Messages

2351

G-Code, CAD, and CAM discussions / Re: G42 problem

« on: December 04, 2006, 03:50:12 AM »

Hi Michael,

I have looked at your files and all look OK,  I think the problem is with Lcam, its just not putting the compensation size (P) or a tool offset (D) into the code.

This is what I would do :-

Create your programs with Lcam

Set a tool length and diameter in the tool offset table, use tool 1 with a length of 0.00 and a diameter of .0625"

On the first G41/G42 in your program add D1, you do not need to do this for every G41/G42 as D1 is global.

e.g.

N5 (File Rib1 )
N10 (Default Mill Post)
N15 (File Posted in Mill Mode)
N20 (Sunday, December 03, 2006)
N25 G90 G80 G40 G91.1
N30 G0  Z1.0000
N35  X1.3309  Y1.9273
N40  Z0.2500
N45 M3
N50 G1  Z-0.1250  F10.00
N55 G42 D1
N60  X1.5034   F15.00
...........

This will make Mach use the tool offset you set in tool 1 for the compensation on the contours.

Try this with the tool just scratching the face of the material, you should be able to measure the size to comfirm all is well.

This is what my Sim gives as the profile.

Graham.

2352

G-Code, CAD, and CAM discussions / Re: G42 problem

« on: December 03, 2006, 05:49:45 PM »

Michael,

No DXF file yet.

Graham.

2353

G-Code, CAD, and CAM discussions / Re: G42 problem

« on: December 03, 2006, 03:43:08 PM »

Email me your DXF file and the code generated by Lcam and let me see what we are talking about.

You can get my email by clicking on my user name above the picture of my car.

Graham.

2354

G-Code, CAD, and CAM discussions / Re: G42 problem

« 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.

2355

VB and the development of wizards / Re: Modify text file

« on: December 03, 2006, 11:32:17 AM »

If you click the EDIT PROGRAM button, the text file should be sent to notepad for editing.

Graham.

2356

G-Code, CAD, and CAM discussions / Re: G42 problem

« 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.

2357

G-Code, CAD, and CAM discussions / Re: G42 problem

« 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

2358

G-Code, CAD, and CAM discussions / Re: G42 problem

« on: December 02, 2006, 12:35:16 PM »

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

Graham.

2359

G-Code, CAD, and CAM discussions / Re: G42 problem

« 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.

2360

G-Code, CAD, and CAM discussions / Re: G42 problem

« on: December 02, 2006, 01:42:23 AM »

That would depend on where you live UK or US 

G41 and G42 are dependent on the direction you are traveling clockwise or counterclockwise

This should help to explain it :-

O0001 (COMP G41 AND G42)

G21 G40
G91 G28 X0 Y0 Z0

(OUTSIDE CW)
G54 G00 G90 G43 X-19.445 Y35.91 Z25. H3 S2500 M3
G00 Z1.
G01 Z-1. F500.
G01 G41 D23 X-5.303 Y14.697 F800. S2500
G03 X0. Y12.5 R7.5
G02 X10.827 Y-6.248 R12.5
G02 X-10.827 R12.5
G02 X0. Y12.5 R12.5
G03 X5.303 Y14.697 R7.5
G01 G40 X19.445 Y35.91
G00 Z25.

(INSIDE CW)
G00 X46.25 Y3.75
G00 Z1.
G01 Z-1. F500.
G01 G42 D23 X50. Y12.5 F800. S2500
G02 X60.827 Y-6.248 R12.5
G02 X39.173 R12.5
G02 X50. Y12.5 R12.5
G01 G40 X53.75 Y3.75
G00 Z25.

(INSIDE CCW)
G00 X53.75 Y-46.25
G00 Z1.
G01 Z-1. F500.
G01 G41 D23 X50. Y-37.5 F800. S2500
G03 X39.173 Y-56.248 R12.5
G03 X60.827 R12.5
G03 X50. Y-37.5 R12.5
G01 G40 X46.25 Y-46.25
G00 Z25.

(OUTSIDE CCW)
G00 X19.445 Y-14.09
G00 Z1.
G01 Z-1. F500.
G01 G42 D23 X5.303 Y-35.303 F800. S2500
G02 X0. Y-37.5 R7.5
G03 X-10.827 Y-56.248 R12.5
G03 X10.827 R12.5
G03 X0. Y-37.5 R12.5
G02 X-5.303 Y-35.303 R7.5
G01 G40 X-19.445 Y-14.09
G00 Z25.

G91 G28 Y0 Z0
M30