|Export CNC Keyboard Command 'EXPRTCNC'|
Export CNC code files from drawing.
The Export command is used to create G & M Code files from items in the drawing buffer. This is for creating 2D and 2.5D code files.
The EXPRTCNC command found on bottom of sidebar menu and under Files / G-code pull down menu.
The Export G & M Codes dialog form is independent of the main form. It can be moved around and resized.
While this command is in operation, the other commands can also be executed.
Items can be drawn and edited all the while the Export G & M Codes form is operational.
The File text box displays the current file name and path.
Below that and making up the majority of the form is the text box for the script of the G & M Code file being created.
The Exit button will terminate the command.
The Save button will save the contents of the text box for the program script in the file specified by the File text box.
The Export Setup button will bring up a dialog form for controlling the script generated by the command.
The Export All button will create the G & M codes for all the items in the drawing buffer.
The Export Items button will create G & M codes for the currently selected graphic items. The code will be place starting where the character cursor is located in the script text box.
The Altitude text box is for setting the distance above the surface of the material at which rapid travels will be performed by the machine.
The Surface text box is for defining where the surface of the material to be worked with is at.
The Cut Depth text box is for setting how deep below the surface of the material the single pass cut depth will be.
The Incremental check is for making multiple passes at ever increasing depths of cut. If it is checked the Cut Depth text box will be disabled and the Final Cut and Incremental Cut text boxes will become enabled.
The Final Cut text box contents define how deep the final cut depth will be.
The Incremental Cut text box contents define how much deeper each incremental cut will be until the final depth is reached.
The Pecking check determines how the multiple pass cuts will be performed.
If the check is on the code for each individual item will be created with the cut progressively deeper, completing the code for each item before moving on to the next one.
If the check is off the code for all the items will be created with the cut at the incremental depth, then the depth will be increased and code for all the items will be created at the new depth of cut. This is repeated until the final depth of cut is reached
The Export All button presents the dialog form for controlling the type G and M codes will be created for the different tool path events.
The Line Numbers check determines if the G-code file will have line numbers automatically generated when the G and M code is created.
The Verbose Comments check determines if comments are automatically added to the G and M code generated. This is helpful for learning and recognizing events in the file text and associated them to machine movement events.
The Machine Type label displays the current machine type that SuperCamXp is setup for. Clicking on the label will change the Machine Type for which the G and M code will be generated for and also reconfigure the main program. Rotating Spindle, Three Axis Plasma Torch, Torch XY are the three possible machine configurations.
The Spindle On and Spindle Off text boxes contain the code that will be put in the G & M Code file, normally this will be M03 and M05 respectively.
The File Start is normally a percent sign character. What ever is in the text box will be put at the very beginning of the file created.
The File End is normally M30. The contents of the text box is put on the last line of the code file created.
The Select Tool is normally T01. Selecting tool number one(1) normally.
The Lead In is normally G17. Setting up the machine for inches as the units of measurement.
The Rapid Travel is normally G00. This will preceed any change in feedrate when the machine is to rapidly move from one point to another with out considerations given to cutting material while moving.
The Cutting is normally G01. This will preceed any change in feedrate when the machine is cutting material.
The Point Drill is normally G01. This is dependent upon the machine g code interpreter the code is to be used on.
The Arc CW is for Clock Wise arcs and is normally G02. The code is generated with I and J variables.
The Arc CCW is for Counter Clock Wise arces and is normally G03. The code is generated with I and J variables.
The Export Defaults button will set the text boxes to the default settings.
Notes on How to Use It
Drawings can be made and imported while the Export CNC command form is being used.
The current cursor position is important when using the Selected Items mode. The code will be placed in the file where the cursor is positioned.
The pecking only works with the Export Items.
Home Page at http://www.super-tech.com
Published 7/6/2017 4:28:07 PM
Copyright 2016 Dennis Bohlke