|
. |
VS3D Machine Mode
1.7.3 Cutting Path continued.
"Make Cuts / Add To Protocol..." : Once the Cutting Protocol has been initialized, the cutting tool bit has been defined or loaded, and the tool path parameters have been entered, click on this button to start a tool path. If VS3D is running in licensed mode, the "Tool Path File Parameters" dialog will appear. This dialog has settings for controlling the output machine file. The available controls will vary depending upon the chosen Protocol "Machine Type".
- "File Intro" : Two lines of text that will be inserted at the beginning of the file (for example, "%" and "01"). Leave blank to omit this in the output G-Code file.
- "Line Suffix" : One or more characters that will be inserted at the end of every line in the file. For example, enter in this field " *" (a space followed by an asterisk without quotes) to have a space and an asterisk appended to every line in the file. Leave blank to omit this in the output G-Code file.
- "Spindle RPM" : The RPM for cutting. Some machines will override this with a manual setting on the spindle itself.
- "Pause For Spindle Speed-Up" : If the machine supports the G-Code "M31" spindle speed-up pause command, set this to "M31", other wise set it to "None".
- "Inches/mm (English/Metric) G-Code" : Choose the G-Code command that the machine accepts for inches or mm operation (G20/G70 or G21/G71).
- "Coordinate Accuracy Decimal Places" : For G-Code, use this to set the number of decimal places of accuracy for coordinates in the output file. For example, if this is set to "3", then three digits will appear to the right of the decimal point (like "0.123"). The "Auto" setting will compute the setting automatically based upon the resolution of the scuplture grid.
- "Feed Rate (XY)" : This is the XY cutting speed. Normally this is inches per minute, but for different machines, this value may have different units. This value should be chosen carefully, based upon the RPM, the tool bit size and type, and the material being cut.
- "Plunge Rate (Z)" : This is the Z cutting speed. It is similar to the "Feed Rate (XY)", but specifies the speed at which to dive into the material. It is normally less than or equal to the "Feed Rate (XY)". If the Feed Rate is equal to the Plunge Rate, then for some file types (such as G-Code) the output file is more compact.
- "Jog Rate (XY)" : This is the XY fast (in air) movement speed. Normally this is inches per minute, but for different machines, this value may have different units.
- "Jog Rate (Z)" : This is the Z fast (in air) movement speed. Similar to "Jog Rate (XY)", but for the Z (vertical) direction.
Continued ...
|
