Centroid Community CNC Support Forum

Trying to cut a circular pocket with intercon. Calling out tool #1 at beginning of program. When i change the size of the cutter in the tool offsets page nothing happens to the size of the pocket?? I go into the program in intercon and look at the tool line and it shows that the size of the tool has changed. Then when i post and rerun the program it changes the size like what i wanted. But if i change it again nothing until i open the the intercon edit again??

Intercon is a conversational programming language. When you click F10 Post and Exit, it converts the conversational program into g-code. Any changes made after that to the tool tables are unknown to the g-code. Only after you reload the conversational program and re-post it will the changes be incorporated.

If you use cutter comp in your intercon programs, and later change the cutter diameter offset in the tool table, then that change WILL make a difference in your program.

According to the manual circular pocket has cutter comp automatically added. But nothing happens when i change the tool dia. in setup, tool, offsets lib.
I messed with it all day yesterday and made another test program today still doesn't work. I have tool 1 progamed as .5 dia. originally and then changed it to .1 dia. still cut the same size hole??

The "cutter comp" that is "automatically added" is pre-compensation: Intercon posts out G codes that go around circular path that is smaller than the requested pocket diameter, by the current cutter diameter.

Intercon does not include G41 or G42 codes, for on-the-fly cutter compensation, in any of its pocket or frame cycles.

Therefore, if you are using pocket or frame cycles, and you want to change your cutter diameter value, you need to re-post.

Guess that explains why i never use the conversational.

cnctc wrote: ↑Thu Sep 16, 2021 9:50 am Guess that explains why i never use the conversational.

Intercon works great for what it is intended for.
Take the time to read the operator's manual and understand it, you might find it beneficial at times.
I use it more and more.
Marty

I'm hijacking this thread since all the experts chimed in... Intercon - circular pocket. I have a 3/8" dia end mill = 9.525mm and I need to make a counterbore of 10.1mm x 10mm deep. I can't seem to get the program to post. It gives me an error on the circular pocket line but I don't know what the error is. Could it be that the pocket diameter is too small for my endmill? If so, how do I make a counterbore without having a tool with exact diameter?

It would help us if you actually told us what the error was. Your tool block should have the tool dia as 9.525. The circular pocket block should have the diameter as 10.1.

johnballard wrote: ↑Tue Jun 21, 2022 8:45 pm I'm hijacking this thread since all the experts chimed in... Intercon - circular pocket. I have a 3/8" dia end mill = 9.525mm and I need to make a counterbore of 10.1mm x 10mm deep. I can't seem to get the program to post. It gives me an error on the circular pocket line but I don't know what the error is. Could it be that the pocket diameter is too small for my endmill? If so, how do I make a counterbore without having a tool with exact diameter?

Quick test whats Intercon puts out with an 9.525mm mill:

; ICN_PATH = C:\intercon\c.icn
; --- Header ---
N0001 ; CNC code generated by Intercon v4.20
; Description: 10.1
; Programmer: Uwe
; Date: 22-Jun-2022
M25 G49 ; Goto Z home, cancel tool length offset
G17 G40 ; Setup for XY plane, no cutter comp
G21 ; millimeter measurements
G80 ; Cancel canned cycles
G90 ; absolute positioning
G98 ; canned cycle initial point return
; --- Tool #2 ---
;Tool Diameter = 9.5250 Spindle Speed = 4000
;9.525mm Alu
G49 H0 M25
G0 X0.0 Y0.0
N0002 T2 M6
S4000 M3
M8
G4 P1.00 ; pause for dwell
G43 D2
; --- Circular Pocket ---
N0003 X0.0 Y0.0 Z3.0 H2
G1 G91 X0.0 Y0.0 Z-3.0 F150.0
X0.0 Y0.0 Z0.0
X0.0 Y0.0 Z-2.0
G2 X0.0 Y0.288 Z0.0 J0.144
X0.0 Y0.0 Z0.0 J-0.288 F200.0
G1 X0.0 Y-0.288 Z0.0 F150.0
X0.0 Y0.0 Z-2.0
G2 X0.0 Y0.288 Z0.0 J0.144
X0.0 Y0.0 Z0.0 J-0.288 F200.0
G1 X0.0 Y-0.288 Z0.0 F150.0
X0.0 Y0.0 Z-2.0
G2 X0.0 Y0.288 Z0.0 J0.144
X0.0 Y0.0 Z0.0 J-0.288 F200.0
G1 X0.0 Y-0.288 Z0.0 F150.0
X0.0 Y0.0 Z-2.0
G2 X0.0 Y0.288 Z0.0 J0.144
X0.0 Y0.0 Z0.0 J-0.288 F200.0
G1 X0.0 Y-0.288 Z0.0 F150.0
X0.0 Y0.0 Z-2.0
G2 X0.0 Y0.288 Z0.0 J0.144
X0.0 Y0.0 Z0.0 J-0.288 F200.0
X0.0 Y-0.288 Z0.0 J-0.144
G0 G90 X0.0 Y0.0 Z3.0
; --- End of Program ---
N0004 G49 H0 M25
G40 ; Cutter Comp Off
M5 ; Spindle Off
M9 ; Coolant Off
G80 ; Cancel canned cycles
M30 ; End of program

Uwe

Which seems correct - arc moves between +0.288 and -0.288. So (0.288*2)+9.525 = 10.101