PDA

View Full Version : F360 - returns to machine zero not work offset



routercnc
20-03-2017, 09:25 PM
Just tried out my first bit of gcode posted [boring out a hole] from Fusion 360, using an air cut, and it all worked well except:

1. Pressing cycle start makes the machine move to machine coords Z zero (i.e. Z home switch)

2. After cutting out the part it moved back to machine coords X, Y, Z zero (i.e all home switches)

I'm used to Vectric posting code out which moves the machine to work offset zero and safe Z (e.g. local 0,0,20), which is much more handy than having the machine march off to home somewhere over in the far corner.

The code posts out G28 (line 6, and last but 2 lines), which is moving the machine to machine zero. Here it is:
(OP2_SINGLEHOLE_6MM_0P5_300)
(0.5MM PITCH)
(T1 D=6. CR=0. - ZMIN=-20. - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21
G28 G91 Z0.
G90

(BORE2)
M5
M9
T1 M6
(6MM_2F_19S)
S12000 M3
G54
M9
G0 X9.409 Y61.753
G43 Z15. H1
Z2.
G1 Z0.6 F900.
X9.416 Y61.749 Z0.506
X9.435 Y61.739 Z0.415
X9.467 Y61.722 Z0.328
X9.51 Y61.698 Z0.247
X9.563 Y61.669 Z0.176
X9.626 Y61.634 Z0.115
X9.697 Y61.596 Z0.065
X9.773 Y61.554 Z0.029
X9.853 Y61.51 Z0.007
X9.936 Y61.465 Z0.
X10.199 Y61.321
G3 X10.878 Y61.521 R0.5
X9.122 Y62.479 Z-0.5 R1. F300.
X10.878 Y61.521 Z-1. R1.
X9.122 Y62.479 Z-1.5 R1.
X10.878 Y61.521 Z-2. R1.
X9.122 Y62.479 Z-2.5 R1.
X10.878 Y61.521 Z-3. R1.
X9.122 Y62.479 Z-3.5 R1.
X10.878 Y61.521 Z-4. R1.
X9.122 Y62.479 Z-4.5 R1.
X10.878 Y61.521 Z-5. R1.
X9.122 Y62.479 Z-5.5 R1.
X10.878 Y61.521 Z-6. R1.
X9.122 Y62.479 Z-6.5 R1.
X10.878 Y61.521 Z-7. R1.
X9.122 Y62.479 Z-7.5 R1.
X10.878 Y61.521 Z-8. R1.
X9.122 Y62.479 Z-8.5 R1.
X10.878 Y61.521 Z-9. R1.
X9.122 Y62.479 Z-9.5 R1.
X10.878 Y61.521 Z-10. R1.
X9.122 Y62.479 Z-10.5 R1.
X10.878 Y61.521 Z-11. R1.
X9.122 Y62.479 Z-11.5 R1.
X10.878 Y61.521 Z-12. R1.
X9.122 Y62.479 Z-12.5 R1.
X10.878 Y61.521 Z-13. R1.
X9.122 Y62.479 Z-13.5 R1.
X10.878 Y61.521 Z-14. R1.
X9.122 Y62.479 Z-14.5 R1.
X10.878 Y61.521 Z-15. R1.
X9.122 Y62.479 Z-15.5 R1.
X10.878 Y61.521 Z-16. R1.
X9.122 Y62.479 Z-16.5 R1.
X10.878 Y61.521 Z-17. R1.
X9.122 Y62.479 Z-17.5 R1.
X10.878 Y61.521 Z-18. R1.
X9.122 Y62.479 Z-18.5 R1.
X10.878 Y61.521 Z-19. R1.
X9.122 Y62.479 Z-19.5 R1.
X10.878 Y61.521 Z-20. R1.
X9.122 Y62.479 R1.
X10.878 Y61.521 R1.
X10.679 Y62.199 R0.5 F900.
G1 X10.415 Y62.343
X10.333 Y62.388 Z-19.993
X10.253 Y62.432 Z-19.971
X10.176 Y62.473 Z-19.935
X10.106 Y62.512 Z-19.885
X10.043 Y62.546 Z-19.824
X9.989 Y62.576 Z-19.753
X9.946 Y62.599 Z-19.672
X9.914 Y62.616 Z-19.585
X9.895 Y62.627 Z-19.494
X9.889 Y62.631 Z-19.4
G0 Z15.

M9
G28 G91 Z0.
G28 X0. Y0.
M30

In the post processor screen for F360 I tried changing the 'use G28' option to 'no', but this just omits the G28, and looks like it will then just home above the feature just cut.

Any thoughts to get it to go to work offset zero instead of machine zero ?

Neale
20-03-2017, 11:42 PM
One option might be to redefine the G28 position to be somewhere more useful/less inconvenient? Mine is over the fixed touchplate to help height setting when tool-changing in the middle of a job. I have a feeling that G28 is always in machine coordinates. What difference to the code does the "no G28" option make? Does it then generate some G0 moves instead?

GND
21-03-2017, 12:11 AM
I have used Fusion for many months now with my CNC router, and I discovered very early on that the G28 operation is complex and confusing if you are using Mach3. The answer however is simple - just turn it off in the CAM options. All works as expected then! I read this somewhere on a forum, along with long discussions as to what it should do, and what it actually does. Dazed and confused, I just turned it off, and I haven't looked back.

Hope that helps
Graeme

charlieuk
21-03-2017, 06:21 AM
how do you go about changing it or turning it of?

routercnc
21-03-2017, 08:07 AM
Hi Charlie,

When you post process the toolpath you get this menu:
21203
(red box)
Select G28 - no
I've also looked into searching the post processor library (green box) and there is another Mach3 PP in there which mentions various features including G28. I'll look into that.

Hi Neale,
Here is the code comparison with and without G28:

1) With G28
OP3_COUNTERBORE_6MM_0P5_300)
(0.5MM PITCH)
(T1 D=6. CR=0. - ZMIN=-15. - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21
G28 G91 Z0.
G90

(BORE1)

... boring operating in here

G0 Z15.

M9
G28 G91 Z0.
G28 X0. Y0.
M30
___________________________________________

2) Without:
(OP3_COUNTERBORE_6MM_0P5_300_NOG28)
(0.5MM PITCH)
(T1 D=6. CR=0. - ZMIN=-15. - FLAT END MILL)
G90 G94 G91.1 G40 G49 G17
G21

(BORE1)

... boring operating in here

G0 Z15.

M9
M30

I've not run the without G28 code on the machine but the last G0 just moves to Z15 above the feature just cut, not the work offset zero. Might be good enough.

Clive S
21-03-2017, 08:58 AM
I think you need to edit the F360 post. as a workaround you could just hand edit the file in notepad and change the G28 to a G0 and put the numbers in where you want it to go. Don't quote me though:concern:

Neale
21-03-2017, 10:26 AM
I think that the use of g28 by F360 and what happens with g28 in Mach3 show how there are differences in interpretation. F360 takes a fairly strict interpretation so throws in a G91 Z0, which should mean that the tool goes to the tool change point via machine coord Z0. However, Mach3 treats G28 as "go to SafeZ, then move to tool change point", making the G91 Z0 redundant. Generally, a safe option but I'm not sure if it is documented, just what I have observed. As it happens, my favourite tool change position is close to the corner of the bed where I normally have work zero, so it's not much of an issue for me - not too much unnecessary tool travel. Remember that it is easy to set the g28 position so if you are doing a big job, it might be worth temporarily changing it.

I'm guessing that for this F360 CAM you have the clearance height (is that the right one?) set to 15, so as far as F360 is concerned, this is a safe z value.

My personal bete noire is the M6 start/finish macro sequence, because what I want it to do might vary according to whether I shall be doing a tool height set/reset in the middle of it. Still working on that one. Especially when you find that the CSMIO plugin doesn't do what it's supposed to...

What it comes down to is that whoever writes the post-processor/Mach3 gcode interpreter etc has their own mental model of the "ideal" work flow, which is a bit of a pain if you work differently :frown:

routercnc
21-03-2017, 01:54 PM
Forgot to say thanks Graeme. As you can see from the above switching off G28 could be an option for me.

Clive, Neale,
Thanks for your thoughts on it. I thought about editing the code in notepad with find replace (G28 > G0) and am sure that would work, but bit of a pain to do it every time.

I will try and look into the F360 online site of post processors as this mentions a Mach 3 version with various features including something about G28 usage. . . With a bit of luck it will create G0 instead of G28

charlieuk
21-03-2017, 10:15 PM
thanks for this will be interested to hear if you figure anything else as I have just got in to using fusion and while mostly great there are a few things throwing me.