My PP is adding extra commands

[rink]

Good eveing.

Today, I output a toolpath, went to the CNC, hit “go”, and the machine just sat there…for a few seconds…then moved.

Turns out, the CNCPiranha-Arcs (mm) PP is outputting some extra commands into the G-code. It doesn’t happen when using the CNCPiranha-Arcs (inch) PP. Only when using the metric one. I’m attempting to attach a screen shot showing both gcode files side-by-side, with the extra commands highlighted. I wasn't able to attach the toolpath files.

The metric version of the PP is inserting commands to set the router speed, turn on the spindle, and then dwell for a while. Those are not needed. Is this by design or is it a bug?

Thx, rink.

[jfederer]

My nc PPs do the same thing, the metric one goes to "home", pauses, then goes to 0,0. The Inch one skips the first 2 steps and just goes to 0.0. I haven't looked that the PP templates, but I assume whoever programmed them added the extra steps. We can edit them, I just haven't bothered.

[gkas]

The metric version of the PP is inserting commands to set the router speed, turn on the spindle, and then dwell for a while. Those are not needed. Is this by design or is it a bug?

Vectric does not write the PP. So, you either get official changes from the hardware folks, or make the changes yourself.

[TReischl]

Is this by design or is it a bug?

Thx, rink.

Not a bug. It is the way someone over at the machine place thought the post should run. Have you ever took a look at the post processor files?

[rink]

Thanks for the thoughts guys. Actually I did look at the PP today. Both the one for inch and the one for metric. I couldn’t figure out what line in the PP was causing that. I’ll take another look.

How can I learn more about the code that makes up the PP? Would I have to contact the hardware manufacturer? Or is that language standard?

Thx, rink.

[rink]

Update: I read the Vectric help doc on editing post processors. Pretty straightforward. Below is the entire text of the CNCPiranha-Arcs (mm) post processor. Couple thoughts:
1. This PP appears to be incomplete. There is no block section for rapid moves, plunge moves, footer, etc.as there is in the Piranha "inch" PP. If someone can confirm that...where would I get a complete one? Or could I just copy/paste the missing sections from the Piranha "inch" PP?
2. I don't see anywhere in this metric PP where it generates a DWELL (G04) command. So any idea why there would be one (a G04 P5) in my resulting g-code? It happened when saving out just the "selected toolpath", as well as when saving out "visible toolpaths to multiple files".

I'm using VCarve Desktop 10.513.

Thx, rink.

+================================================
+
+ G Code - Vectric machine output configuration file
+
+================================================
+
+ History
+
+ Who When What
+ ======== ========== ===========================
+ Tim 08/09/2015 Written
+ Mark 11/5/2016 Renamed to be standard pp for V8.5
+ MohamedM 08/07/2020 Inherit Next_Wave_CNC_mm
+================================================

POST_NAME = "CNCPiranha-Arcs (mm) (*.tap)"

POST_BASE = "Next_Wave_CNC.pp"

UNITS = "MM"

LASER_SUPPORT = "NO"


+================================================
+
+ Formating for variables
+
+================================================

VAR LINE_NUMBER = [N|A|N|1.0]
VAR POWER = [P|A| S|1.0|10]
VAR SPINDLE_SPEED = [S|A|S|1.0]
VAR CUT_RATE = [FC|A|F|1.1]
VAR PLUNGE_RATE = [FP|A|F|1.1]
VAR X_POSITION = [X|A| X|1.3]
VAR Y_POSITION = [Y|A| Y|1.3]
VAR Z_POSITION = [Z|A| Z|1.3]
VAR ARC_CENTRE_I_INC_POSITION = [I|A| I|1.3]
VAR ARC_CENTRE_J_INC_POSITION = [J|A| J|1.3]
VAR X_HOME_POSITION = [XH|A| X|1.3]
VAR Y_HOME_POSITION = [YH|A| Y|1.3]
VAR Z_HOME_POSITION = [ZH|A| Z|1.3]
VAR DWELL_TIME = [DWELL|A|P|1.2]
+================================================
+
+ Block definitions for toolpath output
+
+================================================

+---------------------------------------------------
+ Commands output at the start of the file
+---------------------------------------------------

begin HEADER

"( [TP_FILENAME] )"
"( File created: [DATE] - [TIME])"
"( for Next Wave Automation from Vectric )"
"( Material Size)"
"( X= [XLENGTH], Y= [YLENGTH], Z= [ZLENGTH])"
"( Z Origin for Material = [Z_ORIGIN])"
"( XY Origin for Material = [XY_ORIGIN])"
"( XY Origin Position = X:[X_ORIGIN_POS], Y:[Y_ORIGIN_POS])"
"( Home Position)"
"( X = [XH] Y = [YH] Z = [ZH])"
"( Safe Z = [SAFEZ])"
"([FILE_NOTES])"
"(Toolpaths used in this file:)"
"([TOOLPATHS_OUTPUT])"
"(Tool used in this file: )"
"([TOOLS_USED])"
"([TOOLNAME])"
"(|---------------------------------------)"
"(| Toolpath:- '[TOOLPATH_NAME]' )"
"(|---------------------------------------)"
"G90"
"G21"
"[FC]"

[scotttarnor]

Support@nextwavecnc.com they write the PP

[Adrian]

1. This PP appears to be incomplete.

It appears incomplete because you're not looking at the whole thing. It's a post processor that inherits another. The POST_BASE command says that it using everything in the Next_Wave_CNC file and then anything in this file are additions/replacements to that file.

[GEdward]

The problem may not be in the PP. If you are running Mach3 the problem might be in the Ports and Pins Configuration menu. In Ports and Pins there is a tab for spindle set up. Within the drop down menu is a section to set up dwell for spindle spin up time and spindle spin down time. This parameter allows time for the spindle to achieve full commanded rpm before the machine attempts to engage the tool.

Ed

[GEdward]

Ooops! The OP clearly shows the dwell command in the g code. By contrast, the inch g code generated with the CNC Piranha inch PP doesn't even show a spindle start command as far as I can see. In my PP menu there is a CNC Piranha mm processor which might be different from the Next Wave Automation processor that was used.

Ed

[Adrian]

As I said in my post you have to look at the CNCPiranha-Arcs and Next_Wave_CNC files together and treat them as one with the CNCPiranha-Arcs commands taking precedent where there is duplication.

The POST_BASE command is used to merge another post processor into this one. That's why there is no dwell command in the CNCPiranha-Arcs file, it's in the Next_Wave_CNC file but as far as VCarve is concerned it is in the CNCPiranha-Arcs post processor when it comes to saving the toolpath file.

[rink]

Good morning.
Sure enough, Adrian nailed it. There is another PP “Next_Wave_CNC.pp”. It does, indeed, include a dwell command. Here is the relevant section:
+---------------------------------------------------
+ Command output after the header to switch spindle on
+---------------------------------------------------

begin SPINDLE_ON

"G0 [ZH]"
"[S]"
"M3"
"G04 P5"

What an education for me! Now I think I can fix this situation by either:
1. Simply commenting out the dwell command from the existing POST_BASE PP.
2. Make a new, complete metric PP that has all the necessary commands and doesn’t need to inherit anything from another one.
3. Make a new abbreviated metric PP that only has one command which sets units to metric, then inherits everything else from the inch PP.
Would those approaches work?

Thx, rink.