[aseylys]

Hi again guys,

I'm trying to configure my mill. I've written a simple gcode to make 2 lines, each 50 mm, having a space between them. The line part is working, the space between is where I'm failing. It's supposed to go 5 mm up to not be in the material and then start with the second line. It's not doing that, if anything it's getting lower. Can anyone help with figuring out the problem with the code?

( Untitled 2/5/2014 8:40:23 PM )
( T0 : 0.0 )
G21 G90 G64 G40
G0 Z3.0
( T0 : 0.0 )
T0 M6
( Engrave1 )
G17
M3 S1000
G0 X-2.0 Y-11.5
G0 Z1.0
G1 F300.0 Z-0.1
G1 F800.0 Y38.5
G0 Z3.0
G0 X6.75
G0 Z1.0
G1 F300.0 Z-0.1
G1 F800.0 Y-11.5
G0 Z3.0
M5
M30

[cyclestart]

The code is good.

a) tool is pulling out of holder
or
b) the machine is not going to commanded z position

[urbnsr]

Scanning the code looks OK. If it matters, your code is pulling up your Z 3mm, not 5mm. If the other axis are staying accurate, I would look at a mechanical issue with your Z axis. If it's progressively getting off, I would wonder about a tool offset/compensation issue.

Paul

[aseylys]

Dang, I was hoping it was the code. Alright I'll check the machine out. Thanks guys.

[Heavy_Metal]

Hi,

Try something like this.
Why G64 ??

%
G54 G17 G40 G80 G90
G49 ( Tool Lenght Compensation Cancel )
G0 G91 G28 Z0
S1000 M3
G0 X10. Y10.
G0 G43 Z3.0 H1 ( G43 + H1 = Tool Lenght Compensation for T1 )
( T1 = Tool in pot 1 )
T1 M6
( Engrave1 )
G0 X-2.0 Y-11.5
G0 Z1.0
G1 F300.0 Z-0.1
G1 F800.0 Y38.5
G0 Z3.0
G0 X6.75
G0 Z1.0
G1 F300.0 Z-0.1
G1 F800.0 Y-11.5
G0 Z3.0
M5
G0 G28 G91 Z0
M30
%

Regards,
Heavy_Metal.

[chucker]

maybe your part is not flat

[urbnsr]

Why G64 ??

Yeah?
It shouldn't hurt this issue though, but I believe a G64 without a 'P' value = G64 P0 which is the same as G61 (Exact Path Mode).

[cyclestart]

I shortened up your code and ran it on my very basic router

G17 G21 G90 G54 G49
G0 Z3.0
G0 X-2.0 Y-11.5
G0 Z1.0
G1 F300.0 Z-0.1
G1 F800.0 Y38.5
G0 Z3.0
G0 X6.75
G0 Z1.0
G1 F300.0 Z-0.1
G1 F800.0 Y-11.5
G0 Z3.0
M2

If you have a toolchanger the M06 line will have to be added. If you have software spindle control the M03 line will have to be added.

What I did in order:
Edited your file
Fired up linuxcnc
homed the machine
moved the machine to a random x-y location
moved the tip of the tool to the top of an imaginary piece of stock
touched off all axis, chose relative 0.0 (the default option), G54 coordinate system (the default option)
single stepped first run

I also ran your original file with no problems.

If your machine runs fine up until it reaches Y38.5 and then gags on the G0 Z3 retract move it may help to reduce acceleration on Z axis.

I like the part not being flat comment. Someone thinks outside the box

[cyclestart]

The question regarding G64 got me into a bit of reading.
When a session of linuxcnc is started (this thread was moved from the linuxcnc forum) G64 is active by default. It remains active unless G61 is explicitly called
in MDI or another program. If G64 or G61 is called it is persistant for that session, ie: it remains active for that linuxcnc session until the other commandi is
called.

Is G64 with no P specified the same as G61 (exact stop) ?
The documentation states:

G64 and G64 P0 tell the planner to sacrifice path following accuracy in order to keep the feed rate up. This is necessary for some types of material or tooling where exact stops are harmful, and can work great as long as the programmer is careful to keep in mind that the tool’s path will be somewhat more curvy than the program specifies. When using G0 (rapid) moves with G64 use caution on clearance moves and allow enough distance to clear obstacles based on the acceleration capabilities of your machine.

Since P0 suggests no deviation from path the above seems a bit of a contradiction. The next block in the documentation may offer a hint:

Beware that a specification of G64 P0 has the same effect as G64 alone (above), which is necessary for backward compatibility for old G Code programs.

The quotes come from this page:
Important User Concepts

Anyway that's how I read it.

Aseylys
Ignore my bad advice to mess with the machine settings for now, if the machine was running properly before it's best to find out what has changed. You could try experimenting with G61 or retacting at a G1 feed move. I'm guessing your machine is running steppers.