PlasmaC User Guide

Installation instructions are available at: http://linuxcnc.org/docs/devel/html/getting-started/getting-linuxcnc.html

Following these instructions will yield a machine with the current stable branch (v2.8) of LinuxCNC.

Upgrading instruction are available at: http://linuxcnc.org/docs/devel/html/getting-started/updating-linuxcnc.html

Following these instructions will yield a machine with the current stable branch (v2.8) of LinuxCNC.

Some recommended settings:

where: o = overrun, a = acceleration in units/sec2 and v = velocity in units/sec.

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

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

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.

The user may opt to create a base machine manually or one of the existing configuration helpers may be used:

If using a Mesa Electronics board, use the pncconf wizard (enter the following command into a terminal window):

If using a parallel port, use the stepconf wizard (enter the following command into a terminal window):

If using a Pico Systems board:
This LinuxCNC forum thread may be helpful.

If the user already has a dual motor gantry configuration that requires the configuration to be hand edited:
This LinuxCNC forum thread may be helpful.

ONLY WHEN this criteria is met should the user proceed with configuring PlasmaC "on top" of a working machine by running the configurator.

PlasmaC 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 PlasmaC GUI.

Breakaway Switch is not mandatory because 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.

The selection window is now visible:

Select New from the selection window, this will show an info dialog, select Continue and the New Configuration window will display.

HAL connection examples in the following table show examples for both a parallel port config and a Mesa 7i96 config. Change the pin names as required to suit the breakout board configuration.

Fill in the required entries to suit the machine wiring/breakout board configuration, click Create and a working PlasmaC configuration will be created in the following directory: ~/linuxcnc/configs/<machine_name>

The newly created PlasmaC configuration can be run by entering the following command into a terminal window (change "<machine_name>" to the machine name entered into the PlasmaC configurator):

After creating a new configuration some initial setup is required before using the PlasmaC component.

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

After running the command at the end of section 5.1, LinuxCNC should be running with the PlasmaC panels visible.

Click on the Config tab to open the Config Panel and 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 PlasmaC, 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 Config Panel. This will be done by running a "Probe Test" cycle.

The Configurator may also be used to reconfigure an existing PlasmaC configuration to change settings instead of modifying files manually.

The Configurator is only able to modify:

Reconfiguring a PlasmaC configuration is done from the Configurator which is located in the configuration directory.

It is recommended that a backup copy of the existing PlasmaC configuration is made before proceeding.

To start the configurator enter the following command into a terminal window:

The selection window is now visible:

Select Reconfigure from the selection window, this shows an info dialog, select Continue and the Reconfigure window will display:

Select the <machine_name>.ini file of the PlasmaC configuration to reconfigure.

If the user changes modes, the entry boxes will change depending on the currently selected mode.

When all entries are correct, click Reconfigure and the user’s PlasmaC configuration will be reconfigured.

Entry descriptions can be found here

The PlasmaC component has an 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 <machine_name>_connections.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 interpreting a very quick on-off of the input. One method of mitigating contact bounce is to "debounce" the input. To summarize debounce, as soon as the software sees an input with a debounce delay change states, it waits for a prescribed delay period before checking the state of the input again. After the debounce period the software will regard state changes as normal behavior of the input and react accordingly.

Debounce periods can be changed by editing the appropriate debounce value in the <machine_name>_connections.hal file in the <machine_name> config folder.

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 5000000ns, or 5ms.

For the Float and Ohmic switches this equates to a 0.001mm (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.

There are two versions of contact debouncing available in PlasmaC. The method used is determined by when the configuration was first created. There is no automatic update method available to convert from the original debounce setup to the alternate debounce setup as it is difficult to apply the necessary changes without understanding any manual edits that may have been made to the machine’s configuration files and potentially "breaking" a working configuration. If the user wishes to change from the original setup to the new setup, they must do so manually.

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 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 PlasmaC installation, the following files are created in the configuration directory:

In addition to the above files, the following links are created to files or directories in the source directory:

Finally, the following directories are created:

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

PlasmaC requires some specific <machine_name>.ini file variables as follows:

PlasmaC makes several modifications to the GUI. Some additions are panels on permanent display and others are tabs behind the preview tab.

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

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

If the user is using PlasmaC without multiple tools enabled then 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.

See recommended Z axis settings.

Each time LinuxCNC (PlasmaC) is started Joint homing is required. This allows LinuxCNC (PlasmaC) 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 PlasmaC 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 Touch Off with the Z axis selected to set the Z axis at zero offset. This should not need to be done again.

Before starting a program, jog the Z axis up to approximately 5mm (0.196") from the top of travel (Z Axis MAXIMUM_LIMIT). Leave the Z axis at this position as PlasmaC will control all Z axis motion while running a program, and park the Z Axis in this position when the program completes.

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.

The provided RS274NGC_STARTUP_CODE files: metric_startup.ngc and imperial_startup.ngc set the motion blending path tolerance with a G64 command P value to 0.1mm and 0.004" respectively. The P value corresponds to the amount the actual cut path followed by the machine may deviated from the programmed cut path before reducing velocity. If LinuxCNC (PlasmaC) receives an E-stop signal at any stage, the path tolerance will be set to the default (no P value) which will maintain the best possible speed and round corners off as a result. To prevent this, 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.

For Metric:

For Imperial:

PlasmaC 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 Cut Parameters section of the Run Panel has expired, PlasmaC will proceed with the M5 command to turn off and raise the torch.

PlasmaC has the ability to allow the use of more than one tool when running a cut program. Multiple tools must be enabled in PlasmaC before they can be used. Valid tools are:

If multiple tools are enabled then a LinuxCNC tool number (designated by $n) is required to be in the M3 command to select the correct tool to be used. Examples:

To enable the multiple tools feature the user will need to edit the following line in the <machine_name>_connections.hal file.

from:

to:

In order to use multiple tools with a scribe, it is necessary for the user to add the X and Y axis offsets to the LinuxCNC tool table. The tool.tbl file is found in the <machine_name> config folder. 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.

For example:

Material handling uses a material file that was created for the machine configuration when the configurator 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.

PlasmaC does not require the use of a material file. Instead, the user could change the cut parameters manually from the Run Panel. 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.

The THC can be controlled from the THC frame of the Run Panel.

The THC can also be enabled or disabled directly from the G-Code program provided that THC is not disabled in the THC section of the Run Panel.

PlasmaC uses a control voltage which is dependent on the state of the Use Auto Volts checkbox in the Run Panel:

The THC does not become active until the velocity reaches 99.9% of the CutFeedRate.

G-Code THC

THC may be disabled and enabled directly from G-Code, provided the THC is not disabled in the Run Panel, 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:

Velocity Based THC

If the cut velocity falls below a percentage of CutFeedRate (as defined by the VAD Threshold % value in the THC frame of the Config Panel) the THC will be locked until the cut velocity returns to at least 99.9% of CutFeedRate. This will be made apparent by the THC Velocity Lock indicator illuminating in the Monitor Panel.

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 (PlasmaC) 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:

IHS may be skipped in one of two different ways:

A value of zero for Skip IHS will disable 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.

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-probe-offset in the Config Panel.

Probing setup is done in the Probing frame of the Config Panel. Probing speed is controlled in the Motion frame of the Config Panel.

PlasmaC 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.

PlasmaC allows two different cut modes:

Pierce Only mode is useful for thick materials which may produce enough dross on the material surface from piercing to interfere with the torch while cutting. This enables the entire sheet to be pierced and cleaned off before cutting.

This also enables near-end-of-life consumables to be used for piercing and then they can be swapped out for good consumables to be used while cutting.

There are two ways of enabling this feature:

If using a custom user button is utilized then PlasmaC 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 32mm (1.26") are cut at 60% of the feed rate used for profile cuts. This should also lock out THC due to velocity constraints.

PlasmaC 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 PlasmaC 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.

Hole Cutting Velocity Reduction

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.

Sample code:

Arc Dwell (Pause At End)

This method can be invoked by setting the Pause At End parameter in the Cut Parameters frame of the Run Panel.

Overcut

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 PlasmaC 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 4mm (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:

PlasmaC has the ability to automatically modify the G-Code to reduce the velocity and/or apply Overcut which can be useful when cutting holes.

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

The default velocity for PlasmaC 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:

PlasmaC 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:

Arc Dwell (Pause At End)

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 Cut Parameters frame of the Run Panel.

Overcut

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

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

Sample code:

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 machines current X/Y position.

Automatic Single Cut

This is the preferred method. The parameters for this method are entered in the Run Panel.

Pendant 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 In Axis

Manual Single Cut In Gmoccapy

If the user wishes to use the keyboard jogging keys then enable keyboard shortcuts in the Hardware tab of the Settings page, otherwise the GUI jog buttons must be used.

PlasmaC 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 Cutting Mode section of the Run Panel.

If the machine has RS485 communications enabled with a Hypertherm PowerMax plasma cutter, selecting Mesh Mode will disable the Cut Mode spinbutton in the Cut Parameters section of the Run Panel and it will select cut mode 2 (CPA). When Mesh Mode is disabled, the Cut Mode spinbutton will be re-enabled and the original cut mode will be restored.

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 Cutting Mode section of the Run Panel.

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 dialog box 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. This feature is only available from a user-programmed button (named Cut-Recovery by default) in the Extras panel and may only be clicked while 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 dialog box. 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 dialog box will become disabled.

Once the torch position is satisfactory, press Resume Cut or the GUI’s Resume button (Pause symbol) and the cut will resume from the new position and travel the shortest distance to the original paused motion location. The dialog box will close when the torch returns to the original paused motion location.

Pressing Cancel (or the X in the title bar) will cause the torch to move back to where it was positioned when the motion became paused and the dialog box will close.

The Conversational Shape Library consists of several basic shapes and functions to assist the user with generating quick G-Code at the machine to cut simple shapes quickly. This feature is started by clicking the Conversational button found in the Extras tab.

Blank entries in the shape input boxes will use the current setting at the time the G-Code was generated. For example, if X start was left blank then the current X axis position would be used.

All lead-ins and lead-outs are arcs except for:

The cut order will occur in the same order as the shape was built.

Pressing Return on the keyboard while editing parameters will automatically show the preview of the shape if there are enough parameters entered to create the shape. Clicking any of the available check boxes will do the same.

The button functions are as follows:

If there is a G-Code file loaded in LinuxCNC (PlasmaC) when the Conversational Panel is opened, that code will be imported into the conversational as the first shape of the job. If this code is not required then it can be removed by pressing the New button.

A scribe may be operated by PlasmaC in addition to the plasma torch. This ability is disabled by default so as not to adversely affect existing configurations. To enable scribing, see the Multiple Tools section for guidance in editing the <machine_name>_connections.hal file.

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.

If the user has not yet assigned the HAL pins for the scribe in the Configurator then they will need to do so by invoking the reconfigure mode of the Configurator.

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

The next step is to open the tool table editor in the GUI or edit tool.tbl in the <machine_name> configuration directory and enter the X and Y axes offsets. These are the distances in X and Y the scribe is away from the torch as measured from the center of the torch nozzle. In most cases, if the user is standing at the front of the machine and the scribe is to the right of the torch, a positive X offset would be required. Similarly, if the scribe is to the rear of the torch, a positive Y offset would be required. The offsets for the torch should always be zero.

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., PlasmaC 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 enable spotting, see multiple tools.

LinuxCNC (PlasmaC) 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:

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.

If Gas Pressure is set to Zero then the PowerMax will automatically calculate the required pressure from the Cut Mode, Cut Current, torch type, and torch length.

Changing the cutting mode will set the gas pressure to zero causing the machine to use its automatic gas pressure mode.

The maximum and minimum values of these parameters are read from the plasma cutter and the related spin-buttons in the Cut Parameters are then limited by these values. Gas pressure can not be changed from zero until communications have been established.

This feature is enabled by setting the correct port name for the PM_PORT variable in the [PLASMAC] section of the <machine_name>.ini file. If the PM_PORT variable is not set in the <machine_name>.ini file then the widgets associated with this feature will not be visible.

Example showing enabling the Hypertherm PowerMax Communications on USB0:

If the user is unsure of the name of the port, there is a python script in the configuration directory that will show all available ports and can also be used to test communications with the plasma unit prior to enabling this feature in the PlasmaC GUI.

To use the test script enter the following command into a terminal window:

The gas pressure units display (psi or bar) is determined by the data received during initial setup of the communication link and is then shown next to the Gas Pressure spinbutton on the Run Panel.

The PowerMax machine will go into remote mode after communications have been established and may only be controlled remotely (via the PlasmaC GUI) at this point. The connection can be validated by observing the PowerMax display.

To switch the PowerMax back to local mode the user can either:

To install pyserial, enter the following command into a terminal window:

A typical connection diagram is shown in the appendix of this document as well as confirmed working interfaces.

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

PlasmaC 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.

There are buttons available in the PlasmaC GUI that are programmable by adding commands in the <machine_name>.ini file. The number of buttons varies by whether the user chose to use PlasmaC with Axis or Gmoccapy.

Five buttons are available in the main window of the Axis GUI, numbered 1-5 from left to right.

Four buttons are available in the main window of the Gmoccapy GUI, numbered 1-4 from top to bottom.

There are an additional ten buttons available in the Extras panel, numbered 10-19 from top left to bottom right.

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

There is a directory named test in the machine’s configuration folder which has a simple Test Panel and associated python file which can be used to test the example configuration as referenced in the <machine_name>.ini file.

If the user wishes to use this in a sim configuration then the user will need to create a link to this directory and edit the <machine_name>.ini file to suit.

Void sensing may be further tuned by adjusting the required number of consecutive times that the threshold has been exceeded before applying the void lock to the THC.

The parameter for adjusting this is named plasmac.kerf-errors-max and the default value is 2. To change this value, add the parameter and the required value to the <machine_name>_connections.hal file. The following example would set the required number of consecutive times to exceed the threshold to 3:

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 PlasmaC 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.

The following code would set a delay of 0.1 seconds:

It is recommended that the user set this parameter in the <machine_name>_connections.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.

PlasmaC has a HAL pin named plasmac.state-out which can be used to interface with user-coded components to provide PlasmaC’s current state.

The different states PlasmaC could encounter are as follows:

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

There are example configuration files for both the Axis and Gmoccapy GUIs which use the PlasmaC HAL component to simulate plasma cutting machines.

If the user has copied any example configs to the ~/linuxcnc/configs directory then they are able to be updated by running the Configurator in Update mode. This will replace any copied PlasmaC system file with a link to the latest version the user has updated to.

There are some sample G-Code files in nc_files/plasmac.

Before changing the type of installation, the existing PlasmaC installation needs to be updated to the latest version. If PlasmaC is not at the latest version then changing the installation type may corrupt the existing PlasmaC configuration.

It is recommended that a backup copy of the existing PlasmaC configuration is made before proceeding.

If the user has changed the type of LinuxCNC installation from a Package installation to a Run In Place or vice versa the user will need to run the Configurator from the new LinuxCNC installation directory, NOT from the ~/linuxcnc/configs directory. This is required to reset the file links for the correct installation type.

Enter the following command into a terminal window do one of the following:

Reset to a new Package installation:

Reset to a new Run In Place installation:

The Mesa THCAD is the most common way of obtaining the arc voltage from a plasma cutter. The THCAD may be used for parallel port configurations or for configurations using Mesa Electronics hardware.

The preferred method is to setup the required parameters for the THCAD in the <machine_name>_connections.hal file.

Hypertherm RS485 Wiring Diagram (wire colors inside the Hypertherm in parentheses):

RS485 interfaces that are known to work:

DTECH DT-5019 USB to RS485 converter adapter:

The following is necessary to convert a motherboard Serial connection or Serial card (RS232) to RS485:

DTECH RS232 to RS485 converter:

Serial card example (Sunnix SER5037A PCI Card shown with Breakout Board):

An effective and very reliable method of obtaining an Arc OK signal from a plasma power supply without a CNC port is to mount a reed relay inside a non-conductive tube and wrap and secure three turns of the work lead around the tube.

This assembly will now act as a relay that will switch on when current is flowing through the work lead which only occurs when a cutting arc has been established.

This will require that PlasmaC be operated in Mode 1 rather than Mode 0. See the INI File and PlasmaC Modes sections for more information.