G53 G0 Z0.

can you show us your ini file
there is maybe somthing we can change
[AXIS_2]
# Zachse
TYPE = LINEAR
HOME = -5.0
MAX_VELOCITY = 40.0
BACKLASH = 0.03
MAX_ACCELERATION = 80.0
STEPGEN_MAXACCEL = 120.0
SCALE = 100.0
FERROR = 1
MIN_FERROR = .25
MIN_LIMIT = -65.0
MAX_LIMIT = 1.0
HOME_OFFSET = 0.000000
HOME_SEARCH_VEL = 3.000000
HOME_LATCH_VEL = 3.000000
HOME_FINAL_VEL = 5.0
HOME_SEQUENCE = 0

here is ini file :

0

[AXIS_2]
TYPE = LINEAR
HOME = 0.0
MAX_VELOCITY = 100.0
MAX_ACCELERATION = 750.0
STEPGEN_MAXACCEL = 937.5
SCALE = 80.0
FERROR = 1
MIN_FERROR = .25
MIN_LIMIT = -0.001
MAX_LIMIT = 200.0
HOME_OFFSET = 0.0

flylowgofastturnleft wrote: Hello,

So I can just remove G53 lines, but perhaps there is a better way to proceed ?

Could you give me a post or a link to the good way to take origins ?

I think I miss something

Thanks

Do you home your machine when you power up? If you do then leave the G53 there.

It all depends on how you home your machine.

If you move to the bed of your machine and home and touchoff tool to table then G53 Z0 will dive through your workpiece.

You could before touching off, move your Z to the highest point and home Z there, then touchoff on the table, then G53 Z0 will move the Z to where you homed it.

You have to remember where you touchoff Z will be G54 Z0 which should not be the same place as G53 Z0 is. G54 is an offset to G53 and G53 X0 Y0 Z0 is suppose to be the same place all the time.

That is basic with no special circumstances.

hello,

If I understand, Z axis need to work in negatives value ?

This is the opposite with fusion 360.

How to have a good file from Fusion ?

You did not tell, how you home Z. If it is possible for your machine to change G53 Z0(machine Z0) to the most faraway position from working area, if this action doesn`t affect machine safety. After all Z moves are Z-
You can try change ini entrys,

MIN_LIMIT = -0.001 to -200.001
MAX_LIMIT = 200.0 to 0.001
HOME_OFFSET = 0.0 to -200

flylowgofastturnleft wrote: hello,

If I understand, Z axis need to work in negatives value ?

This is the opposite with fusion 360.

How to have a good file from Fusion ?

Where you set the machine coordinates Z0 (G53) has nothing to do with the work coordinate (G54) settings where your G-code actually does its moves.
You should set the home position to the top of travel so all G53 moves are Z-, then touch off the G54 work coordinates to set Z0 to be your work or table surface, as needed by your G-code from Fusion. Doing that will give you the movements you need. (It sounds like you really are not getting the difference between "machine" and "work" coordinates and how they are used. It also sounds like you are using homing like touching off, these are not the same thing and should not be used interchangeably. You home once at start up, you touch off when ever you change tools, or setups.

so you do not autohome the mashine at all
just you press every axis and REFERENCE at the point where it stands

THEN you need to DELETE *var and *.var.bak
in the Mashine folder all the time
as it holds last Mashine position and Parameters
that come from Fusion360

ADVICE GET yoi some switches
CHERRY switch 5pices 4USD
or go the real way use LJ12A3 BX version NPN NO

and get your mashine automated to a Mashine Reference point

I know this is a late reply, but F360 has a Setup/Machine/Edit section (was a Preview option, looks standard now). Set up a Machine Configuration and change the Kinematics/Z Linear/Home position to the desired machine position for G53.
In my case, I pick up my Z max with a limit switch and have 95mm of travel. I set home to be 90mm.

Post processed code will have the correct:
N20 G53 G0 Z90.

Prior to adding the machine config, I was mucking around with the post processor scripting or trying to remember to delete the G53 lines. This was a major headache and I had some crashes. Since I used the F360 machine config I have had no problems with the G53.

Hi.

I have only one limit switch too on all axis. On Z my switch is on an offset of -2 and home is 0. Travel is alway in minus range. Thats quite different to the US practice where 0 is on the bottom of the workpiece. I use the top of the workpiece and the bottom left edge .

Best,
Udo

flylowgofastturnleft wrote:

hello,

If I understand, Z axis need to work in negatives value ?

This is the opposite with fusion 360.

How to have a good file from Fusion ?
 

its not opposite with Fusion. Up direction is positive in fusion. If you increase the Z value you fly, if you decrease it, you sink.
Think intuitively, up is +, right is +, depth is + and their respective opposite axis are negative direction.

G53 Z0 is at the upper limit of the spindle because it is safe location and a safe number.
You can very well change that value to be something like 200 instead of 0 from the ini file. but then 0 will be on your table and when you have long endmills, entering G0 G53 Z0 means goodbye endmill. But when G53 Z0 is topmost which is the convention, it doesnt change, safe, easier to remember than 200

you'll use g54 99% of the time. You need G53 for stuff like safe z retracts, toolchanges or to park your spindle when job is finished. So these moves will not be affected by where you zero your tool and workpiece.

Btw its possibly not the reason why linuxcnc is not starting to cut.