G0 Z-10 at the start of the job ... Why ? I though this was the end of the code / job When I run the post process (Fusion 360) it always puts this at the start of the job , so the if I set zero for the z axis imm above the work piece the first instruction is to push the tool into the work piece ..... got me stumped and the it seems to want to position the tool at the start of the job and raise it 16 and the 3 .....mm (This file contains the following operations: ) (1 : Pocket1) ( Work Coordinate System : G54) ( Tool 4: Flat End Mill 3 Flutes, Diam = 4mm, Len = 25.00mm) ( Spindle : RPM = 18000) ( Machining time : 36 min 22 sec) G90 G94 G17 G21 (Operation 1 of 1 : Pocket1) G54 G53 G0 Z-10 S18000 M3 G4 P15. G0 X-211.067 Y405.539 Z16 Z3 G1 X-211.067 Y405.539 Z2.45 F500 S10000 G1 X-211.052 Y405.549 Z2.329 X-211.005 Y405.577 Z2.219
What controller are you using? Are you homing the machine on power on? It's actually G53 G0 Z-10 - ie; MACHINE co-ordinates, 10 mm below the home position on a typical grbl machine. Alex.
If you are homing your machine, then the only time it will hit your stock is if -10 from Z home isnt enough clearance. I have a few jobs where I dont have 10mm of clearance so I have to adjust it down to -4mm.
So if I position the tool to say 1 mm above the work piece and then set all axis to zero then I must have to raise the tool a further 10m or when the code executes its going to move the tool down into the work piece ,,,, or is the mistake I am making that I move the axis XY&Z to the start point and I am then setting ZERO ....
You can set 0 wherever you want. That doesnt mater nor does is play any role in where the first Z move will be. Where you set 0 is called your Work Coordinates. The Fusion post uses Machine Coordinates for the first Z move and the last Z move. In simple terms, Machine Coordinates are where your limit switches are. What the Fusion post is doing is moving Z to -10mm from your limit switch. You can think of this as "Move the spindle up as far as it will go, but with a 10mm buffer so that it doesnt trigger your limit switch". So with that knowledge, here's two scenarios. 1. The top of your stock is 25mm below the tip of your tool when Z is at max height. You have Z -10mm in your fusion post processor settings. The first Z move will put the tip of the bit 15mm above your stock (25mm - 10mm = 15mm). 2 The top of your stock is 5mm below the tip of your tool when Z is at max height. You have Z -10mm in your fusion post processor settings. The first Z move will put the tip of the bit 5mm INTO your stock (5mm - 10mm = -5mm). To avoid this, set Z to -4mm in your post processor settings. This will result in the first Z move being 1mm above your stock (5mm - 4mm = 1mm).
The G53 move is a safety move, an industry standard for preventing expensive crashes. Z home is the top of Z travel, so moving to Z-10 raises the bit as far from the work as possible before moving to X0 Y0 It does not have to be -10, it can be -1 if that is enough to avoid triggering your limit switch. (with GRBL controllers is has to always be a negative number) This is an editable option in the post options dialog. If you hover your mouse over each option in turn, the help will popup and help you if you read it. (read the help, knowledge is power!) In the image below the green text lines are the options. Green means it is set to default, blue means it has been changed (by you). Changes will be remembered by Fusion.
I just wanted to say to those that replied to my post that it has inspired me to do more challenging CNC projects knowing that there is friendly help and advice to help me when I get stuck .... which I am sure I will Thank you
I've been having this problem today and it's driving me a little crazy! I have a RatRig Killer Bee with a Black Box controller. I think I might have worked out whats going on though.... if I'm correct G53 G0 Z-10 tells the machine to go to minus 10mm from your limit switch, G53 being the homed positions for the machine and not the work piece. So does this mean if I haven't homed my machine lately, yet zeroed the work piece it might not know where -10mm from home is so just go from some other place... maybe the position it's at? I haven't homed my machine today, I've just been setting zero for the work piece, I'm guessing this could be the problem?
Yes, ALWAYS home the machine after switching on, resetting the controller etc - it's the only way to establish the MACHINE co-ordinate system correctly. The blackbox will set the home position wherever it is when you switch on, so you need to home it so it knows where you put your limit switches. And if you are using soft limits and set your workspace (max dimensions for each axis) it will "know" where all the corners and edges of your machine are. Alex.
Thanks for confirming @Alex Chambers I've just been out to the workshop to confirm this and all good now. The joys of learning
