Messages

571

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

572

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

573

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.

574

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

575

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

« on: July 19, 2020, 09:49:46 AM »

Turn CV mode off and run it again, then turn it on and slow down the feed into the corners, its the feed verses CV mode that is doing this.

576

Mach4 General Discussion / Re: The scale when cutting is off.

« on: July 15, 2020, 10:22:54 AM »

Motor Settings:
  counts/unit; 40960.0
  units/minute; 35
  units/sec^2; 0.49

My motor has 200 steps (1.8deg.) each and has a 128 microsteps.

My math: (200*128)/(0.625)=40960.0 counts/unit

For one rev of the motor your axis should move .625", Put a mark on the end of the motor shaft and on to the case and enter the following code in MDI:-

G20 G01 G91 X0.625 F2.

If the machine moves .625" and the lines on the motor are in line its not the machine.

577

G-Code, CAD, and CAM discussions / Re: Randomly stopping on G4 P0.1 Command

« on: July 15, 2020, 10:05:46 AM »

G4 is a delay, this can be in seconds or microseconds depending on the setting in the mach3 config screen.  I think Mach4 uses P for microseconds and X for seconds

578

CS-Lab / Re: CSMIO/P-M

« on: July 15, 2020, 09:56:55 AM »

I have had a very similar experience with them, my CSMIO-IP/A ran perfect with Mach3 so I purchased a new IP/A to run Mach4 and the thing drove me crazy.  nothing was stable, things did not work, probing I just dare not use.

When I contacted CSLabs the attitude stunk, its all my fault for some reason or another.

It went on eBay and the machine is now on a ESS and working great, luckily the drives could do 0-10v analogue or step and direction.

No more CSLabs for me.

579

General Mach Discussion / Re: Totally Lost with Offsets.

« on: July 13, 2020, 07:56:55 PM »

One line at the start of your g-code will do it and one at the end.

O0001
G21 G40 G00 G99
G54
G52 X-88. Y-63.
G00 ETC...

(MORE LINES)

G52 X0 Y0
M30

580

General Mach Discussion / Re: Puzzled :(

« on: July 13, 2020, 07:48:40 PM »

Broken or missing ground wire, pc and machine not grounded together, or power supply failing on machine.  All candidates for random steps.