tiling toolpath malfunction

[Diggin2day1]

I attempted to cut a 45” workpiece(table) on my Laguna IQ with 36” bed. I used the tiling toolpath feature and tiled the 49” slab of wood into 2 pieces at 24.5” with a 3” overlap. Used two dowel pins on each side of the workpiece, Slid the workpiece through the “Y” axis and it all lined up perfectly. Continued through the second(T2) portion of my toolpaths without issue(large pocket toolpaths lined up perfectly, etc)... UNTIL... I attempted to run (2) separate outside profile toolpaths. One of the profile cuts is a 3/8” roundover bit and the other is a 1/2” endmill used to cut out the shape. The cut lined up perfect from the start and proceeded about 12” until it took a wild turn inward and ruined(for the second time in two days) almost $100 in cherry.
The first time this happened I was running the 3/8” roundover bit along the profile and at the same spot it started cutting inward and ruined the workpiece. At the point when it veered off, the feed slowed to a crawl(almost like when it ramps). By the time I realized and heard what was going on it had already cut over an inch. Due to other screw-ups and miss alignment issues(my fault) I scrapped that slab of cherry and tried it again.
After the first wild ride I actually started from scratch and opened new vcarve file. Drew the piece from scratch with all new toolpaths... previewed the toolpaths(whole piece and T1/T2 separately) and they all looked perfect.
I am still new to CNC and Vcarve, but I have been moving along with great success. This is my first attempt at a tiled toolpath and I am confident that it was done correctly.
After the piece was ruined, I figured “what the heck”... let it run and see what it is doing. I re-zeroed the Z-axis to be higher than the workpiece and not actually cut anything... just so I could see where it was going. It seems that when it veered off that it cut across the 4” radiused corner and continued the rest of the profile without issue(even cut the opposing 4” radiused corner with perfection).
I am at a loss and feel like it is a software malfunction and not a “operator error”... The profile shape was simply made with a rectangle and radiused corners(no wonky design)... hopefully I can get some help/ideas or others that have experienced a similar issue.

first attempt with 3/8" roundover bit...

2nd attempt with 1/2" endmill for profile cut.

another view of 2nd attempt

What its supposed to look like!!!

[martin54]

What does the toolpath preview look like ? If that looks good then have a look at your control software & check your machine for any sort of mechanical problems.
After you had stopped the machine did you send it back to zero ? Did it return to its original starting position??

Uploading your file (copyright permitting) is helpful as it will aid the forum experts

[Diggin2day1]

The preview looks perfect... even watched the animated preview in slow motion to be sure there wasn't any discrepancies. VCarve Pro is my controlling software, machine is in excellent/new condition without ever an issue.

[martin54]

No vcarve is your Cad/Cam software your control software is the software that controls the CNC machine, don't know what that would be for your brand of machine.
If the toolpath preview is perfect then the problem lies else where, are you using the correct post processor for your machine ? Even new machines can go wrong or have problems

[Diggin2day1]

I have the RichAuto controller... just seems strange that the ONLY time I have ever had an issue is when I tried using the tiling toolpath function. Machine has been operating flawlessly.

[Diggin2day1]

I forwarded all of this information to a software tech at Laguna(who was extremely helpful) and he spent a few days trying to figure it out as well. He called me and had me check the settings on the HandHeld Controller of my CNC and they were fine. He had me send him the .crv file so he could run it... his machine messed it up as well. He looked further into the G Code and got back to me with this email response:

The good news it isn't you or your IQ CNC it is some kind of glitch in the G-code out put.
I have try many things to get it to work but no luck. It is something when it outputs the G-code in VCarve Pro.
Below is where the problem is in the G-code this J should be 0.00. I change it on the attached (T2_endA.mmg ) file and did a air run and it looks good.
I would contact Vectric support at http://support.vectric.com.
I'm sorry that I can't be of more help.

[Diggin2day1]

Following up with this issue, I contacted Vectric with all the information that I had... Her is their response:

Charlie Pullen (Vectric Ltd.)
Jan 3, 09:56 WET

Hello Keith.
Please see the new Post Processor linked below for download.
This has been edited to remove all Arc commands.
Please download this linked file below and save it to your PostP folder.
This can be accessed via the software by going to File Menu -> Open application Data Folder
Once the .pp file is saved into your PostP Folder, close the software and restart it to load the new Post Processor.
With all new Post Processors we recommend doing a dry run before using it in any important projects, to ensure it is working as fully intended.
I hope this helps.
Best Regards
Charlotte
Vectric Support
Vectric Ltd | Precision House| 2 Arden Road
Alcester | Warwickshire | B49 6HN | United Kingdom
Attachment(s)
Laguna_IQ_HHC_Noarc.pp