Post Processor not working

This forum is for general discussion regarding VCarve Pro
Post Reply
TopStyle
Posts: 6
Joined: Wed Jul 07, 2021 2:55 pm
Model of CNC Machine: Giben G4 EVO

Post Processor not working

Post by TopStyle »

Hello, im new here to the forum
We have a Giben G4 EVO and a Laguna SmartShop 2 here at the shop, we do mainly cabinet boxes ( kitchen, bath etc) and closets, this is the first job ill be needing a software like V Carve. Ive always used Cabinet Vision and cabinet making software for my softwares.
I designed the molding we need for this job, saved the toolpaths with the " Laguna SmartShop BR ATC" post processor and it worked fine, then i saved with the " Giben G4 510 Arc ATC inch" post processor. i believe everything worked except the Z height that was messed up.
I created a new job, 21” wide 6” high and 2” thick, one profile toolpath across the part with 1” deep. I copied the same toolpath 2 more times, each toolpath using a different tool bit. Tool#1 using 3/8” compression. Tool#2 using ¼”downshear. Tool#3 using 3/8” downshear.
All toolpaths should lower 1” from the spoilboard on the ideal scenario, but..
Tool #1 lowered to about 1 7/8” from the spoil board.
Tool #2 lowered to about 1 3/4” from the spoil board.
Tool #3 lowered to about 4” from the spoil board!
I sent this to the support email last week but i guess no one figured out why this happened. I don't know if I'm missing something simple on the software, but when i preview the toolpaths the 3d shows me exactly what i need, and since its working fine on my laguna im assuming this is something with the post processor.
Anyone has any ideas? Anyone has a Giben?
I would appreciate the help! Thank You!

User avatar
adze_cnc
Vectric Wizard
Posts: 4324
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Post Processor not working

Post by adze_cnc »

In this case viewing the g-code file (the one that is sent to the cnc machine) would help. If all the Z moves in the g-code correctly go down to 1" below the surface then there is something wrong with how you specify the tools on your machine (which is what I suspect).

User avatar
TReischl
Vectric Wizard
Posts: 4575
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 48X36X7 RP 2022 UCCNC Screenset
Location: Leland NC

Re: Post Processor not working

Post by TReischl »

+1 on learning to read g code. Saves tons of guessing when things go wrong.

It is not complicated when it comes to the motion commands.
"If you see a good fight, get in it." Dr. Vernon Johns

TopStyle
Posts: 6
Joined: Wed Jul 07, 2021 2:55 pm
Model of CNC Machine: Giben G4 EVO

Re: Post Processor not working

Post by TopStyle »

These are the 3 gcodes i just tested. 3 different tools using the same line i drew, doing a profile toolpath, 1" deep, using the same post processor. My material was 2" high, so all tools should be 1" from the spoilboard, but the same thing happened
Tool#1 ended up 1 7/8" from the spoilboard
Tool#2 - 1 3/4"
Tool#3 - 4"
Since i have the post processor i use for cabinet making software, would that be of any help to check if there are any differences with this on in vcarve? And could this post processor work in any way in vcarve software?
Sorry if its a silly question, this is really out of my area
Attachments
Tool3.txt
(360 Bytes) Downloaded 48 times
Tool1.txt
(361 Bytes) Downloaded 39 times
Tool2.txt
(358 Bytes) Downloaded 36 times

JBL
Posts: 4
Joined: Tue Jan 12, 2021 3:41 pm
Model of CNC Machine: stepcraft m1000
Location: Northwest Tenn USA

Re: Post Processor not working

Post by JBL »

If i read your gcode files correctly you are calling for tool 3 in the H register and telling machine to use tool 13 hope this makes sense.

TopStyle
Posts: 6
Joined: Wed Jul 07, 2021 2:55 pm
Model of CNC Machine: Giben G4 EVO

Re: Post Processor not working

Post by TopStyle »

The tools are displayed like that on this machine, i believe its because it has a drill block (multi drill), so my tools on the spindle are 11 for tool #1, 12 for tool #2, 13 for tool #3.. etc
I recreated the same part and operation on my cabinet making software, im sending it attached.
I hope this helps
And i really appreciate you guys trying to help me out!!!
Attachments
Tool1Mozaik.txt
(609 Bytes) Downloaded 39 times

User avatar
adze_cnc
Vectric Wizard
Posts: 4324
Joined: Sat Jul 27, 2013 10:08 pm
Model of CNC Machine: AXYZ 4008
Location: Vancouver, BC, Canada

Re: Post Processor not working

Post by adze_cnc »

Yup, all 3 files are going to 1" depth.

Code: Select all

G0 X0.1233 Y-3.0000 Z2.2000
G1 Z1.0000 F200
1st line goes "in the air" to XY position 0.20" above the 2" material thickness (2.20 in total)
2nd line goes down to 1" above machine bed.

Only difference in the 3 files is that tool2.txt uses F20 as speed in line 2,

It's probably something to do with how your tool lengths are specified on the cnc machine. Luckily it didn't plunge into the machine bed.

TopStyle
Posts: 6
Joined: Wed Jul 07, 2021 2:55 pm
Model of CNC Machine: Giben G4 EVO

Re: Post Processor not working

Post by TopStyle »

Thats good that the gcode is working
I just dont understand why on cabinet making software it apparently doesn't specify anything different for the Z height.
Ill keep trying different things here and let you guys know! And if anyone has any ideas of tests let me know
Thanks

User avatar
sharkcutup
Vectric Wizard
Posts: 2885
Joined: Sat Mar 26, 2016 3:48 pm
Model of CNC Machine: Shark HD3 Pro Extended Bed with Spindle
Location: U.S.A.

Re: Post Processor not working

Post by sharkcutup »

I know that this may be a redundant question BUUUUTTTT --- How is the Z-zero being set at the machine after each tool change (bit change)?

Sharkcutup
V-Carve Pro Tips, Gadget Tips & Videos
YouTube Channel - Sharkcutup CNC
V-Carve Pro 11.554

User avatar
Adrian
Vectric Archimage
Posts: 14541
Joined: Thu Nov 23, 2006 2:19 pm
Model of CNC Machine: ShopBot PRS Alpha 96x48
Location: Surrey, UK

Re: Post Processor not working

Post by Adrian »

I expect Steven is on the right track. It's probably to do with tool length compensation.

From your previous posts you seem to be saying that the Vectric files are using tools 11, 12 and 13. They aren't they are using 1,2 and 3 instead so check what you have the tool numbers set to in the tool database. The cabinet making software file is using tool number 11.

TopStyle
Posts: 6
Joined: Wed Jul 07, 2021 2:55 pm
Model of CNC Machine: Giben G4 EVO

Re: Post Processor not working

Post by TopStyle »

Success!! On both g codes ( from cabinet making software and VCarve) it indicates "T11", which is my tool #1. But on cabinet making software it then says G43 H11 Z2.
and Vcarve says G43 H1 Z3.0000. So i just manually changed the "H1" to "H11" and it worked! I tried setting the tool number on vcarve to #11 insted of #1, but then it shows "T111" as tool selection, so i believe there is something on the post processor that changes that H1 to H11.
Ill do some more digging to see if i change this, but worst case scenario since for this job ill only need 3 different gcodes i can change them manually.
Thank You ALL for the help!
God Bless you all

TopStyle
Posts: 6
Joined: Wed Jul 07, 2021 2:55 pm
Model of CNC Machine: Giben G4 EVO

Re: Post Processor not working

Post by TopStyle »

Quick update, i compared the two post processor VCarve (Left side) vs cabinet making software (Right side), you can see the attached image, the simplest thing was causing me such a pain..
Just added the "1" between the H and [T] and voila, its working!
Attachments
PostProcessor.JPG

Post Reply