Machsupport Forum
G-Code, CAD, and CAM => G-Code, CAD, and CAM discussions => Topic started by: andy_con on March 07, 2013, 09:36:40 AM
-
so i used the wizard to drill a load of holes
heres the main part of the code -
G73 X5 Y40 Z-7 Q1 R7 F76
so its drilling a hole, coming up 7mm, going to the next hole and drilling etc...
but i have to come up 7mm to clear a screw i n the jig and when it comes back down its g1'ing form 7mm high. so takes ages to come down.
is there a way to edit the coding so it does like g00 z1 then g1 the rest of the way down???
thanks
-
you'll have to edit the gcode yourself. unless they have better ideas here.
but.............
g0 z7
x5 y40
G73 G1 F? X5 Y40 Z-7 Q1 R7
somthing like that. just move to pass the screw.
-
but if the code is like this
G73 X5 Y40 Z-7 Q1 R7 F76
x20 y50
x50 y65
and so on
im guess theres no quick was of doing it?
-
i know of no way except to edit the code yourself.
let's hope one of these good people know something.
-
Hi Andy
this should do the job.
G98
G0 Z7
X5 Y40
G73 X5 Y40 Z-7 Q1 R1 F76
Alex
-
IF there is just a single area where the clearance needs to be 7mm then change the code ONLY in that area to clear. The rest can be much closer.
G0 X0Y0 Z1
G73 X5 Y40 Z-7 Q1 R1 F76
X1
Y1
X2
Y2
X3 Y3 R7
X4 Y4
X5 Y5 R1
X6 Y6
G80
-
im drill 144 holes in one bit of work and each holes the drill bit needs to come up 7mm to avoid a screw.
so whats the best way?
the actual code
(Code by Newfangled Wizard, 26/10/2012)
(Program Posted for Aluminum )
G0 G49 G40.1 G17
G80 G50 G90 G98
G21 (mm)
(***** Drill Hole Positions *****)
M6 T2
M03 S3200
M9
G00 G43 H2 Z7
G81 X5 Y5 Z-0.5 R7 F200
X15 Y5
X25 Y5
X35 Y5
X45 Y5
X55 Y5
X65 Y5
X75 Y5
X85 Y5
X95 Y5
X105 Y5
X115 Y5
G80
(***** Drill Hole Positions *****)
G00 Z7
G81 X5 Y15 Z-0.5 R7 F200
X15 Y15
X25 Y15
X35 Y15
X45 Y15
X55 Y15
X65 Y15
X75 Y15
X85 Y15
X95 Y15
X105 Y15
X115 Y15
G80
(***** Drill Hole Positions *****)
G00 Z7
G81 X5 Y30 Z-0.5 R7 F200
X15 Y30
X25 Y30
X35 Y30
X45 Y30
X55 Y30
X65 Y30
X75 Y30
X85 Y30
X95 Y30
X105 Y30
X115 Y30
G80
(***** Drill Hole Positions *****)
G00 Z7
G81 X5 Y40 Z-0.5 R7 F200
X15 Y40
X25 Y40
X35 Y40
X45 Y40
X55 Y40
X65 Y40
X75 Y40
X85 Y40
X95 Y40
X105 Y40
X115 Y40
G80
(***** Drill Hole Positions *****)
G00 Z7
G81 X5 Y55 Z-0.5 R7 F200
X15 Y55
X25 Y55
X35 Y55
X45 Y55
X55 Y55
X65 Y55
X75 Y55
X85 Y55
X95 Y55
X105 Y55
X115 Y55
G80
(***** Drill Hole Positions *****)
G00 Z7
G81 X5 Y65 Z-0.5 R7 F200
X15 Y65
X25 Y65
X35 Y65
X45 Y65
X55 Y65
X65 Y65
X75 Y65
X85 Y65
X95 Y65
X105 Y65
X115 Y65
G80
(Code by Newfangled Wizard, 30/01/2013)
(Program Posted for Aluminum )
G0 G49 G40.1 G17
G80 G50 G90 G98
G21 (mm)
(***** Drill Hole Positions *****)
M6 T3
M03 S3200
M8 (Flood On)
G00 G43 H3 Z7
G73 X5 Y40 Z-7 Q1 R7 F76
X15 Y40
X25 Y40
X35 Y40
X45 Y40
X55 Y40
X65 Y40
X75 Y40
X85 Y40
X95 Y40
X105 Y40
X115 Y40
G80
(***** Drill Hole Positions *****)
G00 Z7
G73 X5 Y30 Z-7 Q1 R7 F76
X15 Y30
X25 Y30
X35 Y30
X45 Y30
X55 Y30
X65 Y30
X75 Y30
X85 Y30
X95 Y30
X105 Y30
X115 Y30
G80
(***** Drill Hole Positions *****)
G00 Z7
G73 X5 Y15 Z-7 Q1 R7 F76
X15 Y15
X25 Y15
X35 Y15
X45 Y15
X55 Y15
X65 Y15
X75 Y15
X85 Y15
X95 Y15
X105 Y15
X115 Y15
G80
(***** Drill Hole Positions *****)
G00 Z7
G73 X5 Y5 Z-7 Q1 R7 F76
X15 Y5
X25 Y5
X35 Y5
X45 Y5
X55 Y5
X65 Y5
X75 Y5
X85 Y5
X95 Y5
X105 Y5
X115 Y5
G80
(***** Drill Hole Positions *****)
G00 Z7
G73 X5 Y55 Z-7 Q1 R7 F76
X15 Y55
X25 Y55
X35 Y55
X45 Y55
X55 Y55
X65 Y55
X75 Y55
X85 Y55
X95 Y55
X105 Y55
X115 Y55
G80
(***** Drill Hole Positions *****)
G00 Z7
G73 X5 Y65 Z-7 Q1 R7 F76
X15 Y65
X25 Y65
X35 Y65
X45 Y65
X55 Y65
X65 Y65
X75 Y65
X85 Y65
X95 Y65
X105 Y65
X115 Y65
G80
M5
m09
-
use G98 as Alex said or do as i said.
either way, you'll need to edit the gcode unless you can edit the
post processor.
-
i cant edit myself not a problem, but what does the g98 code do. i dont get alexs code
-
G98 = return to initial Z level in canned cycle
-
ok
G98
G0 Z7 (z goes to 7)
X5 Y40 (find position)
G73 X5 Y40 Z-7 Q1 R1 F76 (goes down 7)
sorry for being slow dont get how this would work?
so in my code being would g98 replace g73?
M6 T3
M03 S3200
M8 (Flood On)
G00 G43 H3 Z7
G73 X5 Y40 Z-7 Q1 R7 F76
X15 Y40
X25 Y40
X35 Y40
X45 Y40
X55 Y40
X65 Y40
X75 Y40
X85 Y40
X95 Y40
X105 Y40
X115 Y40
G80
-
g98 will retract the z to the level where you started the canned cycle.
so everywhere you have a screw, put g98 before the move and then it will go
back to g73
M6 T3
M03 S3200
M8 (Flood On)
G00 G43 H3 Z7
g98
G73 X5 Y40 Z-7 Q1 R7 F76
X15 Y40
X25 Y40
X35 Y40
X45 Y40
X55 Y40
X65 Y40
X75 Y40
X85 Y40
X95 Y40
X105 Y40
X115 Y40
G80
-
I do not know of a way to do what you want OTHER than using SUB Programing and creating a drill cycle with a fast move to Z0 . That is a LOT of screws to have to clear (;-).
(;-) TP
-
Andy,
the G code you postet ( all the 144 holes ) already contains the G98.
Only thing you have to do is replace The R7 with R1 to get what you want( so far i can see)
Alex
-
Alex I think he needs the R7 to clear the screws BUT does not want to start the drill function at Z7 but at Z0. Needs a rapid from Z7 to Zo before the cycle restarts.
Hopefully I read it correctly on this one. (;-)
I have a sub program that can do it but SUbs can be strange bedfellows if you are just getting started with Gcode.
Just a thought, (;-) TP
-
Alex you are correct that will work that way , I had never thought of it that way.
Good Call (;-),
(;-) TP
-
i spoke to a friend last night as i just wasnt getting it and yes you are correct z7 r2
all sorted, many thanks
-
Hi all,
glad you got it sorted :)
Alex