500 Ω resistor, giving a small safety margin.

The power dissipation can by calculated using P = U_s² / R_s where:

This gives a value of 0.38 W. This could then be rounded up to 1 W, giving a good safety margin. The final selection would be a 1500 Ω 1 W resistor.

If a link to the launch the configuration was not created when creating the config, the user could create a desktop launcher to the config by right clicking on the desktop and selecting Create Launcher or similar. This will bring up a dialog box to create a launcher. Give the icon a nice short name, enter anything for the command and click OK.

After the launcher appears on the desktop, right click on it and then edit it with the user’s editor of choice. Edit the file so it looks similar to:

If the user would like a terminal window to open behind the GUI window then change the Terminal line to:

Displaying a terminal can be handy for error and information messages.

After a successful QtPlasmaC installation, the following files are created in the configuration directory:

After running a new configuration for the first time the following files will be created in the configuration directory:

QtPlasmaC has some specific <machine_name>.ini file variables as follows:

These variables are mandatory.

[RS274NGC] Section

These variables are mandatory.

[HAL] Section

These variables are mandatory.

[DISPLAY] Section

This variable is mandatory.

There are multiple QtVCP options that are described here: QtVCP INI Settings

For example the following would start a 16:9 resolution QtPlasmaC screen in full screen mode:

[TRAJ] Section

This variable is mandatory.

[AXIS_X] Section

These variables are mandatory.

[AXIS_Y] Section

These variables are mandatory.

[AXIS_Z] Section

These variables are mandatory.

Exiting or shutting down QtPlasmaC is done by either:

A shutdown warning can be displayed on every shutdown by checking the Exit Warning checkbox on the SETTINGS Tab.

Screenshot example of the QtPlasmaC MAIN Tab in 16:9 aspect ratio:

Some functions/features are only used for particular modes and are not displayed if they are not required by the chosen QtPlasmaC mode.

The Button Panel contains buttons useful for the operation of the machine.

The EDIT and MDI buttons are permanent, all other buttons are user programmable in the <machine_name>.prefs file.

See custom user buttons for detailed information on custom user buttons.

The QtPlasmaC preview screen has the ability to be switched between different views and displays, as well as zooming in and out, and panning horizontally and vertically.

When QtPlasmaC is first started, the Z (top down) view will be selected as the default view for a loaded G-code file, but the full table view will be displayed.

When a G-code file is loaded, the display will change to the selected view.

Whenever there is no G-code file loaded, the full table will automatically be displayed irrespective of which view is currently selected (the highlighted button representing the currently selected view will not change).

If a full table is displayed due to no G-code file being loaded and the user wishes to change the view orientation, then pressing either Z or P will change the display to the newly selected view. If the user then wishes to display the full table while maintaining the currently selected view as the default view for a loaded G-code file, then pressing CLEAR will achieve this and allow the selected view orientation to prevail the next time a G-code file is loaded.

Screenshot example of the QtPlasmaC CONVERSATIONAL Tab in 16:9 aspect ratio:

The CONVERSATIONAL Tab enables the user to quickly program various simple shapes for quick cutting without the need for CAM software.

See Conversational Shape Library for detailed information on the Conversational feature.

It is possible to hide this tab so the conversational feature cannot be used by an operator. This may be achieved either by wiring the pin to a physical key-switch or similar or it may also be set in a HAL file using the following command:

Screenshot example of the QtPlasmaC PARAMETERS Tab in 16:9 aspect ratio:

Some functions/features are only used for particular modes and are not displayed if they are not required by the chosen QtPlasmaC mode.

This tab is used to display configuration parameters that are modified infrequently.

It is possible to hide this tab so machine settings cannot be modified by unauthorized personnel. This may be achieved either by wiring the pin to a physical key-switch or similar or it may also be set in a HAL file using the following command:

Two methods of THC activation are available and are selected with the Auto Activation checkbutton. Both methods begin their calculations when the current velocity of the torch matches the cut feed rate specified for the selected material:

The SAVE button will save the currently displayed parameters to the <machine_name>.prefs file.

The RELOAD button will reload all the parameters from the <machine_name>.prefs file.

The SAVE button will save the current material set to the <machine_name>_material.cfg file.

The RELOAD button will reload the material set from the <machine_name>_material.cfg file.

The NEW button will allow a new material to be added to the material file. The user will be prompted for a material number and a material name, all other parameters will be read from the currently selected material. Once entered, QtPlasmaC will reload the material file and display the new material. The Cut Parameters for the new material will then need to be adjusted and saved.

The DELETE this button is used to delete a material. After pressing it, the user will be prompted for a material number to be deleted, and prompted again to ensure the user is sure. After deletion, the material file will be reloaded and the drop down list will display the default material.

Screenshot example of the QtPlasmaC SETTINGS Tab in 16:9 aspect ratio:

This tab is used to display GUI configuration parameters, button text, and shutdown text that are modified infrequently as well as some utility buttons.

It is possible to hide this tab so machine settings cannot be modified by unauthorized personnel. This may be achieved either by wiring the pin to a physical key-switch or similar or it may also be set in a HAL file using the following command:

This section shows parameters that effect the GUI appearance and GUI behaviors.

To return any of the color changes to their default values, see the Returning To The Default Styling section.

This section shows the text that appears on the Custom User Buttons as well as the code associated with the user button. User buttons may be changed and the new settings used without restarting LinuxCNC.

The text and/or code may be edited at any time and will be loaded ready for use if the SAVE button is clicked.

Deleting the Name and Code text will cause that user button to be hidden if the SAVE button is clicked.

To return all the Name and Code text to their last saved values press the RELOAD button.

This section shows the text that appears on the shutdown dialog if the Exit Warning is enabled .

The text may be edited at any time and will be loaded ready for use if the SAVE button is clicked.

To return the EXIT WARNING MESSAGE text to the last saved value press the RELOAD button.

Some standard LinuxCNC utilities are provided as an aid in the diagnosis of issues that may arise:

In addition the following two QtPlasmaC specific utilities are provided:

The SET OFFSETS button is used if the table has a laser or camera for sheet alignment, a scribe, or uses offset probing. The required offsets for these peripherals need to be applied by following the procedure described in Peripheral Offsets.

The BACKUP CONFIG button will create a complete machine configuration backup for archiving or to aid in fault diagnosis. A compressed backup of the machine configuration will be saved in the user’s Linux home directory. The file name will be <machine_name><version><date>_<time>.tar.gz, where <machine_name> is the machine name entered in the configuration wizard, <version> is the current QtPlasmaC version the user is on, <date> is the current date (YY-MM-DD), and <time> is the current time (HH-MM-SS).

Prior to the backup being made, the machine log will be saved to a file in the configuration directory named machine_log_<date>_<time>.txt where <date> and <time> are formatted as described above. This file along with up to five previous machine logs will also be included in the backup.

These files are not required by QtPlasmaC and are safe to delete at any time.

The STATISTICS Tab provides statistics to allow for the tracking of consumable wear and job run times. These statistics are shown for the current job as well as the running total. Previous job statistics are reset once the next program is run. The total values may be reset either individually by clicking the corresponding "RESET" button, or they may all be reset together by clicking "RESET ALL".

The RS485 PMX STATISTICS panel will be only be displayed if the user has Hypertherm PowerMax communications and a valid RS485 connection to the PowerMax is established. This panel will show the ARC ON TIME for the PowerMax in hh:mm:ss format.

The MACHINE LOG is also displayed on the STATISTICS Tab, this log will display any errors and/or important information that occurs during the current LinuxCNC session. If the user makes a backup of the configuration from the SETTINGS Tab then the machine log is also included in the backup.

All settings and parameters in QtPlasmaC are required to be in the same units as specified in the INI file, being either metric or imperial.

If the user is attempting to run a G-code file that is in the "other" units system then all parameters including the material file parameters are still required to be in the native machines units. Any further conversions necessary to run the G-code file will be handled automatically by the G-code filter program.

For example: If a user had a metric machine and wished to run a G-code file that was set up to cut 1/4" thick material using imperial units (inch - G20) then the user with the metric machine would need to ensure that either the material number in the G-code file was set to the corresponding metric material to be cut, or that a new material is created with the correct metric parameters for the metric material to be cut. If the metric user wanted to cut the G-code file using imperial material, then the new material parameters would need to be converted from imperial units to metric when they are entered.

The following stanzas are the minimum recommended codes to include in the preamble and postamble of any G-code file to be run by QtPlasmaC:

Metric:

Imperial:

A detailed explanation of each G-code can be found in the docs here.

Note that throughout this user guide there are several additional recommendations for codes that are prudent to add to both the preamble and postamble depending on the features the user wishes to utilize.

Aside from the preamble code, postamble code, and X/Y motion code, the only mandatory G-code syntax for QtPlasmaC to run a G-code program using a torch for cutting is M3 $0 S1 to begin a cut and M5 $0 to end a cut.

For backwards compatibility it is permissible to use M3 S1 in lieu of M3 $0 S1 to begin a cutting job and M5 in lieu of M5 $0 to end a cutting job. Note, that this applies to cutting jobs only, for scribe and spotting jobs the $n tool identifier is mandatory.

See recommended Z axis settings.

Each time LinuxCNC (QtPlasmaC) is started Joint homing is required. This allows LinuxCNC (QtPlasmaC) to establish the known coordinates of each axis and set the soft limits to the values specified in the <machine_name>.ini file in order to prevent the machine from crashing into a hard stop during normal use.

If the machine does not have home switches then the user needs to ensure that all axes are at the home coordinates specified in the <machine_name>.ini file before homing.

If the machine has home switches then it will move to the specified home coordinates when the Joints are homed.

Depending on the machine’s configuration there will either be a Home All button or each axis will need to be homed individually. Use the appropriate button/buttons to home the machine.

As mentioned in the Initial Setup section, it is recommended that the first time QtPlasmaC is used that the user ensure there is nothing below the torch then jog the Z axis down until it stops at the Z axis MINIMUM_LIMIT then click the 0 next to the Z axis DRO to Touch Off with the Z axis selected to set the Z axis at zero offset. This should not need to be done again.

If the user intends to place the material in the exact same place on the table every time, the user could jog the X and Y axes to the machine to the corresponding X0 Y0 position as established by the CAM software and then Touch Off both axes with a zero offset.

If the user intends to place the material randomly on the table then the user must Touch Off the X and Y axes at the appropriate position before starting the program.

QtPlasmaC is able to read a material file to load all the required cut parameters. To enable to G-code file to use the cut feed rate setting from the cut parameters use the following code in the G-code file:

It is possible to use the standard G-code F word to set the cut feed rate as follows:

If the F word is used and the F word value does not match the cut feed rate of the selected material then a warning dialog will indicate this during loading of the G-code file.

Material handling uses a material file that was created for the machine configuration when the configuration wizard was ran and allows the user to conveniently store known material settings for easy recall either manually or automatically via G-code. The resulting material file is named <machine_name>_material.cfg.

QtPlasmaC does not require the use of a material file. Instead, the user could change the cut parameters manually from the MATERIAL section of the PARAMETERS Tab. It is also not required to use the automatic material changes. If the user does not wish to use this feature they can simply omit the material change codes from the G-code file.

It is also possible to not use the material file and automatically load materials from within the G-code file.

Material numbers in the materials file do not need to be consecutive nor do they need to be in numerical order.

The following variables are mandatory and an error message will appear if any are not found when the material file is loaded.

The following variables are optional. If they are not detected or have no value assigned, they will be assigned a value of 0 and no error message will appear.

The material file uses the following format:

It is possible to add new material, delete material, or edit existing material from the PARAMETERS tab.. It is also possible to achieve this by using magic comments in a G-code file.

The material file may be edited with a text editor while LinuxCNC is running. After any changes have been saved, press Reload in the MATERIAL section of the PARAMETERS Tab to reload the material file.

For manual material handling, the user would manually select the material from the materials list in the MATERIAL section of the PARAMETERS Tab before starting the G-code program. In addition to selecting materials with materials list in the MATERIAL section of the PARAMETERS Tab, the user could use the MDI to change materials with the following command:

The following code is the minimum code necessary to have a successful cut using the manual material selection method:

For automatic material handling, the user would add commands to their G-code file which will enable QtPlasmaC to change the material automatically.

The following codes may be used to allow QtPlasmaC to automatically change materials:

For automatic material handling, the codes MUST be applied in the order shown. If a G-code program is loaded which contains one or more material change commands then the first material will be displayed in the top header of the PREVIEW WINDOW on the MAIN Tab as the program is loading.

By using "magic comments" in a G-code file it is possible to do the following:

Temporary materials are numbered automatically by QtPlasmaC and the material change will also be done by QtPlasmaC and should not be added to the G-code file by CAM software or otherwise. The material numbers begin at 1000000 and are incremented for each temporary material. It is not possible to save a temporary material, however the user could create a new material while a temporary material is displayed and it will use the settings from the temporary material as the defaults.

The options are:

Mandatory parameters are:

Optional parameters are:

A complete example:

If a temporary material has been specified in a G-code file then the material change line (M190…) and wait for change line (M66…) will be added by the G-code filter and are not required in the G-code file.

This application is used to convert existing tool tables into QtPlasmaC material files. It can also create a material file from manual user input to entry fields.

At this stage the only conversions available are for tool tables exported from either SheetCam or Fusion 360.

SheetCam tool tables are complete and the conversion is fully automatic. The SheetCam tool file must be in the SheetCam .tools format.

Fusion 360 tool tables do not have all of the required fields so the user will be prompted for missing parameters. The Fusion 360 tool file must be in the JSON format of Fusion 360.

If the user has a format from a different CAM software they would like converted, create a New Topic in the PlasmaC forum section of the LinuxCNC forum to request this addition.

Material Converter may be run from a terminal using one of the two following methods.

For a package installation (Buildbot) enter the following command in a terminal window:

For a run in place installation enter the following two commands in a terminal window:

This will bring up the Material Converter Main dialog box with Manual selected as the default.

Select one of:

For SheetCam only, select whether the user requires a metric or imperial output file.

To convert:

For both a Manual creation or a Fusion 360 conversion, a dialog box will show with all available parameters displayed for input. Any entry marked with *** is mandatory and all other entries are optional depending on the user’s configuration needs.

QtPlasmaC has the ability to use a laser to set the origin with or without rotation compensation. Rotation compensation can be used to align the work offset to a sheet of material with edge(s) that are not parallel to the machine’s X/Y axes. The LASER button will be enabled after the machine is homed.

To use this feature, the user must set the laser’s offset from the torch center by following the procedure described in Peripheral Offsets.

To modify the offsets manually, the user could edit either or both the following options in the [LASER_OFFSET] section of the <machine_name>.prefs file:

where n.n is distance from the center line of the torch to the laser’s cross hairs.

Additionally, the laser can be tied to any available output to turn the laser on and off via a HAL pin with the following name:

To set the origin with zero rotation:

To set the origin with rotation:

To turn the laser off and cancel an alignment:

If an alignment laser has been set up then it is possible to use the laser during CUT RECOVERY for accurate positioning of the new start coordinates.

QtPlasmaC has the ability to use a USB camera to set the origin with or without rotation compensation. Rotation compensation can be used to align the work offset to a sheet of material with edge(s) that are not parallel to the machine’s X/Y axes. The CAMERA button will be enabled after the machine is homed.

To use this feature, the user must set the camera’s offset from the torch center by following the procedure described in Peripheral Offsets.

To modify the offsets manually, the user could edit either or both the following axes options in the [CAMERA_OFFSET] section of the <machine_name>.prefs file:

where n.n is distance from the center line of the torch to the camera’s cross hairs.

To set the origin with zero rotation:

To set the origin with rotation:

In the CAMVIEW panel, the mouse can affect the cross hairs and the zoom level as follows:

Path tolerance is set with a G64 command and a following P value. The P value corresponds to the amount that the actual cut path followed by the machine may deviate from the programmed cut path.

The default LinuxCNC path tolerance is set for maximum speed which will severely round corners when used with normal plasma cutting speeds.

It is recommended that the path tolerance is set by placing the appropriate G64 command and P value in the header of each G-code file.

The provided G-code filter program will test for the existence of a G64 P__n__ command prior to the first motion command. If no G64 command is found it will insert a G64 P0.1 command which sets the path tolerance to 0.1 mm. For a imperial config the command will be G64 P0.004.

QtPlasmaC has the ability to allow the repositioning of the X and Y axes along the current cut path while the G-code program is paused.

In order to use this feature, LinuxCNC’s Adaptive Feed Control (M52) must be turned on (P1).

To enable Paused Motion The preamble of the G-code must contain the following line:

To turn off Paused Motion at any point, use the following command:

This feature can be used to allow the arc to "catch up" to the torch position to fully finish the cut. It is usually required for thicker materials and is especially useful when cutting stainless steel.

Using this feature will cause all motion to pause at the end of the cut while the torch is still on. After the dwell time (in seconds) set by the Pause At End parameter in the MATERIAL section of the PARAMETERS Tab has expired, QtPlasmaC will proceed with the M5 command to turn off and raise the torch.

QtPlasmaC has the ability to allow the use of more than one type of plasma tool by utilizing LinuxCNC spindles as a plasma tool when running a G-code program.

Valid plasma tools for use are:

A LinuxCNC spindle number (designated by $n) is required to be in the starting command and also the end command to be able to start and stop the correct plasma tool. Examples:

It is permissible to use M5 $-1 in lieu of the M5 $n codes above to stop all tools.

In order to use a scribe, it is necessary for the user to add the X and Y axis offsets to the LinuxCNC tool table. Tool 0 is assigned to the Plasma Torch and Tool 1 is assigned to the scribe. Tools are selected with a Tn M6 command, and then a G43 H0 command is required to apply the offsets for the selected tool. It is important to note that the LinuxCNC tool table and tool commands only come into play if the user is using a scribe in addition to a plasma torch. For more information, see scribe.

There is a HAL pin available named motion.analog-out-03 that can be changed in G-code with the M67 (Synchronized with Motion)/M68 (Immediate) commands. This pin will reduce the velocity to the percentage specified in the command.

It is important to thoroughly understand the difference between Synchronized with Motion and Immediate:

Examples:

The minimum percentage allowed is 10%, values below this will be set to 10%.

The maximum percentage allowed is 100%, values above this will be set to 100%.

If the user intends to use this feature it would be prudent to add M68 E3 Q0 to both the preamble and postamble of the G-code program so the machine starts and ends in a known state.

The THC can be enabled or disabled from the THC frame of the MAIN Tab.

The THC can also be enabled or disabled directly from the G-code program.

The THC does not become active until the velocity reaches 99.9% of the CutFeedRate and then the THC Delay time if any in the THC section of the PARAMETERS Tab has timed out. This is to allow the arc voltage to stabilize.

QtPlasmaC uses a control voltage which is dependent on the state of the AUTO VOLTS checkbox on the MAIN Tab:

THC may be disabled and enabled directly from G-code, provided the THC is not disabled in the THC Section of the MAIN Tab, by setting or resetting the motion.digital-out-02 pin with the M-Codes M62-M65:

It is important to thoroughly understand the difference between Synchronized with Motion and Immediate:

If the cut velocity falls below a percentage of CutFeedRate (as defined by the VAD Threshold % value in the THC frame of the CONFIGURATION section of the PARAMETERS Tab) the THC will be locked until the cut velocity returns to at least 99.9% of CutFeedRate. This will be made apparent by the VELOCITY ANTI DIVE indicator illuminating in the CONTROL Panel on the MAIN Tab.

Velocity based THC prevents the torch height being changed when velocity is reduced for a sharp corner or a small hole.

It is important to note that Velocity Reduction affects the Velocity Based THC in the following ways:

LinuxCNC (QtPlasmaC) has the ability to automatically adjust the cut path of the current program by the amount specified in Kerf Width of the selected material’s Cut Parameters. This is helpful if the G-code is programmed to the nominal cut path and the user will be running the program on different thickness materials to help ensure consistently sized parts.

To use cutter compensation the user will need to use G41.1, G42.1 and G40 with the kerf width HAL pin:

Initial Height Sense may be skipped in one of two different ways:

A value of zero for Skip IHS will disable all IHS skipping.

Any errors encountered during a cut will disable IHS skipping for the next cut if Skip IHS is enabled.

Probing may be done with either ohmic sensing or a float switch. It is also possible to combine the two methods, in which case the float switch will provide a fallback to ohmic probing. An alternative to ohmic probing is Offset Probing

If the machine’s torch does not support ohmic probing, the user could have a separate probe next to the torch. In this case the user would extend the probe below the torch. The probe must NOT extend more than the minimum Cut Height below the torch and the Z axis offset distance needs to be entered as the Ohmic Offset in the PROBING frame of the CONFIGURATION section of the PARAMETERS Tab.

Probing setup is done in the PROBING frame of the CONFIGURATION section of the PARAMETERS Tab.

QtPlasmaC can probe at the full Z axis velocity so long as the machine has enough movement in the float switch to absorb any overrun. If the machine’s float switch travel is suitable, the user could set the Probe Height to near the Z axis MINIMUM_LIMIT and do all probing at full speed.

Some float switches can exhibit a large switching hysteresis which shows up in the probing sequence as an excessive time to complete the final probe up.

where n is a value from 1-10. It is recommended to keep this value as low as possible.

Using this feature will change the final height slightly and will require thorough probe testing to confirm the final height.

This speed value affects ALL probing so if the user uses ohmic probing and the user changes this speed value then the user will need to probe test to set the require offset to compensate for this speed change as well as the float travel.

The reliability of this feature will only be as good as the repeatability of the float switch.

Offset Probing is the use of a probe that is offset from the torch. This method is an alternative to Ohmic Probing and uses the plasmac.ohmic-enable output pin to operate a solenoid for extending and retracting the probe. The plasmac.ohmic-probe input pin is used to detect the material and the Ohmic Offset in the PROBING frame of the CONFIGURATION section of the PARAMETERS Tab is used to set the correct measured height.

The probe could be a mechanically deployed probe, a permanently mounted proximity sensor or even simply a stiff piece of wire extending about 0.5 mm (0.2") below the torch tip. If the probe is mechanically deployed then it needs to extend/retract rather quickly to avoid excessive probing times and would commonly be pneumatically operated.

To use this feature, the user must set the probe’s offset from the torch center by following the procedure described in Peripheral Offsets.

To modify the offsets manually, the user could edit either or both the following options in the [OFFSET_PROBING] section of the <machine_name>.prefs file:

where n.n is the offset of the probe from the torch center in machine units for the X and Y axes and t.t is the time in seconds to allow for any mechanical deployment of the probe if required.

Each of these parameters is optional and also may appear in any order. If a parameter is not detected then the default is 0.0. There can be no space after the X or Z, lower case is permissible.

When this variable appears in the INI file with either X or Y not equal to zero then QtPlasmaC will do all Ohmic Probing as Offset Probing. When a probe sequence has begun, the plasmac.ohmic-enable pin will be set True causing the probe to extend. When the material is detected the plasmac.ohmic-enable pin will be reset to false causing the probe to retract.

The probe will begin moving to the offset position simultaneously with the Z axis moving down to the Probe Height, probing will not commence unless the deployment timer has completed. It is required that the Probe Height in the PROBING frame of the CONFIGURATION section of the PARAMETERS Tab is above the top of the material to ensure that the probe is fully offset to the correct X/Y position before the final vertical probe down movement.

QtPlasmaC allows two different cut modes:

There are two ways of enabling this feature:

If using a custom user button is utilized then QtPlasmaC will automatically reload the file when the cut type is toggled.

It is recommended that any holes to be cut have a diameter no less than one and a half times the thickness of the material to be cut.

It is also recommended that holes with a diameter of less than 32 mm (1.26") are cut at 60% of the feed rate used for profile cuts. This should also lock out THC due to velocity constraints.

QtPlasmaC can utilize G-code commands usually set by a CAM Post Processor (PP) to aid in hole cutting or if the user does not have a PP or the user’s PP does not support these methods then QtPlasmaC can automatically adapt the G-code to suit. This automatic mode is disabled by default.

There are three methods available for improving the quality of small holes:

G-code commands can be set up by either by a CAM Post Processor (PP) or by hand coding.

If cutting a hole requires a reduced velocity then the user would use the following command to set the velocity: M67 E3 Qnn where nn is the percentage of the velocity desired. For example, M67 E3 Q60 would set the velocity to 60% of the current material’s CutFeedRate.

See the Velocity Based THC section.

This method can be invoked by setting the Pause At End parameter in the MATERIAL frame of the PARAMETERS Tab.

The torch can be turned off at the end of the hole by setting the motion.digital-out-03 pin with the M-Codes M62 (Synchronized with Motion)* or M64 (Immediate). After turning the torch off it is necessary to allow the torch to be turned on again before beginning the next cut by resetting the motion.digital-out-03 pin with the M-Codes M63 or M65, this will be done automatically by the QtPlasmaC G-code parser if it reaches an M5 command without seeing a M63 P3 or M65 P3.

After the torch is turned off the hole path will be followed for a default length of 4 mm (0.157"). This distance may be specified by adding #<oclength> = n to the G-code file.

It is important to thoroughly understand the difference between Synchronized with motion and Immediate:

Sample code:

QtPlasmaC has the ability to automatically modify the G-code to reduce the velocity and/or apply Over cut which can be useful when cutting holes.

For valid hole sensing it is required that all values in the G2 or G3 G-code line are explicit, an error dialog will be displayed if any values are mathematically calculated.

QtPlasmaC Hole Sensing is disabled by default. It can be enabled/disabled by using the following G-code parameters to select the desired hole sensing mode:

The default hole size for QtPlasmaC hole sensing is 32 mm (1.26"). It is possible to change this value with the following command in a G-code file:

The default velocity for QtPlasmaC small holes is 60% of the current feed rate. It is possible to change this value with the following command in a G-code file:

If Hole Sensing modes 2 or 4 are active, QtPlasmaC will over cut the hole in addition to the velocity changes associated with modes 1 and 3.

The default over cut length for QtPlasmaC hole sensing is 4 mm (0.157"). It is possible to change this value with the following command in a G-code file:

This feature can be used in addition to setting the desired hole sensing mode via the appropriate G-code parameter by setting the Pause At End parameter in the MATERIAL frame of the PARAMETERS Tab.

A single cut is a single unidirectional cutting move often used to cut a sheet into smaller pieces prior to running a G-code program.

The machine needs to be homed before commencing a single cut.

A single cut will commence from the machine’s current X/Y position.

This is the preferred method. The parameters for this method are entered in the following dialog box that is displayed after pressing a user button which has been coded to run single cut:

If the machine is equipped with a pendant that can start and stop the spindle plus jog the X and Y axes, the user can manually perform a single cut.

Manual single cut requires that either keyboard shortcuts are enabled in the GUI SETTINGS section of the SETTINGS Tab, or a custom user button is specified as a manual cut button.

If the user is using a custom user button then substitute F9 with User Button in the following description.

Cutting thick materials can be problematic in that the large amount of molten metal caused by piercing can shorten the life of consumables and also may cause a puddle high enough that the torch may hit the puddle while moving to cut height.

The are two functions built into QtPlasmaC to help alleviate these issues.

Pierce Only mode converts the loaded G-code program and then runs the program to pierce the material at the start position of each cut. Scribe and Spotting commands will be ignored and no pierce will take place in those locations.

This mode is useful for thick materials which may produce enough dross on the material surface from piercing to interfere with the torch while cutting. The entire sheet can pierced and then cleaned off prior to cutting.

It is possible to use near-end-of-life consumables for piercing and then they can be swapped out for good consumables to be used while cutting.

Pierce Only is one of two different cut types

Puddle Jump is the height that the torch will move to after piercing and prior to moving to Cut Height and is expressed as a percentage of Pierce Height. This allows the torch to clear any puddle of molten material that may be caused by piercing. The maximum allowable height is 200% of the Pierce Height

Setting for Puddle Jump are described in cut parameters

The recommended option is to use Pierce Only due to it being able to utilise near end of life consumables.

QtPlasmaC is capable of cutting of expand (mesh) metal provided the machine has a pilot arc torch and it is capable of Constant Pilot Arc (CPA) mode.

Mesh Mode disables the THC and also ignores a lost Arc OK signal during a cut. It can be selected by checking the Mesh Mode check button in the CONTROL section of the MAIN Tab.

If the machine has RS485 communications enabled with a Hypertherm PowerMax plasma cutter, selecting Mesh Mode will automatically override the Cut Mode for the currently selected material and set it to cut mode 2 (CPA). When Mesh Mode is disabled, the Cut Mode will be return to the default cut mode for the currently selected material.

It is also possible to start a Mesh Mode cut without receiving an Arc OK signal by checking the Ignore Arc OK check button in the CONTROL section of the MAIN Tab.

Both Mesh Mode and Ignore Arc OK can be enabled/disabled at any time during a job.

Ignore Arc OK mode disables the THC, will begin a cut without requiring an Arc OK signal, and will ignore a lost Arc OK signal during a cut.

This mode can be selected by:

It is important to thoroughly understand the difference between Synchronized with motion and Immediate:

This mode may also be used in conjunction with Mesh Mode if the user doesn’t require an Arc OK signal to begin the cut.

Both Mesh Mode and Ignore Arc OK can be enabled/disabled at any time during a job.

This feature will produce a CUT RECOVERY panel that will allow the torch to be moved away from the cut path during a paused motion event in order to position the torch over a scrap portion of the material being cut so that the cut restarts with a minimized arc-divot. The CUT RECOVERY panel will display automatically over top of the JOGGING panel when motion is paused.

It is preferable to make torch position adjustments from the point at which paused motion occurred, however if moving along the cut path is necessary prior to setting the new start point, the user may use the paused motion controls (REV, FWD, and a JOG-SPEED slider) at the top of the CUT RECOVERY panel. Once the user is satisfied with the positioning of the torch along the cut path, moving off the cut path is achieved by pressing the DIRECTION buttons. Each press of the DIRECTION button will move the torch a distance equivalent to the Kerf Width parameter of the currently selected material.

The moment the torch has been moved off the cut path, the paused motion controls (REV, FWD, and a JOG-SPEED slider) at the top of the CUT RECOVERY panel will become disabled.

Once the torch position is satisfactory, press CYCLE RESUME and the cut will resume from the new position and travel the shortest distance to the original paused motion location. The CUT RECOVERY panel will close and the JOGGING panel will display when the torch returns to the original paused motion location.

Pressing CANCEL MOVE will cause the torch to move back to where it was positioned before the direction keys were used to offset the torch. It will not reset any REV or FWD motion.

Pressing CYCLE STOP will cause the torch to move back to where it was positioned before the direction keys were used to offset the torch and the CUT RECOVERY panel overlay will return to the JOGGING panel. It will not reset any REV or FWD motion.

If an alignment laser has been set up then it is possible to use the laser during cut recovery for very accurate positioning of the new start coordinates. If either the X axis offset or Y axis offset for the laser would cause the machine to move out of bounds then an error message will be displayed.

To use a laser for cut recovery when paused during a cut:

If a laser offset is in effect when CANCEL MOVE is pressed then this offset will also be cleared.

If the user has the Run From Line option enabled in the GUI SETTINGS section of the SETTINGS Tab then they will have the ability to start from any line in a G-code program via the following methods:

Note that the "Run From Line"-function will run from the beginning of the selected line.

It is important to note that G-code programs can be run from any selected line using this method, however a leadin may not be possible depending on the line selected. In this case, an error message will be displayed to let the user know the leadin calculation was not possible.

Once the user has selected the starting place, the CYCLE START button will blink "SELECTED nn" where nn is the corresponding line number selected. Clicking this button will bring up the following Run From Line dialog box:

It is not possible to use Run From Line from within a subroutine. If the user selects a line within a subroutine and clicks "SELECTED nn" then an error message will be displayed that includes the O-code name of the subroutine.

It is not possible to use Run From Line if previous G-code has set cutter compensation active. If the user selects a line while cutter compensation is active and clicks "SELECTED nn" then an error message will be displayed.

It is possible to select a new line while Run From Line is active.

After pressing LOAD, the blinking "SELECTED nn" button will change to RUN FROM LINE CYCLE START button. Click this button to start the program from the beginning of the selected line.

Run From Line selections may be canceled in the following ways:

A scribe may be operated by QtPlasmaC in addition to the plasma torch.

Using a scribe requires the use of the LinuxCNC tool table. Tool 0 is assigned to the plasma torch and Tool 1 is assigned to the scribe. The scribe X and Y axes offsets from the plasma torch need to be entered into the LinuxCNC tool table. This is done by editing the tool table via the main GUI, or by editing the tool.tbl file in the <machine_name> configuration directory. This will be done after the scribe can move to the work piece to help determine the appropriate offset.

The plasma torch offsets for X and Y will always be zero. The tools are selected by the Tn M6 command followed by a G43 H0 command which is required to apply the offsets. The tool is then started with a M3 $n S1 command. For n, use 0 for torch cutting or 1 for scribing.

To stop the scribe, use the G-code command M5 $1.

If the user has not yet assigned the HAL pins for the scribe in the configuration wizard then they may do so by using the appropriate configuration wizard or by manually editing the HAL file, see modifying QtPlasmaC.

There are two HAL output pins used to operate the scribe, the first pin is used to arm the scribe which moves the scribe to the surface of the material. After the Arm Delay has elapsed, the second pin is used to start the scribe. After the On Delay has elapsed, motion will begin.

Using QtPlasmaC after enabling the scribe requires the selection of either the torch or the scribe in each G-code file as a LinuxCNC tool.

The first step is to set the offsets for the scribe by following the procedure described in Peripheral Offsets.

The final step is to set the scribe delays required:

Save the parameters in the Config tab.

After the above directions are completed, the scribe may be tested manually by issuing a M3 $1 S1 command in the MDI input. The user may find it helpful to use this method to scribe a small divot and then try to pulse the torch in the same location to align the offsets between the scribe and the torch.

To use the scribe from G-code:

It is a good idea to switch back to the torch at the end of the program before the final rapid parking move so the machine is always in the same state at idle.

The user can switch between the torch and the scribe any number of times during a program by using the appropriate G-codes.

Issuing M3 S1 (without $n) will cause the machine to behave as if an M3 $0 S1 had been issued and issuing M5 (without $n) will cause the machine to behave as if an M5 $0 had been issued. This will control the torch firing by default in order to provide backward compatibility for previous G-code files.

To achieve spotting to mark the material prior to drilling etc., QtPlasmaC can pulse the torch for a short duration to mark the spot to drill.

Spotting can be configured by following these steps:

The torch is then turned on in G-code with the M3 $2 S1 command which selects the plasma torch as a spotting tool.

To turn the torch off, use the G-code command M5 $2.

For more information on multiple tools, see multiple tools.

LinuxCNC (QtPlasmaC) requires some motion between any M3 and M5 commands. For this reason, a minimal movement at a high speed is required to be programmed.

An example G-code is:

Virtual keyboard support is available for only the "onboard" onscreen keyboard. If it is not already on the system it may be installed by typing the following in a terminal:

The following two custom layouts are used for soft key support:

If the virtual keyboard has been repositioned and on the next opening of a virtual keyboard it is not visible then clicking twice on the onboard icon in the system tray will reposition the virtual keyboard so the move handle is visible.

Below is a list of all available keyboard shortcuts in QtPlasmaC.

In order to utilize them, KB Shortcuts must be enabled in the GUI SETTINGS section of the SETTINGS Tab.

In addition to the typical G and M codes that are allowed by LinuxCNC in MDI mode, the MDI in QtPlasmaC can be used to access several other handy features. The following link outlines the features and their use: [sub:qtvcp:widgets:mdiline][MDILine Widget]

In addition, pressing RETURN (or ENTER) with no entry in the MDI will close the MDI window.

Global settings for the shape library can be set by pressing the SETTINGS button in the CONVERSATIONAL Tab. This will display all of the available settings parameters that are used for G-code program creation. These include:

Any internal circle that has a diameter less than Small hole diameter is classified as a small hole and will have a straight leadin with a length that is the lesser of either the radius of the hole or the specified leadin length. It will also have its feed rate set to Small hole speed.

Preamble and Postamble may be entered as a string of G-Codes and M-Codes separate by spaces. If the user wishes for the generated G-code to have each code on an individual line then this is made possible by separating the codes with \n.

This will place all codes on the same line:

This will place each code on its own line:

Pressing the RELOAD button will discard any changed but unsaved settings.

Pressing the SAVE button will save all the settings as displayed.

Pressing the EXIT button will close the setting panel and return to the previous shape.

Lines and arcs have an additional option in that they may be strung together to create a complex shape.

There are two line types and three arc types available:

To use lines and arcs:

If the user wishes to create a closed shape, they will need to create any required leadin as the first segment of the shape. If a leadout is required it will need to be the last segment of the shape.

The following shapes are available for creation:

To create a shape:

For CIRCLE, the OVER CUT button will become valid when a CUT TYPE of INTERNAL is selected and the value entered in the DIAMETER field is less than the Small Hole Diameter parameter in the Conversational SETTINGS section.

For BOLT CIRCLE the OVER CUT button will become valid if the value entered in the HOLE DIA field is less than the SMALL HOLES DIAMETER parameter in the Conversational SETTINGS section.

For the following shapes, KERF OFFSET will become active once a LEAD IN is specified:

Multiple shapes can be added together to create a complex group.

The cut order of the group is determined by the order in which the individual shapes are added to the group.

Once a shape is added to the group it cannot be edited or removed.

Groups cannot have shapes removed, only added to.

To create a group of shapes:

The Conversational Block feature allows block operations to be performed on the current shape or group of shapes displayed in the CONVERSATIONAL Tab. This can include a G-code file not created using the Conversational Shape Library that has been previously loaded from the MAIN Tab.

A previously saved Block G-code file may also be loaded from the MAIN Tab and then have any of its operations edited using the Conversational Block feature.

Block operations:

To create a block:

If the result is an array of shapes then the cut order of the result is from the left column to the right column, starting at the bottom row and ending at the top row.

The current job displayed in the Preview Panel may be saved at any time by using the bottom SAVE button. If the G-code has been sent to LinuxCNC (QtPlasmaC) and the user has left the CONVERSATIONAL Tab, the user may still save the G-code file from the GUI. Alternatively, the user could click the CONVERSATIONAL Tab which will reload the job, at which time they can press the SAVE button.

All errors are logged into the machine log which is able to be viewed in the STATISTICS Tab. The log file is saved into the configuration directory when QtPlasmaC is shutdown. The five last logfiles are kept, after which the oldest logfile is deleted each time a new log file is created. These saved log files may be viewed with any text editor.

By default, QtPlasmaC will display error messages via a Operator Error popup window. In addition, QtPlasmaC will alert the user that an error has been sent to the machine log by displaying the message "ERROR SENT TO MACHINE LOG" in the lower left portion of the status bar.

The user may opt to disable the Operator Error popup window, and view the error messages by going to the STATISTICS Tab by changing the following option to False in the [SCREEN_OPTIONS] of the <machine_name>.prefs file in the <machine_name> directory:

Additionally, it is possible for ERROR SENT TO MACHINE LOG to flash to get the user’s attention by adding or editing the following option in the [GUI_OPTIONS] section of the <machine_name>.prefs file:

There are a number of error messages printed by QtPlasmaC to inform the user of faults as they occur. The messages can be split into two groups, Critical and Warning.

Critical Errors will cause the running program to pause, and the operator will need to clear the cause of the error before proceeding.

If the error was received during cutting then forward or reverse motion is allowed while the machine is paused to enable the user to reposition the machine prior to resuming the cut.

When the error is cleared the program may be resumed.

These errors indicate the corresponding sensor was activated during cutting:

These errors indicate the corresponding sensor was activated before probing commenced:

The Arc OK signal was lost during cutting motion, before the M5 command was reached:

The Z axis reached the bottom limit before the work piece was detected:

The work piece is too high for any safe rapid removes:

One of these values in MATERIAL section of the PARAMETERS Tab is invalid (For example: if they are set to zero):

No arc has been detected after attempting to start the number of times indicated by Max Starts in the ARC frame of the CONFIGURATION section of the PARAMETERS Tab:

THC has caused the bottom limit to be reached while cutting:

THC has caused the top limit to be reached while cutting:

These errors indicate move to pierce height would exceed the Z Axis MAX_LIMIT for the corresponding probe method:

These errors indicate the move to pierce height would exceed the Z axis maximum safe height for the corresponding probe method:

Warning messages will not pause a running program and are informational only.

These messages indicate the corresponding sensor was activated before a probe test commenced:

This indicates that the corresponding sensor was activated during a consumable change:

This indicates that the corresponding sensor was activated during probe testing:

This indicates that probe contact was lost before probing up to find the zero point:

This indicates that the bottom limit was reached during a probe test:

This indicates that the move to pierce height would exceed the Z Axis MAX_LIMIT during the corresponding probe method:

This indicates that the safe height has been reduced due to THC raising the Z axis during cutting:

This indicates that the value for the Arc Voltage was invalid (NAN or INF) when QtPlasmaC launched.

QtPlasmaC update notices are posted at https://forum.linuxcnc.org/plasmac/37233-plasmac-updates .

Users are strongly encouraged to create a Username and subscribe to the above thread to receive update notices.

For a standard ISO installation, LinuxCNC will only be updated when a new minor release has been released. QtPlasmaC will then automatically update its configuration the first time it is run after a LinuxCNC update.

LinuxCNC is normally updated by entering the following commands into a terminal window (one at a time):

Enhancements and bug fixes will not be available on a standard installation until a new minor release of LinuxCNC has been released. If the user wishes to update whenever a new QtPlasmaC version has been pushed, they could use the LinuxCNC Buildbot repository rather than the standard LinuxCNC repository by following the instructions at http://buildbot.linuxcnc.org/ .

Adding style changes to the default stylesheet is achieved by creating a file in the <machine_name> configuration directory. This file MUST be named qtplasmac_custom.qss. Any required style changes are then added to this file.

For example the user may want the arc voltage display in red, a green Torch On LED of a larger size and a larger Torch Enable button. This would be done with the following code in qtplasmac_custom.qss:

Custom stylesheets are enabled by setting the following option in the [GUI_OPTIONS] section of the <machine_name>.prefs file. This option must be set to the filename of the stylesheet as shown below.

The filename may be any valid filename. The standard extension name is .qss but this is not mandatory.

There are some constraints on the custom stylesheet for QtPlasmaC, e.g., the jog buttons, cut-recovery buttons, and the conversational shape buttons are image files and are not able to be custom styled.

The custom style file requires a header in the following format:

The colors may be expressed in any valid stylesheet format.

The above colors are used for the following widgets. So any custom styling will need to take these into account. The colors shown below are the defaults used in QtPlasmaC along with the color name from the SETTINGS Tab.

The user may return to the default styling at any time by following the following steps:

The next time QtPlasmaC is loaded all custom styling will be removed and the default styling will return.

Below is an example of the section and options to be deleted from <machine_name>.prefs:

It is possible to add custom Python code to change some existing functions or to add new ones. Custom code can be added in two different ways: a user command file or a user periodic file.

A user command file is specified in the DISPLAY section of the <machine_name>.ini file and contains Python code that is processed only once during startup.

A user periodic file must be named user_periodic.py and must be loaded in the machines config directory. This file is processed every cycle (usually 100 ms) and is used for functions that require regular updating.

All incoming G-code is parsed by a G-code filter to ensure it is suitable for QtPlasmaC. It is possible to extend this filter with custom python code executed from a file in the configuration directory to aid in converting different flavours of G-code to a format suitable for QtPlasmaC.

The name of this file is custom_filter.py and it will be automatically used if it exists.

There are three preset methods available for use:

These methods are applied by the following procedure:

For example to remove any code beginning with G71 and change M2 to M5 $0 and M2:

In addition to these it is also possible to override any existing method in the filter the same way. This requires defining the same number of arguments as the existing method, noting that self in the original does not constitute an argument.

The QtPlasmaC GUI offers user buttons that can be customized by adding commands in the USER BUTTON ENTRIES section of the SETTINGS Tab in the <machine_name>.prefs file.

The number of user buttons varies by display type and resolution as follows:

The user will need to run QtPlasmaC at the desired screen size to determine how many user buttons are available for use.

All <machine_name>.prefs file settings for the buttons are found in the [BUTTONS] section.

The text that appears on the button is set the following way:

Where n is the button number and HAL Show is the text.

For text on multiple lines, split the text with a \ (backslash):

If an ampersand is required to be displayed as text then two consecutive ampersands are required:

Buttons can run the following:

To run an external command, the command is preceded by a % character.

To run an external Python script, the script name is preceded by a % character and it also requires a .py extension. It is valid to use the ~ character as a shortcut for the users home directory.

To run G-code, just enter the code to be run.

To run an existing subroutine.

<machine_name>.ini file variables can be entered by using the standard LinuxCNC G-code format. If expressions are included then they need to be surrounded by brackets.

<machine_name>.prefs file variables and also <machine_name>.ini variables can be entered by enclosing each option in {} . You must put a space after each } if there are any following characters. If expressions are included then they need to be surrounded by brackets.

Multiple codes can be run by separating the codes with a "\" (backslash) character. The exception is the special commands which are required to be a single command per button.

External commands and G-code may be mixed on the same button.

The following code will allow the user to use a button to invert the current state of a HAL bit pin:

This code is required to be used as a single command and may only control one HAL bit pin per button.

The button colors will follow the state of the HAL pin.

After setting the code, upon clicking, the button will invert colors and the HAL pin will invert pin state. The button will stay "latched" until the button is clicked again, which will return the button to the original colors and the HAL pin to the original pin state.

There are three External HAL Pins that are available to toggle as an output, the pin names are qtplasmac.ext_out_0, qtplasmac.ext_out_1, and qtplasmac.ext_out_2. HAL connections to these HAL pins need to be specified in a postgui HAL file as the HAL pins are not available until the QtPlasmac GUI has loaded.

For toggle-halpin buttons, it is possible for the user to mark the associated HAL pin as being required to be turned "ON" before starting a cut cycle by adding "runcritical" after the HAL pin in the button code. If TORCH ENABLE is checked and CYCLE START is pressed while the "runcritical" button is not "ON" then the user will receive a dialog warning them as such and asking to CONTINUE or CANCEL.

The following code will allow the user to use a button to invert the current state of the alignment laser HAL bit pin:

This code is also able to be used as a multiple command with G-code or external commands but may control only the alignment laser HAL bit pin.

The button colors will follow the state of the alignment laser HAL pin.

After setting the code, upon clicking, the button will invert colors and the alignment laser HAL pin will invert pin state. The button will stay "latched" until the button is clicked again, which will return the button to the original colors and the alignment laser HAL pin to the original pin state.

The following code would allow the user to use a button to invert the current state of the alignment laser HAL bit pin and then move the X and Y axes to the offset for the alignment laser as specified in the <machine_name>.prefs file:

The position of the "toggle-laser" command is not important as it is always the first command actioned regardless of position.

The following code will allow the user to use a button to pulse a HAL bit pin for a duration of 0.5 seconds:

This code is required to be used as a single command and may only control one HAL bit pin per button.

The pulse duration is specified in seconds, if the pulse duration is not specified then it will default to one second.

The button colors will follow the state of the HAL pin.

After setting the code, upon clicking the button, the button will invert colors, the HAL pin will invert pin state, and the time remaining will be displayed on the button. The button color and the pin state will stay inverted until the pulse duration timer has completed, which will return the button to the original colors, the HAL pin to the original pin state, and the original button name.

An active pulse can be canceled by clicking the button again.

There are three External HAL Pins that are available to pulse as an output, the pin names are qtplasmac.ext_out_0, qtplasmac.ext_out_1, and qtplasmac.ext_out_2. HAL connections to these HAL pins need to be specified in a postgui HAL file as the HAL pins are not available until the QtPlasmac GUI has loaded.

QtPlasmaC will begin a probe and when the material is detected, the Z axis will rise to the Pierce Height currently displayed in the MATERIAL section of the PARAMETERS Tab. If the user has "View Material" selected in the GUI SETTINGS section of the SETTINGS Tab, this value will be displayed in the top left corner of the PREVIEW Window next to PH:.

QtPlasmaC will then wait in this state for the time specified (rounded to no decimal places) before returning the Z axis to the starting position. An example of a 6 second delay is below. If there is no time specified then the probe time will default to 10 seconds.

QtPlasmaC will enable the Ohmic Probe Enable output signal and if the Ohmic Probe input is sensed, the LED indicator in the SENSOR Panel will light. The main purpose of this is to allow a quick test for a shorted torch tip.

This button if selected will toggle between the two cut types, Pierce and Cut (default cutting mode) or Pierce Only.

Pressing this button moves the torch to the specified coordinates when the machine is paused to allow the user easy access to change the torch consumables.

Valid entries are Xnnn Ynnn Fnnn. At least one of the X or Y coordinates are required, Feed Rate (F) is optional.

The X and Y coordinates are in absolute machine coordinates. If X or Y are missing then the current coordinate for that axis will be used.

Feed Rate (F) is optional, if it is missing or invalid then the feed rate of the current material will be used.

There are three methods to return to the previous coordinates:

Loading a G-code program from the directory specified by the PROGRAM_PREFIX variable in the <machine_name>.ini file (usually ~/linuxcnc/nc_files) is possible by using the following format:

If the user’s G-code file is located in a sub-directory of the PROGRAM_PREFIX directory, it would be accessed by adding the sub-directory name to the beginning of the G-code file name. Example for a sub-directory named plasma:

Note that the first "/" is not necessary as it will be added automatically.

Pulse the torch on for a predetermined time. The time must be specified in seconds using up to one decimal place. The maximum allowable time is 3 seconds, anything specified above that value will be limited to 3 seconds. An example of a 0.5 second pulse is below. It there is no time specified then it will default to 1 second. Pulse times with more than one decimal place will be rounded to one decimal place.

Pressing the button again during the countdown will cause the torch to be turned off, as will pressing Esc if keyboard shortcuts are enabled in the SETTINGS Tab.

If the button is released before the countdown is complete then the torch will turn off at countdown completion, holding the button on until after the countdown has completed will cause the torch to remain on until the button has been released.

Run a single unidirectional cut. This utilises the automatic Single Cut feature.

Framing is the ability to move the torch around the perimeter of a rectangle that encompasses the bounds of the current job.

The laser enable HAL pin (qtplasmac.laser_on) will be turned on during the framing moves and any X/Y offsets for the laser pointer in the <machine_name>.prefs file will also be applied to the X/Y motion. After the framing motion is completed, the torch will move to the X0 Y0 position to clear any applied laser offsets and qtplasmac.laser_on will be turned off.

Upon starting a Framing cycle, it is important to note that by default the Z axis will be moved to a height of [AXIS_Z]MAX_LIMIT - 5 mm (0.2") before X/Y motion begins.

The velocity for the XY movements of the Framing motion can be specified so that Framing motion always occurs at a set velocity. This can be achieved by adding the feed rate (F) as the as the last portion of the button code. If the feed rate is omitted from the button code, framing motion velocity will default to the feed rate for the currently selected material.

The following GUI buttons and Keyboard Shortcuts (if enabled in the SETTINGS Tab) are valid during Framing motion:

It is possible for the user to omit the initial default Z movement and run the framing sequence at the current Z height by adding "usecurrentzheight" after "framing".

To specify a feed rate:

or:

Enabling a user button as a framing button will add an external HAL pin that may be connected from a pendant etc. HAL connections to this HAL pin needs to be specified in a postgui HAL file as the HAL pin is not available until the QtPlasmac GUI has loaded.

Manual Cut functions identically to the F9 button to begin or end a manual cut.

This allows the showing/hiding of an offset viewing screen that displays all machine offsets. All relative offsets can be edited and the G54 ~ G59.3 work system coordinates are able to be given custom names.

This allows the loading of the last modified file in a directory. The directory name is optional and if omitted will default to the last directory a file was loaded from.

This allows the showing/hiding of the online HTML user manual specific to the version of LinuxCNC currently running. Note that internet access is required for this functionality.

Use the following sequence to set the offsets for a laser, camera, scribe, or offset probe:

Canceling may be done at any stage by pressing the CANCEL button which will close the dialog and no changes will be saved.

If CAMERA was selected at item 7 above and more than one camera exists then a camera selection dialog will show. The appropriate camera needs to be selected before the Get Peripheral Offsets dialog will appear.

If PROBE was selected at item 7 above then a delay dialog will show prior to the confirmation dialog at item 11. This is for the delay required for the probe to deploy to its working position.

By default, QtPlasmaC will remove all Z motion from a loaded G-code file and add an initial Z movement to bring the torch near the top of travel at the beginning of the file. If the user wishes to use their table with a marker, a drag knife, diamond scribe, etc. mounted in the torch holder, QtPlasmaC has the ability to retain the Z movements when executing a program by adding the following command in a G-code file:

Omitting this command, or setting this value to anything but 1 will cause QtPlasmaC to revert to the default behavior of stripping all Z motion from a loaded G-code file and making an initial Z movement to bring the torch near the top of travel at the beginning of the file.

QtPlasmaC creates some HAL pins that may be used to connect a momentary external button or pendant etc.

HAL connections to these HAL pins need to be specified in a postgui HAL file as the HAL pins are not available until the QtPlasmac GUI has loaded.

The following HAL bit pins are always created. The HAL pin has the identical behaviour of the related QtPlasmaC GUI button.

The following HAL pins which allow the use of an MPG to control height override are always created.

The following HAL bit pins are only created if the function is specified in a custom user button. The HAL pin has the identical behaviour of the related custom user button.

The following HAL bit output pins are always created and can be used by either the Toggle HAL Pin or Pulse HAL Pin custom user buttons to change the state of an output.

If the user has external buttons and/or a pendant that emulates any of the program buttons, CYCLE START, CYCLE PAUSE, or CYCLE STOP then it is possible to hide any or all of these GUI program buttons by adding the following options to the [GUI_OPTIONS] section of the <machine_name>.prefs file:

For the 16:9 or 4:3 GUIs, the hiding of each of these GUI buttons will expose two more custom user buttons in the GUI.

Mode 0 Arc OK relies on the arc voltage to set the Arc OK signal. This is accomplished by sampling the arc voltage every servo thread cycle. There needs to be a specified number of consecutive samples, all within a specified threshold for the Arc OK signal to be set. These voltages are also required to be within a specified range.

There are two settings in the PARAMETERS Tab for setting the range, these are:

Both of these values may be changed by direct entry or by the use of the increment/decrement buttons.

There are also two HAL pins that have been provided to allow the user to tune the set point. These HAL pins are:

The following example would set the number of valid consecutive readings required to 6:

These settings if used should be in the custom.hal file of the configuration.

Some plasma power sources/machine configurations may lose the Arc OK signal either momentarily during a cut, or permanently near the end of a cut causing QtPlasmaC to pause the program and report a "valid arc lost" error.

There is a HAL pin named plasmac.arc-lost-delay that may be used to set a delay (in seconds) that will prevent a paused program/error if the lost Arc OK signal is regained, or the M5 command is reached before the set delay period expires.

It is important to note that the THC will be disabled and locked at the cutting height at the time the Arc OK signal was lost.

The following code would set a delay of 0.1 seconds:

It is recommended that the user set this pin in the custom.hal file.

This setting should only be used if the user experiences the above symptoms. It should also be noted that the user could use the appropriate Ignore Arc OK G-code commands to achieve a similar result.

Small fluctuations in the arc voltage displayed while the machine is at idle are possible depending on many different variables (electrical noise, incorrect THCAD tuning, etc.).

After all contributing factors have been mitigated, if a small fluctuation still exists it is possible to eliminate it by widening the voltage window for which QtPlasmaC will display 0 V.

The pin for adjusting this value is named plasmac.zero-window and the default value is set to 0.1. To change this value, add the pin and the required value to the custom.hal file.

The following example would set the voltage window to be displayed as 0 V from -5 V to +5 V:

In addition to the Void Slope setting in the PARAMETERS Tab there are two HAL pins to aid in the fine tuning of void anti-dive. These HAL pins are:

The following example would set the number of on cycles required to 3:

The objective is to have as low a value of Void Slope as possible without any false triggering then adjust on and off cycles to ensure clean activation and deactivation of void anti-dive. In most cases it should not be necessary to change on and off cycles from the default value.

These settings if used should be in the custom.hal file of the configuration.

Max Offset is the distance (in millimeters) away from the Z MAX_LIMIT that QtPlasmaC will allow the Z axis to travel while under machine control.

The pin for adjusting this value is named plasmac.max-offset and the default value (in millimeters) is set to 5. To change this value, add the pin and the required value to the custom.hal file. It is not recommended to use values less than 5 mm as offset overrun may cause unforeseen issues.

The following example would set the distance from Z MAX_LIMIT to 10 mm:

By default, all tabs except the MAIN Tab are disabled during automated motion. It is possible for every tab but the CONVERSATIONAL Tab to be enabled during automated motion by setting the following HAL pin True:

It is possible to override the jog inhibit by using the GUI or keyboard to jog in the Z+ direction rather than checking the Override Jog box on the SETTINGS Tab.

This is done by changing the following option to True in the [GUI_OPTIONS] of the <machine_name>.prefs file in the <machine_name> folder:
Override jog inhibit via Z+

The plasmac HAL component has a HAL pin named plasmac.state-out which can be used to interface with user-coded components to provide the current state of the component.

The DEBUG state is for testing purposes only and will not normally be encountered.

The plasmac HAL component has a HAL pin named plasmac.debug-print which if set to 1 (true) will print to terminal every state change as a debug aid.

Communications can be established with a Hypertherm PowerMax plasma cutter that has a RS485 port. This feature enables the setting of Cut Mode, Cutting Amperage and Gas Pressure automatically from the Cut Parameters of the material file. In addition, the user will be able to view the PowerMax’s Arc On Time in hh:mm:ss format on the STATISTICS Tab.