Tool Path Rounding Issue

More
25 Apr 2021 16:09 #207026 by Project_Hopeless
I have a spoil board re-surface program I created in Fusion360 with "straight line transition" enabled. When I run the program in a LinuxxCNC simulator I still get rounding, not straight line.

The program is fairly simple.
%
(SPOILBOARD RESURFACE)
(MACHINE)
(  VENDOR AJF)
(  MODEL 2)
(  DESCRIPTION BORG ROUTER)
(T1  D=50.8 CR=0. - ZMIN=-0.02 - FACE MILL)
N10 G90 G94 G17 G91.1
N15 G21
(WHEN USING FUSION 360 FOR PERSONAL USE, THE FEEDRATE OF)
(RAPID MOVES IS REDUCED TO MATCH THE FEEDRATE OF CUTTING)
(MOVES, WHICH CAN INCREASE MACHINING TIME. UNRESTRICTED RAPID)
(MOVES ARE AVAILABLE WITH A FUSION 360 SUBSCRIPTION.)
N20 G53 G0 Z0.
(FACE1)
N25 T1 M6
N30 S15665 M3
N35 G54
N40 G0 X8.187 Y-27.94
N45 G43 Z15. H1
N50 G1 Z5. F1000.
N55 Z-0.02
N60 Y0.
N65 Y1244.6
N70 X55.58
N75 Y0.
N80 X102.972
N85 Y1244.6
N90 X150.365
N95 Y0.
N100 X197.757
N105 Y1244.6
N110 X245.149
N115 Y0.
N120 X292.542
N125 Y1244.6
N130 X339.934
N135 Y0.
N140 X387.327
N145 Y1244.6
N150 X434.719
N155 Y0.
N160 X482.111
N165 Y1244.6
N170 X529.504
N175 Y0.
N180 X576.896
N185 Y1244.6
N190 X624.289
N195 Y0.
N200 X671.681
N205 Y1244.6
N210 X719.073
N215 Y0.
N220 X766.466
N225 Y1244.6
N230 X813.858
N235 Y0.
N240 X861.251
N245 Y1244.6
N250 X908.643
N255 Y0.
N260 X956.035
N265 Y1244.6
N270 X1003.428
N275 Y0.
N280 X1050.82
N285 Y1244.6
N290 X1098.213
N295 Y0.
N300 X1145.605
N305 Y1244.6
N310 X1192.997
N315 Y0.
N320 Z15.
N325 G53 G0 Z0.
N330 M30
%

My machine is a DIY so I have relatively slow accel/decel values.

Is there somthing in G code I can edit to reduce the rounding?
Attachments:

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

More
25 Apr 2021 16:24 #207029 by scotth
Replied by scotth on topic Tool Path Rounding Issue
G61 will get it.

Look at G64 to tune the system to what you need.

Scott

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

More
25 Apr 2021 21:42 - 25 Apr 2021 21:43 #207045 by Project_Hopeless

G61 will get it.

Look at G64 to tune the system to what you need.

Scott

Ok got it.

Now is there an in between command? I read and found a G62 corner override but LinuxCNC does not recognize it. Is there a adjustment to the rounding that is modal?
Last edit: 25 Apr 2021 21:43 by Project_Hopeless.

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

More
25 Apr 2021 22:12 #207047 by scotth
Replied by scotth on topic Tool Path Rounding Issue
G61 is exact path
G64 is Path Control Mode with Optional Tolerance it is adjustable

I don't see a G62.
The following user(s) said Thank You: Project_Hopeless

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

More
25 Apr 2021 22:27 #207050 by Project_Hopeless

G61 is exact path
G64 is Path Control Mode with Optional Tolerance it is adjustable

I don't see a G62.

Perfect that did the trick. Thx!

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

More
25 Apr 2021 22:50 - 25 Apr 2021 22:51 #207051 by Michael
Replied by Michael on topic Tool Path Rounding Issue
G64 P.005 would be a decent in-between depending on cutter size and speed.
G64 is used to maintain constant speed so if you have low acceleration then it will round more corners. The P will allow it to behave similar but only round to .005" (or whatever your machine unit is).

G61 is exact path mode. Just beware of how much tolerance and smoothing you have in your fusion tool operation.

G64 with no P is default at start up. You can add G61 or G64 Pxxx to your ini file start up codes or you can modify every ngc code fusion spits out or you can change the post processor.

linuxcnc.org/docs/2.8/html/gcode/g-code.html#gcode:g64
Last edit: 25 Apr 2021 22:51 by Michael.

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

More
16 Oct 2021 12:27 #223293 by paulsao
Replied by paulsao on topic Tool Path Rounding Issue
MichaelĀ I have a problem with what you mentioned here of the Fusion 360 smoothing, when I use this option in the axis when trying to open a g code I have problem of arcs at the beginning and at the end, and when I don't use this option axis opens the code without problems, maybe you know what is happening?

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

More
16 Oct 2021 18:26 #223309 by Michael
Replied by Michael on topic Tool Path Rounding Issue
Not sure what you are referring to. Are we talking about the settings in fusion 360 or a problem with a line of g code?
The following user(s) said Thank You: paulsao

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

More
16 Oct 2021 18:39 #223311 by paulsao
Replied by paulsao on topic Tool Path Rounding Issue
When I use the smoothing function in Fusion 360 it creates linear and arcs to smooth the splines with the pp it creates a G3, then when I want to open the G code in linuxcnc it gives me a different arc problem in the end and the start error. Now when I don't use that Smoothing function the Plasmac interpreter which is the one I use works fine.

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

More
16 Oct 2021 18:50 #223315 by Michael
Replied by Michael on topic Tool Path Rounding Issue
Smoothing in fusion will linearize the arc. If you want a pure arc turn off smoothing. And decrease the tolerance in the fusion tool path to what ever your machine can tolerate.

Are you referring to the lead in and lead out of the tool path? Fusion creates a lead in/out on most of it's tool paths that is a ramping arc usually in movements of 10% of cutter diameter of I remember correctly. These can be turned off on the final tab of the tool paths.

Also if you want to eliminate linuxcnc from all types of path blending then add G61 to the beginning of your g code file. This is exact oath following.

G64 is blending ng and on low acceleration machines it will blend a lot from the lead in to the actual arc you want.

G64 Px.xxx will blend with the limited amount. So between two paths P.005 will not go more than .005" away from the intersection of those two paths.
The following user(s) said Thank You: paulsao

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

Time to create page: 0.144 seconds
Powered by Kunena Forum