Messages

1801

General Mach Discussion / Re: Machine Coordinates ????

« on: December 16, 2007, 06:45:02 PM »

Look under Config/Motor Softlimits and see what the G28 home positions are set to.

Also under Config/General bottom right of window un-check copy G59.253 to G54

Graham.

1802

General Mach Discussion / Re: Trouble cutting accurate parts

« on: December 15, 2007, 01:41:45 PM »

If it is a mechanical problem then it would not show in the DRO's.

If you tell Mach to move 1.000" then the DRO will show 1.000", the only time this will be different is if you are using compensation of some kind.

Backlash compensation is applied on the start of the move and is not shown on the DRO's

Even on a servo system Mach has no idea if the mechanics are moving.  It just counts pulses out.

What is in your start up line on the config page?

Graham.

1803

General Mach Discussion / Re: Changing tool offsets

« on: December 15, 2007, 01:08:32 PM »

The proper way to set multiple tools is like this :-

Get into the habit of setting G54 or G55 or G56 etc.

The benefit of this is not realised until you try it. The biggest benefit is that the datum of the job can be moved with ease.

Set G54 X and Y axis to datum point on job.

Your Z axis datum is set by tool 1 or your datum tool e.g. a probe.

Touch your datum tool on top of job.

Set G54 Z to the reading in the Z axis machine dro

Zero out on top of job with above tool.

Load next tool.

Your tool offset is the difference in length between the datum tool and this tool.

Touch on same face, the reading in the Z dro is the offset of this tool, enter this in the offset table for this tool.

Repeat above line for all tools.

If more material has to be removed from face of job then the machine Z datum needs to be moved down. e.g. increase the value of Z in G54 fixture offset

Note

if your datum tool is not the first cutting tool then tool 1 will have an offset, if tool 1 is your datum tool then it will have an offset of zero.

Graham.

1804

General Mach Discussion / Re: Changing tool offsets

« on: December 15, 2007, 07:59:37 AM »

Normally you would reset the Z datum and leave the tool offsets the alone.

Graham.

1805

G-Code, CAD, and CAM discussions / Re: G54-G59 Work offsets

« on: December 14, 2007, 06:12:35 AM »

That about sums it up.

G54 is set every time the fixture is set up because the fixture may be in a different place on the machine.

G52's are hard coded into the program as the parts on the fixture should/will be in the same place every time relative to the G54.

Graham.

1806

SmoothStepper USB / Re: Beta Testing Reports

« on: December 13, 2007, 09:13:31 AM »

Just got mine today, I will be playing nice tonight.

Graham.

1807

G-Code, CAD, and CAM discussions / Re: G54-G59 Work offsets

« on: December 13, 2007, 08:39:01 AM »

Hi Chris,

If you have a jig with 6 identical parts located on it, you do not want to have to set 6 lots of offsets.

G54 to G59 are global fixture offsets, that is, you can set each one up with a different fixture datum then when you use that fixture again you have to set all six datums again.  We do not want to do that we want to set one datum and all the other parts are in known locations so we can use 1 global and any number of local datums in this case 6.

To program each location on the fixture you use G52, this is a local datum that is relative to the fixture offset in use.

So, we set the fixture datum using G54, then in our program we have G52's that represent the positions of the individual parts on the fixture, these are hard coded into the program as they never change.

This program would drill the 2 holes in each part in the diagram below. Every time we would use this fixture we would set G54 X0 Y0 at the bottom left side and the Z on top of the job and the program sets all the local datums as it needs them.

Before anybody tells me :-

If I wanted to make things even better I could use incremental or absolute subs or macros to make the program even smaller, but lets start simple.

%
(USE FIXTURE OFFSET G54)

G21 G40
T1 M6
G54 G00 G90 G43 X0 Y0 Z25. H1 S750 M3 (MOVE TO FIXTURE DATUM)
(FIXTURE LOCATION 1)
G52 X20. Y20.                                        (SET FIRST LOCAL DATUM)
G00 X-5. Y0                                          (MOVE TO FIRST HOLE)
G81 Z-10. R1. F125.                                 (DRILL FIRST HOLE)
X5.                                                       (DRILL SECOND HOLE)
G80                                                        (CANCEL DRILLING)
G52 X0 Y0                                               (CANCEL LOCAL DATUM)

(FIXTURE LOCATION 2)
G52 X50. Y20.
G00 X-5. Y0
G81 Z-10. R1. F125.
X5.
G80
G52 X0 Y0

(FIXTURE LOCATION 3)
G52 X80. Y20.
G00 X-5. Y0
G81 Z-10. R1. F125.
X5.
G80
G52 X0 Y0

(FIXTURE LOCATION 4)
G52 X80. Y50.
G00 X5. Y0
G81 Z-10. R1. F125.
X-5.
G80
G52 X0 Y0

(FIXTURE LOCATION 5)
G52 X50. Y50.
G00 X5. Y0
G81 Z-10. R1. F125.
X-5.
G80
G52 X0 Y0

(FIXTURE LOCATION 6)
G52 X20. Y50.
G00 X5. Y0
G81 Z-10. R1. F125.
X-5.
G80
G52 X0 Y0
M5
M30
%

I hope this makes things a bit clearer.

Graham.

1808

G-Code, CAD, and CAM discussions / Re: G54-G59 Work offsets

« on: December 12, 2007, 10:26:54 AM »

G52 X0 Y0 Z0 A0 B0 C0

Cancels any G52 local offset you have set.

If you do not cancel them you will get accumulations of offset and things like go to tool change go to the wrong place. You do NOT want that.

Graham.

1809

G-Code, CAD, and CAM discussions / Re: G54-G59 Work offsets

« on: December 12, 2007, 10:00:17 AM »

OK, like this.

G00 G43 G40.1 G17 G80 G50 G90
G20
(Deep Drill )
G54 (set fixture offset before any moves)
M6 T1
G43 H1
M03 S800

G00 X0.6250 Y-0.7500
Z.2655
G73 Z-0.4595 R0.0 Q0.05 F2.0
X4.8150 Y-0.75
G80

G52 X-5.(SECOND PART)
G00 X0.6250 Y-0.7500
G73 Z-0.4595 R0.0 Q0.05 F2.0
X4.8150 Y-0.75
G80
G52 X0 (you must always cancel)
G00 Z1. M9
M5
M30

Graham.

1810

G-Code, CAD, and CAM discussions / Re: G54-G59 Work offsets

« on: December 12, 2007, 06:52:21 AM »

Hi Chris,

G54 to 59 are machine datums, you use them to set fixture xyz zero points.  To do multiple parts on a fixture you use local datums G52 :-

G00 G43 G40.1 G17 G80 G50 G90
G20
(Deep Drill )
G54 (set fixture offset before any moves)
M6 T1
G43 H1
M03 S800
G00 Z0.2655
X0.6250 Y-0.7500
G73 Z-0.4595 R0.0 Q0.05 F2.0
G80
G00 Z0.2655
G52 X-5. (set local datum offset)
X4.8150 Y-0.7500
G73 Z-0.4595 R0.0 Q0.05 F2.0
G80
G52 X0 (you must always cancel)
G00 Z0.2655
G00 Z1
M5 M9
M30

Graham.