Hello all. Need help with adding a delay to allow vfd spindle to come up to speed before starting job. Have searched the forums, still can’t figure it out. Appreciate any help. BTW I’m using OB PP for Vectric v carve pro Thanks
Checkout Post Processor Editing We have a 1.8 second spinup delay (which is enough for most spindles we use) so you can edit that line and just change the 1.8 to a longer period for your own modified post
Peter, Thanks for your reply. I'm not very savvy at Gcode or any programing for that matter! The article you refered me to kinda blew my mind. however I did find 1.8 sec delay you spoke of and changed it in OB PP to 5 sec. when I run the file using the updated PP it delays the start of job with spindle off then proceeds to run job as spindle ramps up. appreciate your help getting this sorted.
Make sure the G4 delay command is After the M3 Spindle On command Code: begin SPINDLE_ON "M3[S]" "G4 P1.8" attach your edited post, and a gcode file created with the edited post if you want me to check it out
+--------------------------------------------------- + Command output after the header to switch spindle on +--------------------------------------------------- begin SPINDLE_ON "M3" "G4 P5" this was copied from PP that i changed . no change noticed when running job. it appears that I've done it correctly,
Right, so from your gcode: Line 7 is a 1 second pause Line 8 turns on the spindle Line 9 is a 10 second pause Then the XY moves start Looking at the Post processor: Line 103 is the 1 second pause Line 112 is the spindle on Line 113 is the 10 second pause Loaded file up on my machine (equiped with a router, I don't own a VFD) Moved Z to about 0.2 inches above the stock Moved XY to the first plunge point Waited 1 second Router turned on, it waited in place for the full 10 seconds Started plunging down and running the XY moves Moved in XY to above the plunge So all the gcode related actions are working as intended.
thanks for the help. I'm still having the same issue in spite of the gcode being correct! the controller ignores the G4 p10 line I must be missing something somewhere in the setup. unable to run if spindle comes up to speed after cut starts. if you think of something I'm doing wrong, let me know please. thanks again
1) Try G04 instead of G4 just in case? 2) Make sure you are loading the correct file (not an old one with the same name maybe) What controller are you using?
Same here in the tests (also using BlackBox) - Grbl doesn't mind G4 vs G04 So double check the Gcode editor tab after loading your file that you do have a pause after the M3 And then maybe something in your VFD parameters causing some extra delay? (like it gets the signal, then waits 10 seconds to start, gcode also waits 10 seconds, but now its all happening at once? Or its just ramping up much slower than 10 seconds? Look at delay/ramp keywords in VFD manual) You can test this from the Tool On menu in CONTROL - see if it responds in a timely fashion
Peter Was this ever resolved? I seem to be having the same problem. I am using the open-builds black box with a VFD. This is what my code looks like in Gcoder editor: T1 G17 G20 G90 G0Z0.8000 G0X0.0000Y0.0000 M3S18000 G4 P8.5 G0X1.1275Y0.7500Z0.2000 G1Z-0.0750F30.0 G1Y4.7500F60.0 G1X1.1276Y4.7594 The problem is that even with the G4 command after M3, When I hit Run Job in Control, the spindle pauses for 8.5 sec and then turns on. This doesnt give the spindle enough to time to spin up and causes it to "drag" the wood. I have also tried G04 but that has no effect. Any suggestions?
How did you get the P8.5? That is where your 8.5 second delay is. This is what Vectric spits out for me when I use the Grbl mm post processor: T1 G17 G21 G90 G0Z59.000 G0X0.000Y0.000 M3S18000 G4 P1.8 With the OpenBuilds inches Post Processor I get the same 1.8 seconds: T1 G17 G20 G90 G0Z2.3228 G0X0.0000Y0.0000 M3S16000 G4 P1.8
1.8 is for our recommended routers. VFDs are 3rd party items, if you go beyond standard setups, you may also just need to copy and edit the Post to suit your now different spin up times
So I'm changing to a spindle and reading up on PP editing. I feel confident this is well within my abilities but I feel like I'm missing something fundamental and basic. I'm editing the OB Vectric PP to include turning on the cooling relay (M8, I believe) as well as adding a 7 second delay (G4 P7) to allow for spindle spool up. What I don't understand is this......why is there no footer in the OP PP? I open it n the text editor and see no footer at all. Wouldn't instructions on how to end be found there? How does OP Control know to shut down the spindle/router without this information? It was turning off my router automatically before so clearly it's not an issue but I also want to add the command to shut off cooling at the end of the run. So, why no footer? What am I missing here? Thanks!
The OB post defines any overrides of the default post. You'll see in the OB post that there is a POST_BASE defined. That POST_BASE has the footer. So, if you want to change the footer, add it to the OB Post.
I knew I was missing something! In looking over a bunch of documents at midnight with a little vodka in me I must have missed this. So........just so I can get this straight in my own brain, there is a default post processor which contains a footer (presumably with ending instructions). The Openbuilds post processor has no footer therefore it defers to the footer in the default post processor which becomes part of the gcode. If I add a footer to the Openbuilds post processor, it will override the footer in the default post processor. I assume I should be able to find this default post processor in the PP folder where Vectric stores them (just to take a peek)? And to clarify further. The addition of a footer to the Openbuilds post processor doesn't add to the default footer, it replaces/overrides it? Do I have this right? I realllllllly appreciate your help. This kept me up last night, despite the vodka.
