Can Fusion do this?

[markabra123]

Can I command Fusion within the manufacture environment to go to a specific point and simply stop (don't drill, don't cut, just stop)?

Why you ask? The short answer is that I am doing 2 sided flip milling with alignment dowel pins and I want to (after completing side 1) have the spindle move to the center of a pin hole and stop... so that I can - within my machine control software (Mach3) - identify that point within the machine coordinate system -> write that down -> and then flip my stock & create a new setup for side 2 - entering the written down machine coordinates - moving my spindle to that precise point -> and then resetting that point to zero... so that the machine coordinate system and the work coordinate system (within fusion) are now shared for side 2.

[seth.madore]

Technically, yes, sort of?
Method one:

Manual NC where you hardcode in what you want to do:
G0 G54 X0 Y0

M0 (FLIP PART)

Other method would be to use the "Custom" Drill cycle and modify your post to do nothing more than go to that drill point position and stop.

[programming2C78B]

Just fyi if you know the hole position from your g54, you can also just jog there and reset the axis. You can even have the code just set g55 as g54+(hole position) so it's all automatic. 

[markabra123]

Hey Seth, 

Thanks so much for helping out with this! I wonder if you might help me to fully solve this problem with some finished g-code…

As a preface, I’m new to CAD/CAM, fusion, working with a CNC machine and controller software. Until today, I have never looked at g-code before. So the more you assume I don’t know, probably the better 🙂 

That being said, after thinking about what you said & looking at some g-code examples, it doesn’t seem too hard and I think I”ve moved quite a way in the right direction! But still have a little bit left to go to get to the finish line...

In your initial response to my post you said:

"Other method would be to use the "Custom" Drill cycle and modify your post to do nothing more than go to that drill point position and stop."

I’ve posted g-code for a “custom drill cycle” as you suggested. I’ve pasted it below. You suggest that I “modify the post so that the spindle does nothing more than go to the drill point position and stop” Since I have no experience with g-code at all (before today 🙂 I don’t know how to make that modification. Might you be able to help me modify the code below so that the spindle moves to the drill point position & stops and stays there (and so that any code commands that are needed to make the post complete are included)?

(SIDE 1 CUSTOM DRILL CYCLE)

(T1 D=0.0569 CR=0.0312 TAPER=5.4DEG - ZMIN=0. - TAPERED MILL)

G90 G94 G91.1 G40 G49 G17

G20

(-ATTENTION- PROPERTY SAFE RETRACTS IS SET TO CLEARANCE HEIGHT.)

(ENSURE THE CLEARANCE HEIGHT WILL CLEAR THE PART AND OR FIXTURES.)

(RAISE THE Z-AXIS TO A SAFE HEIGHT BEFORE STARTING THE PROGRAM.)

(DRILL1)

T1 M6

S24000 M3

G17 G90 G94

G54

M8

G0 X0.4214 Y1.125

G43 Z0.6 H1

G0 Z0.2

!Error: Failed to post data. See log for details.

Don’t know if is helpful to you at all, but below is g-code for a non custom drill cycle at the same drill point with no error messages and finished code. (of course I can’t use this b/c it will drill - which I don’t want)

(SIDE 1 - REGULAR RAPID OUT DRILLING)

(T1 D=0.0569 CR=0.0312 TAPER=5.4DEG - ZMIN=0. - TAPERED MILL)

G90 G94 G91.1 G40 G49 G17

G20

(-ATTENTION- PROPERTY SAFE RETRACTS IS SET TO CLEARANCE HEIGHT.)

(ENSURE THE CLEARANCE HEIGHT WILL CLEAR THE PART AND OR FIXTURES.)

(RAISE THE Z-AXIS TO A SAFE HEIGHT BEFORE STARTING THE PROGRAM.)

(DRILL1)

T1 M6

S24000 M3

G17 G90 G94

G54

M8

G0 X0.4214 Y1.125

G43 Z0.6 H1

G0 Z0.2

G98 G81 X0.4214 Y1.125 Z0. R0.2 F33.

G80

Z0.6

M9

M5

M30

[programming2C78B · Accepted solution]

The simplest thing is to use this as a passthrough at the very end of your program. You can go more automated and have it copy your current g54 position into a g55 for your op 2, but I feel like thats above you day1 skill level for now. 

(go to position)

T1 M6

G17 G90 G94

G54

G0 X0.4214 Y1.125

M00

(TAKE NOTE OF MACHINE POSITION)
(AND RESET G54 AFTER PROGRAM FINISHES)

M30

[markabra123]

Wow, thanks so much for that. You've saved me many hours of digging! 

Am totally interested in the fully automated way, but think I"ll leave that for another day.