Returning to zero after each toolpath

[gstanczak]

Hello, it seems my gcode from VCarve recently started including a return to home command between every toolpath. Has this always been the case and I never noticed? I don't think so, it's quite a lot of unnecessary movement? Is there a setting that I inadvertently changed? It's not the sending program. There in fact is a G28 command in the output file after each toolpath.

Thanks,
Greg

[SteveNelson46]

Are you sure you are using the correct post processor? From your description it sounds like you are using a PP with a tool changer.

[adze_cnc]

Three questions and two of them only you can answer:

1. I don't know, have you never noticed it before?
2. Yes, it is much wasted movement.
3. I don't know, is there a setting that you've inadvertently changed? (Have you updated VCarve? Have you changed the post-proceessor that you use?)

The G28 code does return to the machine home. Was there a setting in your control software that used to ignore this but now doesn't? (i.e. Have you updated your control software to a new version?)

[mezalick]

Greg,
What are the setting for the XY Home / Start Position in your material setup?

Michael

[Adrian]

Which post processor are you selecting? There is no G28 command in the XCarve/GRBL one.

[gstanczak]

Attached are my post processor (X-Carve_inch.pp) and a screengrab of the simulation in VCarve that indicates all the returns to home, leading me to believe it's not the post processor or controller. One thing to note are that the toolpaths are tiled, but the same thing happens if I remove the tiling.

Adrian- My mistake. Not G28 command, but G0 command followed by home coordinates.

Michael- Home coordinates are set to X=0, Y=0, Z=0.2, similar to your screengrab.

Adze-CNC- I'm using OpenBuilds Controller and it does update frequently and I haven't been able to find a way to prevent it. I've had more success with it than any other program that I've used which is why I put up with that, but it doesn't change the fact that they are in the file in the first place.

Steve- I haven't changed my post processor.

Thanks, all.

-Greg

[Adrian]

Each toolpath will start from home in the preview and that's what would happen if you were to save and run each toolpath individually. However if you output the toolpaths to one file then the home move is at the beginning and end of the whole job not the each toolpath.

[gstanczak]

Thanks, Adrian. That is what I'm used to. The problem is that the machine is now also returning to home between toolpaths and the instruction to do so are in the gcode. There are four locations where the command G0 X0.0 Y0.0 Z0.2 appears in the middle of the file (attached).

-Greg

[adze_cnc]

Are you sure that the .pp file you posted is the one that you used to create the text file that you posted?

I ask because all the arc moves (G2 and G3 commands) in the .pp file have been commented out yet your text file contains G2 and G3 commands.

[Adrian]

The post processor you've posted isn't the one that comes with 10.514.

The X-Carve one in that version inherits the GRBL one and the code in that matches the output in your file as far as the header commands and G2/G3 goes so I believe that is the post processor you're actually running rather than the one you posted.

They aren't any different in terms of rapid moves which is what generates the G0 X Y Z move. The home move at the start and end of the file is a G0 Z followed by a G0 X Y.

I can't see any issues with the processor but if you didn't notice that behaviour before I guess you switched processors without realising.

[gstanczak]

I experimented with different post processors and wasn't able to correct the problem, although I did learn about post processors and appreciate the replies and information on them.

I believe the problem is entirely with the Tiling function. If I setup a job that is 4in x 4in, make two toolpaths, output a file, the machine does not return home between the two toolpaths as expected. If I go back into job setup and change to 4in x 26in, select Tiling, recalculate the same two toolpaths, output a file, the machine returns to home between the two toolpaths and the return to home coordinates command does appear in the output file.

Additionally, there is at least one more difference between the two output files (tiling vs no tiling) which is that the z-coordinate is included in every command line in the Tiled output file wheres in the non-Tiled output file the z-coordinate is included I guess only when the machine needs to change the Z-coordinate.

Would anybody be willing to try to replicate this?

Thanks again,
Greg

[adze_cnc]

Tiling? You mentioned tiling before?

[gstanczak]

Yes, tiling is a feature in Vcarve which allows you to cut material larger than your machine bed, or in the case of the Desktop version of VCarve, material larger than 25in x 25in which the software restricts you to. It appears to me that this feature is the difference between an output file that returns the machine to home between toolpaths and not. Although undesirable, not much of an issue now knowing when to expect it.

[Mark]

Hello Greg,

The chances are that other people may not be able to replicate what you are seeing.
As Adrian mentioned, the post processor that you are using is not the one that is shipped as standard with V10.5.
As adze_cnc pointed out, the post processor that you have posted up does not export G2/G3 arc commands,
so the post processor that you are using is not the one that you have posted up.

Did you get the post processor that you posted up from the "PostP" folder of the software?
If yes, do you have any post processors in your "My_PostP" folder?

If you have any post processors in the My_PostP folder, those are the ones that you will be able to select
from the drop down list of post processors on the Save Toolpaths form.
If this is the case, it will be that copy of the post processor that you are using in the software.

The software will not automatically send a machine to a Home X/Y position before a toolpath,
whether using the Tile Toolpath function or not, however, a number of post processors do contain instructions to do this.

Some machine controls will also automatically do this.

From the sample of code that you have posted up, in the "Header" section of the post processor
there is a line that reads "G0[XH][YH]" If you place a plus symbol (+) at the very beginning of the line,
and save the post processor, that line will be omitted the next time that you save a file.

In the sample that you posted up, there is a move to home at the end of the file as well.
If you wish to remove that as well, place a plus symbol (+) at the very beginning of the second last line of the post processor as well.

I hope that this helps, but if you are still seeing problems, drop a line to support and we will get back to you.

Cheers,

Mark.

[gstanczak]

Thanks, Mark.

I'm still trying to understand the functions within the post processors and information in all the replies. And it is very possible that I uploaded a post processor that was not used to generate the output file that I uploaded. However, my most recent experiment was outputting a file with and without tiling, and I certainly used the same post processor (after learning about the My_PostP folder which is a nice idea) and I saw returning to home between toolpaths in one and not in the other. But, as said, I need to process everyone's replies and understand the post processors more before using up anymore of your guys' time.

Thanks,
Greg