开云体育

Hi
the g28.1 does not work correctly. If you set the z axis to
anything but 0, do a zero all and try a g28.1 it does not set to 0.
It seems to be related to the extrema readings being incorrect after
a zero all. I am using rc10
Todd

Todd:

Sorry about that , I will check the code again on G28.1

The extremea seems to work for me. Remember the extrema numbers are in
machine absolute coordinates. This means if you jog to X10, then zero, when
loading the file, the interpreter will see all movements being from your
zero, so the extrema, which lists the machine coordinates max and min, will
have 10 added to min and to max. This makes the number appear to change, but
they should as the actual machine coordinates will change during that run.
Hitting regen after zero'ing will display the new extrema. Its easy this
way to see if you will go over your limits. If you have a negative number in
any min, you will pass the limits of your machine. If you have a max larger
than your table size, the same will occur on the other side.

I will let you know on the G28.1.
Thanks,
Art
www.artofcnc.ca

Todd:

I think what your seeing is the zero ( or whatever you have in the
corrections page under home switch position) being set into the DRO for that
axis, MINUS whatever offset you have active. When you zero all or type a
number in an axis, you are executing a g92. For example, if you are at a z
of 10, and zero all, then you have set a G92Z0 into the system, which will
give you a z of 0. Now, when you command the G28.1Z0 , the Z will home, set
itself to zero and promptly display -10.0 as you have a G92 set to 10 for
the Z axis. Typing a G92.1 to remove the G92 offset system will now display
zero.
If you have a home switch setting of 5 on the corrections tab and hit
G28.1z0, then the Z will have 5 put in it when it comes off the switch,
MINUS 10 which is still in the G92 registers. You can see this in the Axis
Offset DRO's on the diags page. Each time you "zero", you are really only
changeing the axis offset to get a zero readout. G92.1 will undo zeroing in
this way. By not using the G92.1, the G28.1 can be used as a verify
proceedure. If you zero at a z of 15 , for example, then perform a G28.1z1,
followed by a g0z0, you should end up where you started. In other words, the
DRO readout after a g28.1 will be the distance from where you had your zero
last set.

This is a mach2 thing, where all coordinate systems are respected and
reversable. Try putting a
G28.1z1 G92.1 as your control line. It should give you the right reading at
that point. (0.00) This is different than Mach1 which did not respect the
coordinate systems properly.

This may seem more complex, but in reality it makes better sense. After
all, you can't really "zero" an axis, the interpreter MUST know where it is
in relation to the home switches, so it does so by keeping track of the G92
offsets and the origin offsets, and the tool offsets. All three go into
making up the DRO reading depending on your DRO mode. This is kinda related
to your extremae question.

I know this is confusing, so let me know if I explained it badly.
Thanks,
Art
www.artofcnc.ca

--- In mach1mach2cnc@..., Art <fenerty@a...> wrote:

Todd:

I think what your seeing is the zero ( or whatever you have in the
corrections page under home switch position) being set into the DRO

for that
snip-

Hi Art-

thanks for the in depth info, I think my problem is I am using the
wrong command for zeroing. What command lets me load a file, turn on
my cnc table, jog to the position that I want for 0,0,0 , and will
make the current position 0,0,0 with no offsets, no home switches,
g92's g28's, no extrema offsets, no nothing just plain old, like I
just turned on Mach2, 0,0,0.
Thanks
Todd

Well, the way I do it is load the program, move the table to where I want
0,0,0 to be and click on the "Ref All ctrl A" button to establish that at
0,0,0 Seems to work for me, there may be other ways but this seems to work.
There are no offsets, no home switches, no g92's g28's, no extrema offsets,
no nothing just plain old, like I just turned on Mach2, 0,0,0.

John Guenther
'Ye Olde Pen Maker'
Sterling, Virginia

Todd:

Just turn off the home switches, select Auto-Zero in the Logic settings,
and when you want to "zero" your machine coordinates, just hit the "ref"
button. It will zero on the spot because you have no home switches.

But if you do that, the G28.1 will not work. The only reason a G28.1
works is because it knows where "true" zero is at.So if you wish to use
G28.1 then you have to have a stored referance to true zero. The way your
zeroing is fine, but you have to understand the zero CAN be undone only at
your command. G93.1 . I can't have the G28.1 remove the offsets
automatically, because that would screw the verification proceedures with
Verify and such. It would probaly be easir to simply code G28.1X1G92.3 when
ever you use G28.1, then the zero acts the way you expect.

Thanks,
Art
www.artofcnc.ca

--- In mach1mach2cnc@..., Art <fenerty@a...> wrote:

Todd:

Just turn off the home switches, select Auto-Zero in the Logic

settings,

and when you want to "zero" your machine coordinates, just hit

the "ref"
snip-
Hi Art,
I think I found something, I ran a file 5 times with out the thc
and things worked as expected. I ran the same file twice with the thc
on and no amount of zeroing or referancing would give the correct
positions. Are the thc offsets tied into the z offsets? Is there a
way to clear the thc offsets while doing a thcoff()? Is there a way
to call the homez button from gcode or macro with out using a
g28.1z?, so it will referance from the current location without
rapiding first?
Thanks
Todd

Todd:

That explains why I couldn't find it, I was not using THC. (I never use
THC, as I have no Torch or anything...). I will activate the THC and
probably find this problem fairly quickly. It must be a bug. When the THC is
turned off, the offset for it automatically zero's. I probably missed
something and never noticed. It probably only shows in G28 moves and then
only in THC.

Thanks, I'll let you know...
Art
www.artofcnc.ca

--- In mach1mach2cnc@..., Art <fenerty@a...> wrote:

Todd:

That explains why I couldn't find it, I was not using THC. (I

never use

THC, as I have no Torch or anything...). I will activate the THC and
probably find this problem fairly quickly. It must be a bug. When

the THC is

turned off, the offset for it automatically zero's. I probably

missed

something and never noticed. It probably only shows in G28 moves

and then

only in THC.

Thanks, I'll let you know...
Art
www.artofcnc.ca

Told you!........TOM C

Todd:

I'm curious about something. Are you using an M5 prior to the g28.1?

Art
www.artofcnc.ca

--- In mach1mach2cnc@..., Art <fenerty@a...> wrote:

Todd:

I'm curious about something. Are you using an M5 prior to the

g28.1?

Art
www.artofcnc.ca

Hi-
Yes, at each pierce point I run a macro that g28.1z.1, g0z.25, m03
( torch on) , dwells, and does a thcon(). At the end of each cut
thcoff() m05, g0z1.
Todd

Thanks Todd:

I think I have it fixed. I failed to sync the engine after the THC run, so
whatever the correction was, was being added to the further trajectories. It
SHOULD be fix, but we'll see what your tests show.

Thanks,
Art
www.artofcnc.ca

Thanks!
Once we get past this last little obstacle, the thc software and
tom's control board will be working at 100%. Any Idea how long 'till
the next release so I can try it out?
Todd
--- In mach1mach2cnc@..., Art <fenerty@a...> wrote:

Thanks Todd:

I think I have it fixed. I failed to sync the engine after the THC

run, so

whatever the correction was, was being added to the further

trajectories. It

SHOULD be fix, but we'll see what your tests show.

Thanks,
Art
www.artofcnc.ca

Todd:

This weekend coming I think, or earlier, but I have a few things in the
works so I need to finish them.

Thanks,
Art
www.artofcnc.ca