G53 G0 Z0.
there is maybe somthing we can change
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
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
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.
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.
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
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.
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 .