Switching Post Processor From Carbide Motion to UGCS or CNCjs

(Grant Hultman) #1

I am running Vectric V-Carve Pro 9.5 with my Shapeoko XXL and want to play around with different post-processors. I enjoy the idea of being able to switch between (Edit: G-Code Sender, not post-processors), no reason, just to experiment. I have read that it is best to only run one (Edit: G-Code Sender, not post-processors) because those G-code sender’s settings are now on the controller? From my experience, the solutions to my problems often revolve around my personal knowledge, not the machine or computer.

Im trying to try out a different post processor but not clear about the best path to take for transferring settings and jogging smoothly. I also have a triquetra touch probe and plan on using macros in conjunction with my corner jig.

  1. Just downloaded CNCjs app, do I save my G-Code settings from Carbide Motion to my computer then upload (copy and paste) into CNCjs? Are there any preparatory commands needed or tips you might have? Do I need to reflash anything? I have this same question for UGCS.

  2. In both CNCjs and UGCS, I cant jog the machine smoothly it only travels in the specified increment? Again this is likely user error. I am having a hard time finding useful up to date tutorials for one reason or another.

Thanks!

My current G-Code settings straight from Carbide Motion and below that is the CNCjs settings.

(462): <- $132=80.000
(461): <- $131=850.000
(460): <- $130=845.000
(459): <- $122=400.000
(458): <- $121=400.000
(457): <- $120=400.000
(456): <- $112=5000.000
(455): <- $111=5000.000
(454): <- $110=5000.000
(453): <- $102=40.063
(452): <- $101=39.936
(451): <- $100=39.928
(450): <- $32=0
(449): <- $31=0
(448): <- $30=1000
(447): <- $27=5.000
(446): <- $26=25
(445): <- $25=2000.000
(444): <- $24=100.000
(443): <- $23=0
(442): <- $22=1
(441): <- $21=0
(440): <- $20=0
(439): <- $13=0
(438): <- $12=0.010
(437): <- $11=0.020
(436): <- $10=255
(435): <- $6=0
(434): <- $5=0
(433): <- $4=0
(432): <- $3=6
(431): <- $2=0
(430): <- $1=255
(429): <- $0=10
(428): -> $$

Downloaded from CNCjs this morning directly after app download and first connection.

(462): <- $132=80.000
(461): <- $131=850.000
(460): <- $130=845.000
(459): <- $122=400.000
(458): <- $121=400.000
(457): <- $120=400.000
(456): <- $112=5000.000
(455): <- $111=5000.000
(454): <- $110=5000.000
(453): <- $102=40.063
(452): <- $101=39.936
(451): <- $100=39.928
(450): <- $32=0
(449): <- $31=0
(448): <- $30=1000
(447): <- $27=5.000
(446): <- $26=25
(445): <- $25=2000.000
(444): <- $24=100.000
(443): <- $23=0
(442): <- $22=1
(441): <- $21=0
(440): <- $20=0
(439): <- $13=0
(438): <- $12=0.010
(437): <- $11=0.020
(436): <- $10=255
(435): <- $6=0
(434): <- $5=0
(433): <- $4=0
(432): <- $3=6
(431): <- $2=0
(430): <- $1=255
(429): <- $0=10
(428): -> $$

CNCjs 1.9.20 [Grbl]
Connected to COM5 with a baud rate of 115200
Grbl 1.1f [’$’ for help]
client> $$
[MSG:’$H’|’$X’ to unlock]
$0=10 (Step pulse time, microseconds)
$1=255 (Step idle delay, milliseconds)
$2=0 (Step pulse invert, mask)
$3=6 (Step direction invert, mask)
$4=0 (Invert step enable pin, boolean)
$5=0 (Invert limit pins, boolean)
$6=0 (Invert probe pin, boolean)
$10=255 (Status report options, mask)
$11=0.020 (Junction deviation, millimeters)
$12=0.010 (Arc tolerance, millimeters)
$13=0 (Report in inches, boolean)
$20=0 (Soft limits enable, boolean)
$21=0 (Hard limits enable, boolean)
$22=1 (Homing cycle enable, boolean)
$23=0 (Homing direction invert, mask)
$24=100.000 (Homing locate feed rate, mm/min)
$25=2000.000 (Homing search seek rate, mm/min)
$26=25 (Homing switch debounce delay, milliseconds)
$27=5.000 (Homing switch pull-off distance, millimeters)
$30=1000 (Maximum spindle speed, RPM)
$31=0 (Minimum spindle speed, RPM)
$32=0 (Laser-mode enable, boolean)
$100=39.928 (X-axis travel resolution, step/mm)
$101=39.936 (Y-axis travel resolution, step/mm)
$102=40.063 (Z-axis travel resolution, step/mm)
$110=5000.000 (X-axis maximum rate, mm/min)
$111=5000.000 (Y-axis maximum rate, mm/min)
$112=5000.000 (Z-axis maximum rate, mm/min)
$120=400.000 (X-axis acceleration, mm/sec^2)
$121=400.000 (Y-axis acceleration, mm/sec^2)
$122=400.000 (Z-axis acceleration, mm/sec^2)
$130=845.000 (X-axis maximum travel, millimeters)
$131=850.000 (Y-axis maximum travel, millimeters)
$132=80.000 (Z-axis maximum travel, millimeters)

0 Likes

(Andy Gillanders) #2

Carbide Motion, UGCS and CNCjs are all gcode senders not post processors.
All the settings you list are all stored in nonvolatile RAM on the controller board… so they are all the same irrespective of which sender you use. CM has already set the settings correctly for your machine so you do not need to do anything - unless you choose to tweak them yourself for some specific reason.

CNCjs and ugcs move by increments… that’s how they work unlike CM.

Hope that helps!

3 Likes

(Grant Hultman) #3

Ah that makes more sense. From the below thread I have determined that the M6 command is what I need to adjust via the vectric v-carve pro post processor. This is where I have gotten mixed up.
As usual the answer I needed seems slightly obvious now but, I very much appreciate you taking the time to respond.

1 Like

(Neil Ferreri) #4

What do you mean by this? Are you trying to export multiple tool jobs as one?

0 Likes

(Grant Hultman) #5

I guess one can add the M6 command into the Vectric Post Processor. This allows for a multi-tool project (Ex. .250" EM & 60 V) to be saved as one file. The file runs, time for a tool change and the notification pops up on CNCjs. I am going to read the 30 page post processor instructions provided by Vectric to see about adjusting this. This option is comparable to manually entering the M6 command throughout the Gcode instead of Vcarve automatically populating.

I am trying to figure out macros as we speak. The below command keeps trying to send the Z carriage off the grid? I’m guessing that there is a basic concept that I am missing.
Home machine, then execute:
G0 X-826.611 Y-826.611 (This is supposed to be my corner jig zero on the XY)
(This is likely a setting error on my end)

Just finished reading through this! Thank You!!!

Edit: @neilferreri Running a “well” calibrated XXL and a Triquetra Probe. Planning to use your macros as soon as I can get passed go. I am super excited about joining the CNCjs club.
Edit: I’m wondering if my digital XYZ should be in the corner not in the center?
Capture|690x381

0 Likes

(Neil Ferreri) #6

Adding the tool change to a V-Carve post is pretty simple.
Just add:

±--------------------------------------------------
Commands output for tool change
±--------------------------------------------------
begin TOOLCHANGE
“M6 T[T]”

to your post. I use GRBL (mm) with added support for Tool changes and dwells.

By simply sending G0, you are sending it -826 in both X & Y from your WORK zero in the current WCS. You want to send G0 G53 X-826.611 Y-826.611 to use your MACHINE position.

Not sure what you mean here.

0 Likes

(Gary Mitchell) #7

I don’t think this will work as you think it will with UGS. I doubt UGS will pause and say “Change your Bit”. I think it’ll sent the M6 to the Shapeoko and trudge along happily.

I have UGS setup to filter out T1M6, M6 and M7 commands per instructions I found on the Beaver and other sites.

0 Likes

(Neil Ferreri) #8

This is CNCjs stuff.

Better to just not generate unnecessary tool change commands. If you ARE using different tools, this will cause problems.

0 Likes

(Grant Hultman) #9

@neilferreri Thank you for your directions!!! I am using CNCjs Desktop App as my G-Code sender. (Newbie Mistakes) I was getting mixed up with my Machine and Work coordinates.

@wb9tpg I have decided to run CNCjs, either way, I am trying to develop my workflow to replicate a semi-professional design for efficiency. I don’t mind loading files for specific tools, but my understanding was that the M6 commands are recommendable? My other thinking was that the M6 and Z probe process might introduce the slight possibility for error? I am always open to suggestions!

Thank You All for the support!

0 Likes

(Grant Hultman) #10

@neilferreri On the Vectric Forum I asked how exactly to open the .pp file to begin with and how to add the info you shared.

You may already be in the loop but I was trying to run your macros for probing with a Triquetra probe but found an easier way (easier for my situation) to generate the macros with the Triquetra Toolbox option shown in the video below.

Video for generating probe gcode with the Triquetra Toolbox app

triquetra-cnc.com Just the website

forum.vectric.com/viewtopic Forum Post Link

0 Likes

(Neil Ferreri) #11

Go to File –>Open Application Data Folder…
Open the PostP folder, find the post you want to edit

Which Macro? For the 3-axis probe, you just need to edit the endmill diameter & probe dimensions.

I’m familiar with the Triquetra. Probing is pretty much probing. The gcode is all the same. I’d recommend using G10L20 instead of G92 to set offsets though. I know many examples use G92.

0 Likes

(Grant Hultman) #12

This is what the GCode Generated (see end) using the Triquetra Toolbox 1/4"em. Im not crazy about it as of right now and will use yours if I can get it sorted.

  1. At the risk of sounding daft but I’m still finishing college lol Can you clarify where I am to enter my probe dimensions?

@neilferreri Gcode Credit :point_down: &
G21 ;make sure we’re in mm
G91 ;Incremental mode
G38.2 Z-25 F75 ;Probe Z
G0 Z2 ;lift 2mm
G38.2 Z-25 F45 ;Probe Z
G10 L20 P1 Z22 ;Set Current Z as plate thickness ? is this where I adjust the plate thickness?

  1. I’m bad at reading gcode still but does your probe operation run in the same locations and directions as the Triquetra macro? Such as bottom left of the work piece and physically probes XYZ @ the top right corner of the Tri.

I plan on looking more into :point_down: this. I’m a hobbyist but highly focused on precision and sound procedures.

G20 (G21 is better for me)
G92 X0
G92 Y0
G92 Z0
G38.2 X-1 F2
G91 G0 X0.125 F10
G91 G0 Y1 F10
G91 G0 X-0.625 F10
G38.2 Y-1 F2
G91 G0 Y0.125 F10
G91 G0 X0.625 F10
G91 G0 Y-0.625 F10
G38.2 X-0.5 F1
G92 X2.1210
G91 G0 X0.125 F10
G91 G0 Y0.625 F10
G91 G0 X-0.625 F10
G38.2 Y-1 F1
G92 Y2.2970
G91 G0 Y0.125 F10
G91 G0 Z0.8 F10
G91 G0 Y-0.625 F10
G38.2 Z-0.8 F3
G91 G0 Z0.05 F3
G38.2 Z-0.2 F1
G92 Z0.8415
G91 G0 Z0.125 F10
G91 G0 X1 F30
G91 G0 Y1 F30

0 Likes

(Neil Ferreri) #13

@GrantyGrant The Macro I linked has the defaults for the C3D probe (same concept as triquetra). Which corner probe block do you have?

Wasn’t very clear at all, but you were on it.
I just modified the macro to make it easier to configure / fine tune the probe dimensions.
image
Probing /zeroing works the same way it does in this video by C3D.

You’re reading it at least. Keep reading it, and you’ll be fluent in no time.
Keep asking questions.

0 Likes

(Grant Hultman) #14

Wow! That will be fantastic!

Unfortunately, the Z carriage is maxed out so I cant run the macro as it is with my current setup. The corner jig “maximizes” my bed space while still allowing me to index or mill off the contacting face.
Also, the triquetra touch plates banana clip going into the block is “in the way” but I don’t think it’s impossible.

Not sure how difficult it is to adjust the macro to accommodate the 3 axes probe but at the diagonal location to Carbides? In other words same operation but from the upper right-hand corner of the probe, not the lower left-hand corner as it currently is. While I can change my setup around I thought you might be able to create the option easily and I attached pictures WITH the general dimensions typed onto the pictures for clarity and sanity. Not sure if that’s even needed or if you’re interested but I’m sure others could make use of it. I can test and get you video or whatever info you might need.

Uploading: z probe Bottom.png…

(I desperately wanted the Carbide type probe block back in the day but they were out most of the time)


0 Likes

(Neil Ferreri) #15

Why not? You can start with the probe just above the block.
That connector is not in a great place, huh? You want to probe from the left and front because probing from the right and back could move the block. I guess you could hold it. You could have the probe sequence hit right at X0 instead of X5… That will miss the connector.
Your X and Y dimensions are not the ones you should enter. You want the thickness of the edge your probing (with the current macro).

1 Like