I've used Mach3 with Artcam for years, and recently changed to using Vectric software.   When I tried my first file on my Mach3 machine using Vectric file and Mach3 Arc/In post processor, the Z axis drilled right into the spoilboard and was headed for China.  I hit EStop to stop it. 

I don't think I have made any config changes in Mach3,  so I expect something in my file or post is incorrect.   Here are the first several lines:

( U-End Pockets S1 38_3-S1 Profile 38 )
( File created: Saturday October 30 2021 - 09:06 AM)
( for Mach2/3 from Vectric )
( Material Size)
( X= 96.000, Y= 48.000, Z= 0.750)
()
(Toolpaths used in this file:)
(S1 Profile 38)
(Tools used in this file: )
(1 = Two Flute Straight {3/8" dia. - 1" cut length})
N100G00G20G17G90G40G49G80
N110G70G91.1
N120T1M06
N130 (Two Flute Straight {3/8" dia. - 1" cut length})
N140G00G43Z0.8000H1
N150S18000M03
N160(Toolpath:- S1 Profile 38)
N170()
N180G94
N190X0.0000Y0.0000F120.0
N200G00X9.9652Y2.5655Z0.2000
N210G1Z-0.3850F40.0

Can some one tell me if there is something in the GCode setup that might cause this diving?   If not, what settings can I check to see what's going on?   
Thank you! 

Wayne from White Salmon


 

I would compare it with the old programs you have.

The only thing I do not see is a G54 or G55 etc to set the fixture offset but you may be using G53

Graham- 
Thank you for taking time to reply!   I've compared this file with one I have used on this machine created in Artcam.   While there are some differences (like line numbers) the codes like G17, G20, G90, G49, etc are the same.   I've looked them up to see what they mean and I don't think this code is the issue.

But I want to clarify one thing-  my old Artcam post processor had a .TAP suffix.   The Vectric suffix is .txt.   Does Mach 3 care about this?  Does this change how Mach3 processes a file (TAP versus .txt)? 

I'll take a look at my machine settings-  soft limits and limit switches, and offsets, to see if this is the issue.   

THanks for your input Graham.

Wayne from White Salmon

The file extension is not a problem, mach3 will read TAP,TXT,NC,CNC and any other text based file and it has no bearing on how it is interpreted.

The only code you list that can move the z axis is G49 but it would have to have a G43 and a H to make it move.

It might be good to post the first 20 lines of each program just to be sure.

Here are the first 20 lines of an Artcam file that worked on this machine:
(Insert2Test1)
(Material Size) (X=96.000, Y=48.000, Z=0.750)
(Tool Number:1) (0.375 inches dia. slot drill)
G017 G20 G49 G80 G90 G91.1
G0Z0.7500
M3 S15000
G0 X10.4714 Y4.2107 Z0.7500
G1   Z0.0000 F20
G1 X10.4731 Y4.1785 Z-0.0163 F50
X10.4783 Y4.1455 Z-0.0332
X10.4874 Y4.1122 Z-0.0507
X10.5004 Y4.0793 Z-0.0687
X10.5175 Y4.0474 Z-0.0870
X10.5385 Y4.0173 Z-0.1056
X10.5630 Y3.9897 Z-0.1243
X10.5906 Y3.9652 Z-0.1430
X10.6207 Y3.9443 Z-0.1616
X10.6525 Y3.9272 Z-0.1799
X10.6855 Y3.9141 Z-0.1978
X10.7188 Y3.9051 Z-0.2153

AND... here are 20 lines from the Vectric file for comparison:

( S2 Pockets 38_1-S2 Pockets 38 )
( File created: Saturday October 23 2021 - 05:19 PM)
( for Mach2/3 from Vectric )
( Material Size)
( X= 96.000, Y= 48.000, Z= 0.750)
()
(Toolpaths used in this file:)
(S2 Pockets 38)
(Tools used in this file: )
(1 = Two Flute Straight {3/8" dia. - 1" cut length})
N100G00G20G17G90G40G49G80
N110G70G91.1
N120T1M06
N130 (Two Flute Straight {3/8" dia. - 1" cut length})
N140G00G43Z0.8000H1
N150S18000M03
N160(Toolpath:- S2 Pockets 38)
N170()
N180G94
N190X0.0000Y0.0000F120.0
N200G00X3.7129Y24.6217Z0.2000
N210G1Z0.0000F30.0

Thank you so much for taking time on this Graham.   I'm hoping to make another careful attempt this weekend, so your help is appreciated.

Wayne from White Salmon

Looking at the code the old programs have no tool or offsets active so my guess is that if you check the tool offset for tool 1 and set it to zero all will be well.

Or you could remove the T1 M6 at line 120 and the G43 H1 from line 140 in the new program.

Hi Graham-  just wanted to say I worked on the machine today and set the offset to zero.  That seemed to fix things.  I had some other minor issues but was able to cut files and had no unexpected z axis dives at all. 
THANK YOU!