Usage |
python dmap2gcode-XXX.py [-g file ] or dmap2gcode-XXX.exe [-g file ] |
-g (or --gcode_file) |
dmap2gcode g-code output file to read. Reading the settings from previously saved g-code files only works if the "Suppress Comments" option was not selected in the "General settings" when the g-code file was saved. The default is to suppress the comments because a lot of people are using GRBL these days and GRBL does not handle comments well. |
-h (or --help) |
print syntax help to console window. |
Example (Using python script with preinstalled python distribution) |
python dmap2gcode-XXX.py -g my_file.ngc |
Example (Using precompiled Windows executable) |
dmap2gcode-XXX.exe -g my_file.ngc |
F1 | Open the Help dialog box. (There is nothing in the help except a reference back to the web page and my e-mail address) |
F2 | Opens General Settings Window |
F3 | Opens Roughing Settings Window |
F5 | Refresh display |
dmap2gcode.ngc or .dmap2gcoderc |
When Dmap2gcode starts up the the directory in which Dmap2gcode starts in is searched for a file named "dmap2gcode.ngc". If the file is found it is read and all of the Dmap2gcode options are set according to the settings saved in the config file. After searching for the config file in the current directory the users home directory is searched for "dmap2gcode.ngc" or ".dmap2gcoderc" if either of these are found it will be used as the default settings. Only the first config file found is read. To create a config file with your preferred options for startup just open Dmap2gcode and change the settings to your liking and save a file called "dmap2gcode.ngc" in the users home directory or the directory Dmap2gcode is called from. (If you are not using the precompiled windows executable you could also just edit the settings in the .py file) |
Input Field | Description |
Image Height | The size of the G-Code output for the image in the Y direction (displayed as vertical on the screen) If cutting the full image the tool will move exactly the Image height in the Y direction. This means that if you are cutting with a flat cutter the actual cut size will be the Image height plus the diameter of the cutting tool. |
Image Width | This dimension is automatically calculated and displayed to indicate the width or X axis size of the image G-Code output. This dimension is a function of the image aspect ratio and the "Image Height". |
Pixel Size | This dimension is automatically calculated and displayed to indicate the resulting size of a single pixel based on the selected image and the "Image height" input. |
Depth Color | The depth color setting determines whether the depth of cut is determined by the darkness (black) or lightness (white) of the image. If "black" is selected the portions of the image that are black will be the deepest cuts and white portions of the image will be at Z equals zero. Conversely if "white" is selected the white areas of the image will be cut the deepest. |
Normalize Depth | Selecting this option tells the program to treat the darkest pixel as if it were black and the lightest pixel as if it were white. The remaining levels of grey between are stretched fill the range. |
Origin | The origin determines the relative location of the g-code x and y zero location. The current location of the origin is displayed in the display window as a red and green lines. The red and green lines follow the RGB convention Red is the x-axis, Green in the y-axis. |
Cut Top Surface | If "Cut Top Surface" is selected the whole image is cut even if the cut depth is zero. If this option is not selected the top surface is not cut. The tool path will move to Z-safe and rapid past the areas not cut. |
Top Tolerance | The "Top Tolerance" determines how far a calculated cut has to be below the zero position before it is not considered a top surface cut. |
Tool DIA | Specify the tool diameter. |
Tool End | Specifies the tool shape (Ball End, Flat End, or V-Bit) |
V Bit Angle | If the V-bit tool end option is selected this option determines the included angle of the V-bit. |
Scan Pattern | This option determines if g-code is generated for the "Rows" (X direction), "Columns" (Y direction) or both "R then C" (Rows then Columns) or "C then R" (Columns then Rows). |
Cut Perimeter | This option adds a perimeter cut to the g-code output when only "Rows" or only "Columns" is selected for the "Scan pattern". This can eliminate a scalloped look at the edge of an image. |
Scan Direction |
"Scan Direction" determines the cutting direction methodology.
|
Feed Rate | Specify the tool feed rate that is output in the g-code output file. |
Plunge Feed | Specify the tool feed rate that is output in the g-code output file when moving vertically into the material. |
Stepover | The distance between adjacent rows or columns. |
Z Safe | This is the z location that the tool will be directed to prior to any rapid movement. |
Max Cut Depth | The depth of the deepest possible cut into the material. |
Input Field | Description |
Units (inch/mm) | Set the units used by Dmap2gcode to inches or mm. This option affects the displayed units and the units output in the g-code. |
Tolerance | When a series of points are within tolerance of being a straight line, they are output as a straight line. Increasing tolerance can lead to better contouring performance in LinuxCNC, but can also remove or blur small details in the image. |
G Code Header |
The text that is entered in the G-Code header entry box is added to the beginning of the g-code commands in the Dmap2gcode output file. The commands are interpreted by the CNC machine as entered. The default values (G17 G90 G64 M3 S3000 M7) are explained below: G17 G90 G64 M3 S3000 M7 |
G Code Postscript |
The text that is entered in the G-Code Postscript entry box is added to the end of the g-code commands in the Dmap2gcode output file. The commands are interpreted by the CNC machine as entered . The default values (M5 M9 M2) are explained below: M5 M9 M2 |
Lace Bounding |
"Lace Bounding" controls whether areas that are relatively flat along a row or column are skipped. This option only makes sense when both rows and columns are being milled. Possible bounding options are:
|
LB Contact angle | When Lace bounding is not None, slopes greater than Contact angle are considered to be "strong" slopes, and slopes less than that angle are considered to be weak slopes. |
Offset Stepover | This option allows offsetting the stepover by 1/2 or 1/4 step. If you cut an image and find that the scan lines were not close enough together switch this option to 1/2 and generate a new g-code file. The new file will have the same stepover, however, the steps will be offset by 1/2 step so that the scan lines will be between the previous scan lines. Repeating the process with 1/4 step will automatically half the step size and cut between all of the previously cut scan lines |
Plunge Type | Specifies whether a straight vertical plunge or an arced plunge is to be used for entry into the cut. (NOTE: The arc entry may cause more material to be removed at the entry point. Creating a scallop outside of the image (height + tool diameter) or (width + tool diameter) boundary) |
Input Field | Description |
Roughing Tool DIA | Analogous to the "Tool DIA" specifically for the roughing operation. |
Roughing Tool End | Analogous to the "Tool DIA" specifically for the roughing operation. |
Roughing V Bit Angle | Analogous to the "V Bit Angle" specifically for the roughing operation. |
Roughing Scan Pattern | Analogous to the "Scan Pattern" specifically for the roughing operation. |
Roughing Scan Direction | Analogous to the "Scan Direction" specifically for the roughing operation. |
Roughing Feed Rate | Analogous to the "Feed Rate" specifically for the roughing operation. |
Roughing Plunge Feed | Analogous to the "Plunge Feed" specifically for the roughing operation. |
Roughing Stepover | Analogous to the "Stepover" specifically for the roughing operation. |
Roughing Offset | The "Roughing Offset" is the thickness of material to be left behind after the roughing operation is complete. |
Roughing Depth/Pass | The maximum depth of cut four each roughing pass. |