Vcarve Processor Question for Spindles

Unsupported
1

I have an XXL, HDZ and 2.2 watt spindle, BitSetter, touch probe and working with VCarve. Until I get comfortable with the bitsetter I still export individual files for each tool and use the bitsetter macros for CNCjs that @neilferreri has provided until I get comfortable with the new multi tool workflow using the bit setter.

The issue I have is that the spindle isn’t getting up to full speed before the cutting starts, there is no “pause for spindle to get up to speed” that I can find. Is there a different post processor I should be using for VCarve?

2

My understanding is you should edit the post-processor to add a “Dwell” command.

2 Likes
3

Just after this line ya think?

±--------------------------------------------------

  • Command output after the header to switch spindle on
    ±--------------------------------------------------

begin SPINDLE_ON

“[S]M3”

1 Like
4

Like this: (just add the “G4 P5.0” at the end for adding a 5 second spindle RPM ramp up time)

+---------------------------------------------------
+  Commands output at the start of the file
+---------------------------------------------------
 
begin HEADER
 
"G17"
"G21"
"G90"
"G0[ZH]"
"M0"
"G0[XH][YH][S]M3"
"G4 P5.0"
4 Likes
5

Probably makes sense to add that to the V-carve post processors. Should be an easy add at the start and after tool changes.

1 Like
6

Good luck on that. …

7

Just tried this and the spindle does pause but isn’t running yet. Is there something I am missing?

8

Can you post the first page of the G-code file you ran that does not start the spindle ?

9

Blockquote
T1
G17
G21
G90
G0Z20.320
G0X0.000Y0.000
G4 P5.0
S20000M3
G0X131.976Y52.371Z5.080
G1Z-1.270F762.0
G1X132.763Y51.962F2032.0
G1X134.213Y51.241
G1X134.160Y51.592
G1X134.139Y52.014
G1X134.158Y52.434
G1X134.217Y52.849
G1X134.316Y53.257
G1X134.453Y53.654
G1X134.639Y54.053
G1X134.412Y54.577
G1X134.308Y54.934
G1X134.116Y54.463
G1X133.908Y54.084
G1X133.667Y53.730
G1X133.394Y53.402
G1X133.092Y53.103
G1X132.762Y52.833
G1X132.408Y52.596
G1X131.976Y52.371

10

Yeah so the G4 P5.0 must not be in the right place in the post-processor file, because it shows up before S20000M3 (which is the command starting the spindle…).

Check your post, and/or send it we’ll check together

1 Like
11

I am assuming I need to move it after the “[S]M3” line?

±--------------------------------------------------

  • Commands output at the start of the file
    ±--------------------------------------------------

begin HEADER

“T1”
“G17”
“G21”
“G90”
“G0[ZH]”
“G0[XH][YH]”
“G4 P5.0”

±--------------------------------------------------

  • Command output after the header to switch spindle on
    ±--------------------------------------------------

begin SPINDLE_ON

“[S]M3”

±--------------------------------------------------

  • Commands output for rapid moves
    ±--------------------------------------------------

begin RAPID_MOVE

“G0[X][Y][Z]”

12

Ha, it’s a little bit different from mine. Yes, move the “G4 P5.0” line right after [S]M3 and you’re good to go.

13

Awesome. Thanks again.

1 Like
14

This topic was automatically closed after 30 days. New replies are no longer allowed.