Rando wrote: ↑Wed Jul 06, 2022 5:54 pm
anderjus:
============================
Importing GCode tap files:
Vectric, and most other CAD/CAM programs have ZERO capability to **import** GCode tap files, so that's gonna be a dead-end. That is, you can only use the Vectric tape-splitting feature on toolpaths actually generated in Vectric.
============================
Making the head move to a position, stop, and only then descend to resume cutting:
When you make the head move to a specific XY location (G00 or G01) and you need it go there, STOP, and then descend in Z, put a G04 P250 pause block in between. That way, the machine will go to the XY location, wait a 1/4 second, and then descend. The closer you can get the XY to the right location, the better, of course. The code would look something like the below, if you needed it to start cutting at, for example, X1.050 Y5.653, and then start cutting at Z-0.020:
G01 X1.050 Y5.653 F100.00
G04 P250
G01 Z-0.020 F20.0
The F100 should be your choice of linear feedrate, and the F20.0 should be whatever you use for the vertical plunge rate. Note that if you use ramping, the plunge rate won't actually be purely vertical, but rather will be the rate along the ramp trajectory. So if you use a ramp and your linear rate is 100 with the plunge rate at 65, you might want a true-vertical rate of only 20 or so.
Adding the G04 with a millisecond delay value (e.g., P250) should keep it from interpolating the movement, and head straight down.
============================
Figuring out what's a preamble and what's movement:
To make it all work right, take a look at the following chunk of GCode, written using the "CNCShark-USB 3D Contour (inch)(*.tap)" post processor. The "preamble" starts with a line of +'s and ends with the line of -'s. Everything after the first movement command is typically understood as being that preamble. That is, the first G00 or G01, typically something like "G00 Z0.5" to get the head up to the safe-height. So, when you're cutting out hunks of GCode, leave all of the preamble in, and only cut out lines in the movement section. Be careful if there are actually multiple toolpaths in there, since you only need the **most recent** preamble for things to work.
(+++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++++)
( Shark30DegEngravingSingle )
( File created: Wednesday July 06 2022 - 04:41 PM)
( for CNC Shark from Vectric )
( Material Size)
( X= 4.375, Y= 3.000, Z= 0.750)
( Z Origin for Material = Material Surface)
( XY Origin for Material = Top Left Corner)
( XY Origin Position = X:0.000, Y:0.000)
( Home Position)
( X = X0.0000 Y = Y0.0000 Z = Z0.5000)
( Safe Z = 0.200)
()
(Toolpaths used in this file:)
(30DegEngravingSingle)
(Tool used in this file: )
(Engraving - 30 Deg Incl. Angle Tip 0.005 - 0.353 inches)
(|---------------------------------------)
(| Toolpath:- '30DegEngravingSingle' )
(|---------------------------------------)
G90
G20
F6000.0
G64 P0.050
M6 T1
S20000
M3
G0 Z0.5000
(---------------------------------------------------------------------------------------------------------------------------)
F6000.0
G00 X0.1977 Y-0.9763 Z0.2000
F6000.0
G00 X0.1977 Y-0.9763 Z0.1500
F1200.0
G1 X0.1977 Y-0.9763 Z-0.0300
F6000.0
G01 X0.1979 Y-0.9762 Z-0.0300
G01 X0.2044 Y-0.9779 Z-0.0300
G01 X0.2901 Y-0.9786 Z-0.0300
G01 X0.5180 Y-0.9791 Z-0.0300
F6000.0
So, let's say you want to cut out everything and resume at the second-to-the-last G01 command, "G01 X0.2901 Y-0.9786 Z-0.0300". Your modified code then, would include the preamble including the G00 Z0.5000, and then look something like this:
F6000.0
G01 X0.2901 Y-0.9786
G04 P250
F500.0
G01 Z-0.0300
F6000.0
.... and then the rest of the GCode.
That way, it will go to the XY coordinates, pause for 1/4 second once it's all the way there, and only THEN will it go down to start curving in the material.
Make sense?
Hope that helps.
Rando