Messages

561

Mach4 General Discussion / Re: spindle dwell before run

« on: July 28, 2020, 09:22:02 PM »

Check the spindle tab on the config screen, you may need to scroll left to see it.

562

Mach4 General Discussion / Re: Z zero

« on: July 27, 2020, 08:12:42 AM »

Check your tool offsets, if you are only using 1 tool then you do not need a height value in the offset for that tool.

563

General Mach Discussion / Re: Cutting a Circle - Figures don't add up!

« on: July 25, 2020, 07:14:34 PM »

Why do you want to re-invent the wheel, why not use the built in wizards, click on the wizards menu and you have all the included ones in a window.

564

Mach4 General Discussion / Re: bad allocation error

« on: July 24, 2020, 04:51:59 PM »

What version are you using

565

General Mach Discussion / Re: Cutting a Circle - Figures don't add up!

« on: July 22, 2020, 05:23:56 PM »

You do not have the datum set right.

Move your pencil to a clear space.

Jog down until the pencil touches the paper.

Click Zero X to the left of the X DRO on the program screen.

Click Zero Y

Click Zero Z

Jog clear  in Z

Load and run this code

%
G21 G40 G00 G99 G17

N1 (8MM DIA END MILL)
G54 G00 G90 X0 Y0 Z5. S3000 M3
Z1.
G01 Z0 F100.
X50. F500.
G02 I-50.
G00 X0 Y0 Z5.
M30
%

You should get a 100mm circle give or take the line width of the pencil.

If not something is wrong in your settings

566

General Mach Discussion / Re: Cutting a Circle - Figures don't add up!

« on: July 22, 2020, 01:44:19 PM »

A simple circle with the machine zero on the centre line of the circle and on the top face would be something like this :-

%
G21 G40 G00 G99 G17

N1 (8MM DIA END MILL)
G54 G00 G90 G43 X0 Y0 Z5. H3 S8000 M3
Z1.
G01 Z-52. F100.
X44.375 F200.
G02 I-44.375
G01 Z-54.
G02 I-44.375
G00 X0 Y0
Z5.
M30
%

For helical :-

%
G21 G40 G00 G99 G17

N1 (8MM DIA END MILL)
G54 G00 G90 G43 X0 Y0 Z5. H3 S8000 M3
Z1.
G01 Z-52. F100.
X44.375 F200.
G02 I-44.375 Z-54.
I-44.375 Z-56.
G00 X0 Y0
Z5.
M30
%

567

General Mach Discussion / Re: setting the exact home for 2 different files

« on: July 21, 2020, 07:23:33 PM »

Touch the first tool on the top face of the job.

Click Zero Z button.

Then enter 1 in the 'Tool' DRO in the Tool Information box.

Then enter its diameter in the Dia DRO

Followed by the length, set this to zero

Put the second tool in the spindle.

Touch it on the top of the job

Then enter 2 in the 'Tool' DRO in the Tool Information box.

Then its diameter in the Dia DRO

Then set the length to the value shown in the Z axis DRO, this is the difference in length between tool 1 and tool 2, so tool 2 has and offset in length that Mach3 compensates for.

-----------

Your first program should have G43 H1 on the first Z rapid line

The second program should have G43 H2

e.g.

O0001 (FIRST PROGRAM)

G21 G40 G00 G99 G17

G54 G00 G90 G43 X0 Y0
G43 H1 Z10.
S1000 M3
etc...
M30

O0002 (2ND PROGRAM)

G21 G40 G00 G99 G17

G54 G00 G90 G43 X0 Y0
G43 H2 Z10.
S1000 M3
etc...
M30

Or you could join the 2 programs together.

O0001 (FIRST & 2ND PROGRAM)

G21 G40 G00 G99 G17

N1 (TOOL 1)
G54 G00 G90 G43 X0 Y0
G43 H1 Z10.
S1000 M3
etc...
M0

(CHANGE TO 2ND TOOL)

N2 (TOOL 2)
G54 G00 G90 G43 X0 Y0
G43 H2 Z10.
S1000 M3
etc...
M30

You can also use the Offset screen to set tools, bottom right of screen

568

General Mach Discussion / Re: Simple radius cutting - isn't !

« on: July 21, 2020, 06:54:22 PM »

G41 P2.49 X20. Y-5. F200.

Try changing this line to this

569

General Mach Discussion / Re: Simple radius cutting - isn't !

« on: July 19, 2020, 06:56:43 PM »

If you look at the code sample you can see how the start point has to be set to allow the tangent move to the work, its all based on the rad of the cutter the I words are incremental distances in the X axis the J is the same but in the Y axis.

So on a G03 line the X & Y is the absolute end point and the I & J are the incremental distance to the centre of the radius in X & Y or if not included its zero.

If you do not have CAM have a look at CAMBAM.

570

General Mach Discussion / Re: Simple radius cutting - isn't !

« on: July 19, 2020, 04:03:37 PM »

If you want sharp corners you have to turn off CV G61, this puts the control into exact stop mode.

G64 will turn CV back on but the faster that the cutter is entering the corner the bigger the radius will be to allow Mach3 to get around the corner without slowing the cut.

On some CAM systems you can tell it to output a G61 if the corner is less than a given angle or you can tell it to slow down on the corner and then go back to the programmed feed rate.

Using G61 all the time causes jerky movement on short moves so CV and slowing in tight corners is the best way to go.

-------------------------

Tool compensation is a way to allow for tool wear or to allow you to use a smaller tool than the code was originally programmed for.  It is not a quick fix to bad code.

You have to pre-plan for things to work right, select your tool, allowing for the smallest internal radius to be cut, the tool needs to be smaller than this.

If you wish to machine a square pocket of say 50 x 50mm with internal rads of 3mm then a 5mm cutter is a good choice. The datum is 0/0 in the centre of the square.

Pocket the hole leaving say 0.5mm under size for finishing.

Then you have to lead in to start your finish cut, this is a line followed by a radius that finishes tangent to the following line of cut, the rest of the profile is then machined and a lead out is performed that again is a rad followed by a line.

The finish profile is programmed as if the tool had a zero diameter (on the centre line) and the G41/G42 then allows for the tool diameter with the P word (cutter diameter) or D word (diameter offset number) on entry, which of G41/G42 is to be used depends on which side of the line you are on and the direction of travel, this example we are on the inside/left of the line and moving counter clockwise so its G41, G40 then cancels the compensation on the lead out.

The finish profile code would look something like this:-

O0001 (G41_5MM_ENDMILL_50X50_FINISH_PASS)

G21 G40 G80 G17

N1 (FINISH INNER PROFILE - FLAT  5MM)
T2 M6
G54 G00 G90 G43 X17.5 Y-2.5 Z25. S2000 M3
Z1.
G01 Z-2. F100.
G41 P2.49 X20. Y-5. F200.
G03 X25. Y0. I0. J5.
G01 Y22.
G03 X22. Y25. I-3.
G01 X-22.
G03 X-25. Y22. J-3.
G01 Y-22.
G03 X-22. Y-25. I3.
G01 X22.
G03 X25. Y-22. J3.
G01 Y0.
G03 X20. Y5. I-5.
G01 G40 X17.5 Y2.5
G00 Z25.
G91 G28 Y0 Z0 M5
M30