Code editing of Ghost Gunner AR cutting file for PROBE start postion

If anyone out there can assist. After many months of troubleshooting setup of the GGFlex, I finally have it running DDcut and going through the startup process to begin cutting a lower.

To start the probing process of a magazine well. The bit is centered to the well with OEM cut program. But not far enough back (left) to probe.

I need to move Y about 30mm in the - direction (left).

I understand how to change .dd file to .zip then unzip to see all files, but can anyone assist as to which file to then open in Notepad and which line of code to edit to move this bit left (-) about 30mm? I can then add all files back to zip and change back to .dd. Thanks!

Here is one file I suspect might be where I edit this, but what line should I edit here?

M3
G4 P2 (delay)
S3000 (spindle probing)(go slow)

G0 Y-12 (move over to trigger well)
G38.3 Z-25 F30 (probe Z)
G10 L20 P2 Z0 (zero Z)
G0Z1 (move up)

(Calibrate Y)
G0 Y3 (move back to mag well via Yrough)
G0 Z-8 (lower bit into mag well)
G38.3 Y-10 F30 (probe Y)
G20 (inches)
G10 L20 P2 Y0.125 (zero Y)(account for tool tip)
G21 (mm)

(Calibrate X)
G0 Y+9.175 (0.125" tool radius plus 6mm to clear nonrectangular mag well plus clearance)
G0 X+5
G38.3 X+15 F30 (probe X)

G20 (inches)

G10 L20 P2 X+.324 (set Xrough)

G21 (mm)

G0G90G53Z-1. (RETRACT)

G0G90G55X0.Y0. (MOVE TO G55 HOME)

(cut code with WCS:)
(Z=top of trigger well plane)
(Y=inner mag well plane closest to trigger well)
(X=center plane between two inner mag well contact walls, bisecting mag well)



Or do I edit this file to make the bit starting point further back (left)

$H (Home)
g0 y-0.9 (prepare for dummy probe move)
$C
G38.3 Y-1 F100 (verifies latest firmware is installed before cutting; G38.3 isn't supported in v0.9)
$C
M5 (stop motor if running)
G92.1 (Clear offsets if set)

(Set WCS G55 zero to home position)
G10 L20 P2 X0 Y0 Z0
G55 (Enter WCS G55)
G90 (Abs position)
G21 (mm)

G53 G0 X-1 Y-70 (Move to GG center)
G53 G0 Z-60 (Plunge for 0.250 end mill install)

As with most gcode files there are multiple ways to achieve the desired results and doing a dry run after editing small chunks of code is highly recommended to help you learn how each of the different sequential components in the .dd file works.
Specifically regarding .dd files, troubleshooting and/or editing them is generally better suited to the GG user communities out there. We don't support any particular projects or code as part of the FLEX, and provided that the machine's control suite isn't doing anything weird in running the .dd filetype, questions regarding their code and how to modify it are better suited to the original authors of that code.
(I have decent knowledge and experience with running more generic gcode flavors and CAM but can't comment on a lot of the choices they made in configuring their projects - they also happen to have already answered a lot of the frequently asked questions in their own support documentation and will be able to more rapidly point you in the right direction)

The most straightforward option (and the one that GG has recommended in their documentation in the past) is to edit the "02_trig_align" or equivalent file that plunges the rough location to be probed from. The final line has the coordinate values for the rough center, which will be where you'll want to add your offsets for the jig.

Then if your probe movements don't contact in one or more axes, edit the G38.3 values to adjust distance and probe velocity for each axis in the 04 process. Then if your offsets are inaccurate and the well cut ends up off center, make fine adjustments following their procedure (https://ghostgunner.zendesk.com/hc/en-us/articles/360039139652-How-edit-dd-file-to-Move-Fire-Control-Group-FCG-Pocket)

FYI on probing with coated tools or non-conductive workpieces that have questionable resistance, I was recently told to use the GND and SEL pins (top right of the CNC Shield) for the tool and workpiece wires respectively, since they can take in an analog current value that might not be enough to trip the digital pin on the Z+/- pairs.

https://cobcnc.com/adding-a-z-probe/ for a good visual guide
and
https://ghostgunner.zendesk.com/hc/en-us/articles/360039136352-Anodized-and-Non-Conductive-Work-piece for the non-conductive tape/foil method

I understand GGflex wants NO part of advice on DDcut. But selling a GGflex as a GG clone, means we (buyers) need assistance at integrating the two to work together... (I am starting to believe I am the ONLY buyer that has gotten this far?)

The problem with GG forum post on moving the "well_probe" is that it refers to "wall thickness" which sounds as if its instructing on moving the entire pocket that it starts to cut. I do not want to move the pocket? I need to move the starting point of the bit for probing.

If I can not edit the starting point of the bit... An old email you sent said something about editing the 1mm probe range of travel to a longer distance. Like 10-30mm. Could you advise which line of code to find that in? GG post is not clear at all...

I assume after I get that right, then I need to edit the "probe_selector" file to move the starting point of the side wall pin holes. So I need that line as well.

I am guessing I need to edit the below two files:
02_Trig_Align.txt
06_Align_Selector.txt

First file, this line:
G0G55 X26.5 Y-39.5

Second file, this line:
G53 G0 Y-26 X-35

Adding to Y, correct?

So would this move starting point of bit left 30mm?
G0G55 X26.5 Y-69.5

OK, I think after countless of months and thousands of hours I have to finally give up on this POS. It's clear it "CAN NOT WORK AS A GHOST GUNNER CLONE".

Due to the home action of DDcut banging the X axis upward and not stopping when the X limit is touched, I bought a pack of 6 new limit switches and tried 2 of them. Both with the same result. DDcut not stopping when the x limit is reached.

So I tried ignoring the home feature all together. I leveled the X axis table, mounted my AR15 jig with aligning by hand the bit in the magwell exactly as it needs to sit before probe function. I hooked up my red and black probe wires and opened DDcut. I ran the AR15 cut program and DDcut has NO way I can see to skip to the PROBE step- bypassing all the Home and warm up stages?!?!

How do I go about getting this returned and refunded??? It's clearly never going to function as advertised.

Pegasus wrote:

I am guessing I need to edit the below two files:
02_Trig_Align.txt
06_Align_Selector.txt

First file, this line:
G0G55 X26.5 Y-39.5

Second file, this line:
G53 G0 Y-26 X-35

Adding to Y, correct?

So would this move starting point of bit left 30mm?
G0G55 X26.5 Y-69.5

This is correct. After it homes, the tool moves to the location so that you can remove/install the 1/4" endmill.

The next time it moves, it moves so that the endmill sits where the magwell will be. This second movement is dictated by the text file "02_trig_align.txt"

The line to change would be: G0G55 X26.5 Y-39.5

To lower the table you need to add to the X value, to make the table higher you will need to subtract.

To move the endmill to the left (y axis), you will need to subtract, to move to the right you will add.

For example is your endmill sits 15mm to the right and 15mm too low, you will need to move the endmill to the left and the table down.

Your new line of code would be: G0G55 X41.5 Y-54.5