504,214 active members
4,780 visitors online
Register for free
Results 1 to 6 of 6
  1. #1
    Join Date
    Oct 2008

    G-Code check...

    In format 2.
    Simple spot some holes then quick drill. Playing with peck even tho not needed.
    Getting an error on the peck cycle - R WORD INVALID (thru simulator not on the fadal itself - yet).
    Lines N70, N165

    Is there an issue retracting my Z back to my original feed stop height of 0.200" or with the simulator?

    (  MODEL: VMC-4020HT)
    (T1  D=0.375 CR=0. TAPER=90DEG - ZMIN=-0.05 - SPOT DRILL)
    (T2  D=0.323 CR=0. TAPER=118DEG - ZMIN=-0.722 - DRILL)
    N10 G90 G94 G17
    N15 G20
    N20 M9
    N25 G28 G91 Z0.
    N30 G90
    (*** TOOL CHANGE ***)
    (T1  D=0.375 CR=0. - SPOT DRILL)
    N35 T1 M6
    N40 S1000 M3
    N45 G4 P180
    N50 G0 E1 X2.7375 Y-0.5
    N55 G43 Z0.8 H1
    N60 M8
    N65 Z0.2
    N70 G98 G81 X2.7375 Y-0.5 Z-0.05 R0+0.2 F7.
    N75 X5.1125
    N80 X7.4875
    N85 X14.6125
    N90 X16.9875
    N95 X19.3625
    N100 G80
    N105 Z0.8
    N110 M5
    N115 M9
    N120 G28 G91 Z0.
    N125 G90
    N130 M1
    (*** TOOL CHANGE ***)
    (T2  D=0.323 CR=0. - DRILL)
    N135 T2 M6
    N140 S1060 M3
    N145 G0 E1 X2.7375 Y-0.5
    N150 G43 Z0.8 H2
    N155 M8
    N160 Z0.2
    N165 G98 G73 X2.7375 Y-0.5 Z-0.722 R0+0.2 Q0.0807 P0.0065 F3.
    N170 X5.1125
    N175 X7.4875
    N180 X14.6125
    N185 X16.9875
    N190 X19.3625
    N195 G80
    N200 Z0.8
    N205 M9
    N210 G28 G91 Z0.
    N215 G90
    N220 G53 X1. Y8.5
    N225 M30

  2. #2

    Join Date
    Jun 2018

    Re: G-Code check...

    The decimal point at the end of the "F" word of the "+" with the "R" word?

  3. #3

    Re: G-Code check...

    I think the decimal point is OK, but I have never seen a R0+0.2 I would expect that to be R0.2
    Jim Dawson
    Sandy, Oregon, USA

  4. #4
    Join Date
    Feb 2011

    Re: G-Code check...

    it looks like it should be a macro statement
    if you have macro ability change R0+0.2 to R[0+.02] and it should read it
    but unless you are going to use a variable to control the R PLANE you should just write it out as Jim has said

  5. #5
    Join Date
    Oct 2008

    Re: G-Code check...

    Yes, I see the format oddity on the R word. (Fusion 360 Fadal post)

    So, reading the Fadal Section 4 document on fixed cycles, the R is suppose to be called such as R0+.xxx so the post is almost doing it right.
    I went out this morning and tried the Gcode I posted yesterday and the Fadal digested it fine. The editor simulator just doesn't like it. (GWizard Editor).
    The editor has mixed feelings about my G-Code and I have mixed feelings about the editor

  6. #6

    Re: G-Code check...

    i just went thru a bunch of my g-code files and F360 post process also creates 'R0+0.2' and i have not had a problem with simulation or running the code on my machine?

Similar Threads

  1. G-CODE check
    By itolond in forum CamWorks
    Replies: 2
    Last Post: 11-08-2015, 08:00 PM
  2. check code for a dynapath 20
    By cnctoolman in forum Dynapath
    Replies: 8
    Last Post: 05-14-2012, 03:53 AM
  3. Can someone check this code for Dyna 20
    By cnctoolman in forum Tree
    Replies: 3
    Last Post: 04-29-2012, 10:34 PM
  4. Rotary G-Code check..!
    By xray34 in forum G-Code Programing
    Replies: 2
    Last Post: 11-25-2010, 01:10 PM
  5. Undercut Check not perform in g-code
    By Wiseco in forum FeatureCAM CAD/CAM
    Replies: 5
    Last Post: 11-22-2005, 11:32 PM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts