SheetCam Software Setup & Users Guide¶

This guide provides step-by-step instructions for installing SheetCam and setting up the Avid CNC Mach4 post processor and tool tables for a variety of Hypertherm torches. If you have already installed and licensed SheetCam, skip to Section 3.

The Pro-Tip video below also shows the SheetCam installation process.

1. Install SheetCam¶

• Navigate to https://www.sheetcam.com/downloads

• It is recommended to download "SheetCam TNG Stable version".

• Navigate to your downloads folder (or the directory you downloaded the installer to) and run the SheetCam TNG installer.

• Click "Yes" to begin the installation.

• When the installer asks for an install location, it is highly recommended to use the default location.

• When you get to the prompt shown above, select the "Create a desktop shortcut" option.

• Select the "Run SheetCam TNG" option and finish the SheetCam install.
• Continue with the setup and license procedure in the next section.

2. Install License File¶

• Select your default language.

• Use the "SheetCam TNG setup wizard" to setup SheetCam for plasma cutting.

• Select your preferred units.

• Select "Jet cutting" machine type for plasma machines.

• Choose your selections for "Output file units", "Z zero", and "Output folder". The post processor selection will be set in Section 3Section 3.

• After completing the setup wizard, navigate to "Help > Install license file".

• Select your license file and click "Open".
• Close SheetCam before continuing with the next section.

3. Install Post Processor and Tool Tables¶

In this section you will download and install the Avid CNC Mach4 post processor for SheetCam and tool tables for Hypertherm torches. Begin by downloading the installerdownloading the installer for these items. ({ { config.build.domain.support } }/instructions/software/downloads/sheetcam)

• Run the installer you just downloaded. The name may vary depending on your download selection.

• Click "Install" to begin the installation.

• Part way through the install, you'll be asked about making changes to your device. Click "Yes" to allow the plasma tools files to be installed correctly.
• Once installation has finished, continue to the next section.

4. Post Processor Setup¶

In this section you will configure your post processor setting for your machine. This is a critical step to ensuring programs created in SheetCam work correctly.

Post Processor Selection¶

• Open SheetCam.
• Navigate to "Options > Machine".

• On the "Post Processor" tab, verify "Avid CNC Mach4" is the current post processor.
• At the bottom of the screen, select "Set custom post options".

Post Processor Settings¶

1. Distance between references

   Sets a radius around the most recent probe where subsequent pierces will start without a probe. This value can be increased to reduce program run time on flat, stable (usually thick) material that will not have a significant height difference between pierce locations.

2. Reference feed rate

   Sets the feedrate during the probe portion of a move. Increasing this from the default will reduce run time but also reduce the accuracy of the Z positioning.

3. Slow Probe Height

   Sets a height above the last material Z position that the torch will rapid down to before starting the slow probe move.

   

   The first probe in a program will always be full height at slow speed to initially find the material. Using the Slow Probe Height greatly reduces the run time of programs with many pierces.

4. Touchoff type

   This dialog sets the touchoff type - Ohmic or Mechanical. For general operation, Ohmic touchoff is strongly recommended.

   Note

   Using Mechanical touchoff requires opening the Ohmic Protection Box and changing a jumper position.

   For more information please refer to the Plasma Getting Started Guide.

5. End Program Z Height

   Sets a machine coordinate location to park the Z after a program. This is used to drive the Z up and reduce water splashing at the end of a cut.

   

5. Choosing a Toolset¶

• To load a tool set, navigate to "File > Open toolset".

• Open the folder for your specific Hypertherm plasma system.

• Open the folder for your specific Hypertherm plasma system.

• Open the folder for the type of consumables you are using with the Duramax torch.

  • Duramax consumables - a consumable stack of retaining cap, shield, nozzle, electrode, and swirl ring.
  • SYNC consumables with cartridge adapter - a single piece cartridge with adapter.

• Select the appropriate toolset for your desired units (English or Metric) and the type of mechanized consumables you are using.

  • Shielded - these are standard mechanized consumables.
  • FineCut - these are specific consumable sets designed for improved fine feature cutting.

• After selecting your tool set, the "Tools" pane will show a list of possible tools.
• Double click on one of the tools.

• You will see the tool is pre-populated with the values from the Hypertherm cut charts and Avid CNC calculations.
• Using the AvidCNC Mach4 post processor, these values will be included in your GCode and automatically populated in Mach4 when the program is executed.

6. SheetCam Drawing Import Settings¶

There are settings in Options -> Application Options -> Drawing Import that SheetCam uses to smooth and simplify vectors when drawings are imported. More detail on the settings is available in Help -> Help Window -> Menu Items -> Options Menu.

The Avid CNC Post and Tools installer changes some of the settings from default to better match the capabilities and needs of plasma cutting. Plasma is a relatively rough cutting method that cannot achieve very fine tolerances. Smoothing the imported vectors will result in smaller file size (1/3 - 1/2 reduction in gcode lines) and smoother motion. Smoothing will result in geometry differences that are smaller than the normal variation in kerf width throughout a cut. The final products of these two files will be indistinguishable.

Below is an example of SheetCam defaults (left) and Avid CNC defaults (right).

7. Operation Setup¶

When a new Jet Cutting operation is created, the Path Rules should be set to Default and the Code Snippet should be set to "M62P4 (+++THC Allowed, AD2+++)".

The Code Snippet is necessary to ensure that THC is allowed in the operation. The Path Rules will then allow/inhibit THC for certain features.

Note that if you don't want THC active at all during a specific operation within a gcode program, it is important to also disable the Cut/Path rules for that operation to avoid M62P4 being added automatically on a feature.

8. Using Cut Rules¶

Path or Cut Rules in SheetCam serve as instructions for the post processor to modify the G-Code output for specific toolpath features. The most common uses of Path Rules are preventing dives by inhibiting THC or improving cut quality by locally reducing the feedrate.

• To open the cutting rules editor press the Cut Rules button on the left of the Tools menu on the left of the SheetCam application window, or use the drop down menu Tools -> Cutting Rules.

• The Path Rules window will then be displayed. The default rule set will have been installed by the "AvidCNC for SheetCam" installer.

• To disable or enable path rules click the checkbox to the left of the path rule name.

• To edit a path rule double click on the name of the rule, this will open the rule options. The rule parameters may be edited and saved by clicking "OK." "Start code" and "End code" are the M codes which will be inserted into the g-code program at the beginning and end of the path rule's effect.

• Additional types of path rules may be implemented by clicking the "Add rule" button at the bottom of the Path Rules editor window.

Descriptions of the Avid CNC default path rules are below

• Enabled by default.

• Function: disables THC for holes with a diameter under the "Smaller than" value. Reduces the feed rate to the set percentage.

• For most materials the height change across a small circle is too small to really need THC motion, but the tip voltage is unstable during the cut.

• It is useful to prevent unwanted torch dives caused by unstable tip voltage during short cuts.

• Reducing the feedrate for small circles can help reduce the bevel of the cut.

• Enabled by default.

• Function: disables THC for closed profiles with an equivalent diameter under the "Smaller than" value. Reduces the feed rate to the set percentage.

• Equivalent Diameter is defined as the diameter of a circle with a circumference equal to the shape's perimeter.

• For most materials the height change across a small shape is too small to really need THC motion, but the tip voltage is unstable during the cut.

• It is useful to prevent unwanted torch dives caused by unstable tip voltage during short cuts.

• Reducing the feedrate for small shapes can help reduce the bevel of the cut.

• Disabled by default.

• Function: disables THC for a set distance before and after tight corners. Reduces the feed rate to the set percentage.

• When a cut makes a tight corner it requires the machine to slow down. This causes the plasma arc to grow and the measured tip voltage to increase.

• This rule can prevent unwanted torch dives caused by artificially high tip voltage in tight corners.

• In most cases, this rule is not needed and can hinder THC's ability to track the material properly.

• Disabled by default.

• Function: disables THC during lead-ins.

• During lead-ins the tip voltage is typically unstable and above the target.

• This rule can prevent unwanted torch dives caused by artificially high tip voltage.

• In most cases this rule is not needed due to redundancy with other THC Anti Dive settings.

• Enabled by default.

• Function: disables THC during lead-outs.

• During leadouts the tip voltage is typically unstable and above the target.

• This rule can prevent unwanted torch dives caused by artificially high tip voltage.

• While M codes will not show up in the tool preview, any path rules which change the feedrate percentage will highlight the effected operations in blue instead of the normal green.