Welcome, Guest. Please login or register.
Did you miss your activation email?
July 28, 2014, 11:36:00 PM

Login with username, password and session length
Search:     Advanced search
* Home Help Search Calendar Links Login Register
+  Machsupport Forum
|-+  G-Code, CAD, and CAM
| |-+  G-Code, CAD, and CAM discussions
| | |-+  G42 problem
Pages: « 1 2 3 »   Go Down
Print
Author Topic: G42 problem  (Read 6356 times)
0 Members and 1 Guest are viewing this topic.
Graham Waterworth
Administrator
*
Offline Offline

Posts: 1,768


West Yorkshire, England



View Profile WWW
« Reply #10 on: December 02, 2006, 10:48:54 AM »

Oops, Good point Gerry, forgot to mention that bit,

Its a work habit, we have 20 tools in our machines so we always add 20 to the tool number for the dia offsets as our machines don't have length and dia in one offset.

The circles are 25mm dia on a 50mm grid.

Graham.


« Last Edit: December 02, 2006, 10:50:50 AM by Graham Waterworth » Logged

G-Code is on the cutting edge

Autovalues Engineering, CNC machining specialists, Bradford, England
C.Michael
Active Member

Offline Offline

Posts: 26


View Profile
« Reply #11 on: December 02, 2006, 11:55:12 AM »

I think I have it...Let me see if I have the concept by trying to explain it back to you..If I have a straight level line on my screen horizontal...If the code has the bit traveling left to right and I want the bit to be offset to the north side (top) then a G41...traveling the same direction but offset to the south (bottom) then a G 42....If the code has the bit traveling right to left...and I want the bit offset to the north,then a G42,,,If I want it to the south then a G41...With no tool changer then the code would be G41p.0625...if I had a router cutter bit of .125 inches...Sir Graham..can you grade my test please  : )
Logged
Graham Waterworth
Administrator
*
Offline Offline

Posts: 1,768


West Yorkshire, England



View Profile WWW
« Reply #12 on: December 02, 2006, 12:35:16 PM »

10 out of 10, go to the top of the class  Grin

Graham.
Logged

G-Code is on the cutting edge

Autovalues Engineering, CNC machining specialists, Bradford, England
Graham Waterworth
Administrator
*
Offline Offline

Posts: 1,768


West Yorkshire, England



View Profile WWW
« Reply #13 on: December 02, 2006, 01:59:24 PM »

Here is what you are talking about,  I think I have put in all the detail this time.

Tool dia 10mm
Height offset 3
Using 'P' this time, set to 5.0mm

Graham.

O0002 (G41 - G42)

G21 G40
G91 G28 X0 Y0 Z0

N1 (10MM END/SLOT DRILL)
(TOP LEFT EDGE)
G54 G00 G90 G43 X-2.5 Y12.5 Z25. H3 S2500 M3
Z1.
G01 Z-1. F500.
G41 P5.0 X-7.5 Y7.5
G03 X0. Y0. R7.5
G01 X25.
G03 X32.5 Y7.5 R7.5
G01 G40 X27.5 Y12.5
G00 Z25.

(TOP RIGHT EDGE)
G00 X77.5 Y12.5
Z1.
G01 Z-1.
G42 P5.0 X82.5 Y7.5
G02 X75. Y0. R7.5
G01 X50.
G02 X42.5 Y7.5 R7.5
G01 G40 X47.5 Y12.5
G00 Z25.

(BOTTOM LEFT EDGE)
G00 X-2.5 Y-62.5
Z1.
G01 Z-1.
G42 P5.0 X-7.5 Y-57.5
G02 X0. Y-50. R7.5
G01 X25.
G02 X32.5 Y-57.5 R7.5
G01 G40 X27.5 Y-62.5
G00 Z25.

(BOTTOM RIGHT EDGE)
G00 X77.5 Y-62.5
Z1.
G01 Z-1.
G41 P5.0 X82.5 Y-57.5
G03 X75. Y-50. R7.5
G01 X50.
G03 X42.5 Y-57.5 R7.5
G01 G40 X47.5 Y-62.5
G00 Z25.
G91 G28 Y0 Z0
M30



* G41_-_G42_V2.jpg (19.72 KB, 654x627 - viewed 184 times.)
Logged

G-Code is on the cutting edge

Autovalues Engineering, CNC machining specialists, Bradford, England
C.Michael
Active Member

Offline Offline

Posts: 26


View Profile
« Reply #14 on: December 03, 2006, 02:57:31 AM »

(TOP LEFT EDGE)
G54 G00 G90 G43 X-2.5 Y12.5 Z25. H3 S2500 M3
Z1.
G01 Z-1. F500.
G41 P5.0 X-7.5 Y7.5               I see the g41 code here with P offset and the offset coordinates...  How are you coming up with these coordinates??
G03 X0. Y0. R7.5                    Do you have to have these coordinates?   I thought you just put in the P5.0 and you were done??
G01 X25.                               
G03 X32.5 Y7.5 R7.5
G01 G40 X27.5 Y12.5
G00 Z25.
« Last Edit: December 03, 2006, 03:16:28 AM by C.Michael » Logged
Graham Waterworth
Administrator
*
Offline Offline

Posts: 1,768


West Yorkshire, England



View Profile WWW
« Reply #15 on: December 03, 2006, 04:57:43 AM »

The top left line starts at X0 Y0 and ends at X25. Y0,  by starting the cut at a known point in free space that is larger than or equal to the cutter radius you don't get pips on the edges of the start and finish cut.

I tend to use 1.5 times the cutter radius

The cutter is 10mm dia so, 10/2=5  then 5*1.5=7.5

By applying the comp on the move to x-7.5 y7.5 the tool is in the right place ready to blend without any uncut edges.

It all makes for a much nicer cleaner cut.

If you load the code into Mach3,  double click the code viewer, then scroll down the code line by line you will see the tool path highlighted line by line.

Graham.
Logged

G-Code is on the cutting edge

Autovalues Engineering, CNC machining specialists, Bradford, England
ger21
Global Moderator
*
Offline Offline

Posts: 3,803



View Profile WWW
« Reply #16 on: December 03, 2006, 07:51:24 AM »

When I'm cutting out parts, here's my method for doing comp using AutoCAD. Pick a corner of the part where you want to start and stop, and extend those lines a little more than 1/2 the tool diameter. Then I add the leadin move to the start. I use the leadin to ramp into the part, and since I work with wood, I find that an 1-1/2" long ramp works pretty well with a 1/2" tool. I try to keep in in line with the part profile, offset to the side by the radius, which will actually let the tool enter the stock on a fairly straight path while the comp is being applied.Then I add a leadout move, where I ramp out of the part, which prevents a dwell at the end of the cut which can dull the tool a little bit. I use a macro that I wrote for AutoCAD that exports the g-code directly from AutoCAD, with the G41/G42 code and ramping automatically applied.
Logged

C.Michael
Active Member

Offline Offline

Posts: 26


View Profile
« Reply #17 on: December 03, 2006, 02:18:39 PM »

This is the part where I feel like such a dunce...On that top left line...the cords are X0,Y0....X25,Y0   with the lead in and everything that cutter bit is going right down the middle of the line...then my part would be 1/16th too small (with a 1/8th bit)  I would need the bit to travel on the line of X0,Y.0625...X25,Y.0625...Do I need to draw my part a 1/16th of an inch bigger all away around to make the bit cut my part at the right size???
Logged
Graham Waterworth
Administrator
*
Offline Offline

Posts: 1,768


West Yorkshire, England



View Profile WWW
« Reply #18 on: December 03, 2006, 02:23:26 PM »

You are not a dunce,

when you are using G41 or G42 you program the tool path as if the cutter had a diameter of zero, e.g. you draw it to the correct size you want to cut,  then the compensation dose the rest.

Graham.
Logged

G-Code is on the cutting edge

Autovalues Engineering, CNC machining specialists, Bradford, England
C.Michael
Active Member

Offline Offline

Posts: 26


View Profile
« Reply #19 on: December 03, 2006, 03:36:23 PM »

Thank you Graham,I appreciate your fantastic help..It is amazing how much patience you have!!...This is what I am trying to do..I like to design and build model airplanes using autocad 2000...after drawing the part of the plane (a wing rib for ex.) ..I import the dxf file to Lazycam..this rib may have 3 or 4  lightening holes in it..as you know it has three options for the lead in..I do that for each hole and for the outside profile of the rib..these lead ins are a good size for a clean cut as you described..I put a check in the box that says..Use G41/G42 on lead in outputs...in the Posting options..After creating the G code, I open the file up using notepad ..You can see the lines (many of them) that has the G 41 or G42 on it...But that is all the line has...G42...nothing more...I go to each of these lines and add P0.0625...To make the line read exactly this...G42P0.0625....For a .125 router bit..If it reads G41 I put in...G41P0.0625...With the lead ins created in Lazycam and the modifying of the G41/G42 lines,I should be done ..shouldn't I  ??  Michael
Logged
Pages: « 1 2 3 »   Go Up
Print
Jump to:  

Powered by MySQL Powered by PHP Powered by SMF 1.1.19 | SMF © 2013, Simple Machines Valid XHTML 1.0! Valid CSS!