Cut charts: where the speeds and heights come from
Speed, heights, pierce delay and kerf come from a mix of chart data and job settings. This guide shows how a job picks its chart row, what the Machine ticks do, how to edit the table, and two things about the lookup worth knowing before you trust a number.
Under Machine Settings, set Machine Model, Process, Plasma Unit (Refresh Units reloads the list), Plasma Torch and Units, and tick Flatbed Work; a nest needs it. A job uses its own selected plasma unit when it has one, otherwise the nest machine's unit. The job's plate supplies the material and thickness; a metric thickness is converted to inches to look up the chart.
In the nest, Plasma Settings shows Consumable, Quality, Offset (half the kerf width), Cut Speed, Cut Height and Clearance. Cut Speed and Cut Height each have their own Machine tick: ticked, the chart value for the selected process, material and thickness is used; unticked, the number you typed is used. When you reapply the chart defaults, half of a positive chart kerf goes into Offset, and speed and height refresh only from positive chart values and only where the matching Machine tick is on. Unticked manual values are left alone, and a zero in the chart doesn't necessarily overwrite what was on screen. Pierce height and pierce delay always come from the chart; clearance always comes from the job.
The lookup doesn't need an exact thickness. It takes the row whose thickness is closest to the job's, using a matching quality only to break a tie, and it doesn't interpolate between rows. So a lookup that succeeds doesn't prove the manufacturer published values for that exact thickness. Check that the nearest row is the one you meant, especially when your thickness sits between two listed ones.
Where a thickness has more than one quality row, the pane refreshes using the Quality you picked, but the program composer doesn't currently pass that preference along. So the row you see isn't guaranteed to be the one that gets posted. A zero or negative chart value can leave an earlier value showing, and a manual override can differ from the chart. Check the speed and heights in the generated program rather than assuming they match the pane.
Settings, then Plasma Table Settings, opens the Plasma Cutting Table Editor. Pick the Power Unit, Material and Process. Thickness is read-only; you can edit Cut Speed (IPM), Pierce Height, Pierce Delay, Cut Height, Voltage, Current, Kerf, Quality, Plasma Pressure, Shield Pressure, Rapid Height and R-Plane, and Modified marks changed rows. The table is in inches and inches per minute regardless of the nest's units, and there's no way to add a thickness row here. Save Changes writes the edits to that plasma unit's shared table; closing with unsaved edits asks first.
Reset to Defaults asks for confirmation and then restores the whole table for the selected plasma unit to the shipped values, every material, process and row, not just what is on screen. It isn't an undo. Tables are shared reference data stored per computer under ProgramData in the GCmaker PlasmaTech folder, separate from the shop settings folder, so back them up before an intentional reset. Table edits change what later lookups find; they don't rewrite a program you've already generated. If you only need a different number for one job, untick Machine and type the speed or height instead.
Questions people ask
The table stores those columns, but whether any value reaches the machine depends on the post and the controller. Many controllers own height control and process setup themselves. Check the post's notes and your commissioning record; don't assume a column reaches the machine.