Fusion360 post processor and G76 threading not generating

More
26 Mar 2020 22:54 - 26 Mar 2020 22:58 #161626 by Danimal74
I downloaded the post processor for lathe turning from autodesk, and finally got the post processor to output g-code for a threading operation.

This is the G76 line it made:
N275 G76 X0.4885 Z-0.54 F0.03571

Linuxcnc said it needed the P, I, J, K values, so I hand computed them an put them in but it still would not load stating that there was a G76 line missing a P value "missing around line 280". Here is the entire cycle:

(THREAD1)
N265 M5
N266 M1
N267 T3 M6
N268 G54
N269 M8
N270 G97 S268 M3
N271 G95
N272 G0 X1.425 Z0.1969
N273 G96 D500 S100 M3
N274 G0 Z0.1786
N275 G76 X0.4885 Z-0.54 F0.03571
N276 X0.48
N277 X0.4715
N278 X0.463
N279 X0.4545
N281 G0 X1.425 Z0.1969
N282 G97 S268 M3

I just barely built this machine, so I am still trying to figure everything out. I have close loop PID control on the spindle with Spindle at speed, synchronized motion working (I think). Is there a good simple test to verify synchronized motion? I remember seeing a video where the spindle was off, and by hand rotating it the threading would follow. Being that I have not gotten a canned cycle to work yet, I haven't been able to test it. My thought was to command a S0 and delete the spindle speed command line (N273 G96 D500 S0 M3) and run the first pass by hand rotating the spindle. Is there a better way to do this?
Last edit: 26 Mar 2020 22:58 by Danimal74. Reason: typo

Please Log in or Create an account to join the conversation.

More
26 Mar 2020 23:12 #161630 by Clive S
This is the code that works for me:-
G0 G40 G18 G80  G21 G49 G95
G90 G7 

F1.5 S470

M3
G4 P1
M7
(Change the fist X to the Dia  P = the Pitch   K = Thread depth)
G0 X10 Z10
G76  P1.5  Z-12  I-0.1 J0.1  R1  K1.5  Q29.5 L0  H1

g0 X30
g0 Z50

M9
M5
M2
%
.
linuxcnc.org/docs/2.6/html/gcode/gcode.h...G76-Threading-Canned
.
or
.
linuxcnc.org/docs/2.7/pdf/LinuxCNC_Documentation.pdf - Page 238 G76
The following user(s) said Thank You: Danimal74

Please Log in or Create an account to join the conversation.

More
26 Mar 2020 23:17 #161632 by Danimal74
I did that for line 275 in my code, but then it said that it was expecting something around 280... Not sure what it was looking for. I will try your code and see if it will load on my machine and go from there. Thanks for the help!

Please Log in or Create an account to join the conversation.

More
27 Mar 2020 01:00 #161648 by Danimal74
I did get it working (somewhat) but the values I put in were not right at all. I am thinking that I have some prerequisite information incorrect. Fortunately I was able to verify that the synchronized motion is working properly so I am good there. I set the spindle speed to 0 and turned it by hand, and everything looked great.

Now my main concern is the post processor for fusion 360. I checked the Cycle box to generate the code above, but it is all wrong. Am I using the wrong post processor, is there another one that would work? I have been trying a few other ones out but none of them will compile the g code, they all just say that turning is not supported for one reason or another.

I am assuming that I am missing something, but if I cant find something soon I might give editing the post processor a go. This has to exist right?

Please Log in or Create an account to join the conversation.

More
27 Mar 2020 08:03 #161688 by alkabal
Hi

Not sure what is your problem, but i have do some G76 thread with my modified postpro available here (original also available)
forum.linuxcnc.org/26-turning/38148-lath...k-as-w-axis?start=10

Please Log in or Create an account to join the conversation.

More
27 Mar 2020 09:05 #161697 by Clive S

Danimal74 wrote: I did that for line 275 in my code, but then it said that it was expecting something around 280... Not sure what it was looking for. I will try your code and see if it will load on my machine and go from there. Thanks for the help!


I should have said remove this : (Change the fist X to the Dia P = the Pitch K = Thread depth) from the code.

Also if I remember the code has to have a feed rate ie F and S rate for it to run . I don't think the F rate number is critical but it won't run without it.
The following user(s) said Thank You: Danimal74

Please Log in or Create an account to join the conversation.

More
27 Mar 2020 15:37 #161712 by Danimal74
I did get your code working, and it confirmed the syntax I needed. Before this I would get an error when I tried to load the file so I could not even see what was needed for the cycle.

I then went back and modified my original code and I got it to work but my PIJK settings were screwy because it was doing like 500 TPI and I am not sure where I am missing something. I did change all the values to be the thread I wanted, and I noticed that your machine is metric. I still have some playing around to do, but at least I have a starting point.

Please Log in or Create an account to join the conversation.

More
28 Mar 2020 20:12 #161830 by Danimal74
I think that I am done trying to work on a custom post processor for the time being. I got about half of it done, but I keep running into trouble finding the correct variable names in fusion360 and I got the other manual code working pretty well. I commented it pretty well so hopefully the next time I am using it, I will remember a little better what everything does.

If anyone sees anything that is wrong, or should be added/removed let me know. I used responses here as well as others around the forum to build one that is easy enough to edit.

Here is what I ended up with:
%
(THREAD1)

#<_Diameter>=0.5          (Initial position, Driveline)
#<_Z_LeadIn>=0.05         (Frontside Stock Offset)
#<_Pitch>=0.03571         (Thread Pitch 1/TPI)
#<_Z_Finish>=-0.5         (Lenght of threads from Z0)   
#<_PeakOffset>=-0.003     (Major Diameter - Driveline, !0, Negative for External, Positive for Internal Thread )
#<_First_Cut_Depth>=0.01  
#<_Depth_Regression>=1.5  (1.0 = constant depth, 2.0 = constant area, values between have decreasing depth but increasing area)
#<_ThreadDepth>=0.0425    (Set to Diameter Mode, Major diameter - Minor diameter)
#<_CompoundSlideAngle>=0
#<_Spring_Passes>=2
#<_TaperAmount>=0
#<_TaperType>=0
#<_X_End_Position>=1      (Retract X position after complete)

#<_FeedSP>=0.03571
#<_SpeedSP>=250 

N10 G18 G20 G40 G49       (XZ Plane select, Units Inch, Cutter Compensation Off, Tool Offset Cancel)
N11 G54 G80 G90 G95       (Work Offset, Cancel Motion Mode, Absolute Distance Mode, Feed per Revolution)
N12 G7                    (Diameter Mode)
N15 F#<_FeedSP> S#<_SpeedSP> M3
N20 G4 P10                (Dwell P= Time in seconds)
N25 M7

N30 G0 X#<_Diameter> Z#<_Z_LeadIn>
N35 G76 P#<_Pitch> Z#<_Z_Finish> I#<_PeakOffset> J#<_First_Cut_Depth> R#<_Depth_Regression> K#<_ThreadDepth> Q#<_CompoundSlideAngle> H#<_Spring_Passes> L#<_TaperType>
N40 G00 X#<_X_End_Position>

N45 M5                   (Spindle Stop)
N46 M30                  (Program End)
%

Please Log in or Create an account to join the conversation.

Time to create page: 0.101 seconds
Powered by Kunena Forum