Simple Rectangle has a radius on all edges ... strange

More
27 May 2022 17:02 #244001 by Roman Simon
Hello,

I use Fusion 360 to generate Gcode (for my sherline lathe). This program

%
(3_5MM_KUGEL_RANTASTEN)
(T5  D=5. CR=2.5 - ZMIN=-2. - KUGELKOPFFRSER)
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.
(PROJEKTION1)
N25 T5 M6
N30 S5000 M3
N35 G54
N40 M8
N45 G0 X-75.5 Y-18.875
N50 G43 Z15. H5
N55 G1 Z5. F1000.
N60 Z-2. F333.33
N65 Y18.875 F1000.
N70 X75.5
N75 Y-18.875
N80 X-75.5
N85 Z5.
N90 Z15.
N95 M9
N100 G53 G0 Z0.
N105 M30
%

draws just a rectangle. But when I ran the program with Linux CNC, all edges has a radius. How, Why???
I can not see the radius in Fusion 360 or on a other g code viewer (ncviewer.com/). Or even in the Linux CNC preview.

Any help would be great.

Thank you & Best Regards
Simon


 

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

More
27 May 2022 17:12 #244002 by Todd Zuercher
Add this to the end of your N10 line.
G64P0.01

The default start up setting is G64 with no P tolerance. G64 is constant feed, and will round corners to prevent the tool from stopping in a corner. Adding a Pxx tolerance to the g64 command forces the path to remain withing that tolerance of the programed path. G61 is exact path, but will come to a complete stop at every corner (not usually a good thing.)

linuxcnc.org/docs/html/gcode/g-code.html#gcode:g64

You may want to edit the post you are using to add the G64P0.01 code.
(I don't use Fusion 360 so can't tell you how.)
The following user(s) said Thank You: Roman Simon

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

More
27 May 2022 17:22 #244003 by andypugh
More explanation here: linuxcnc.org/docs/html/user/user-concept...#_trajectory_control

It might be worth increasing the maxaccel of each joint. If those numbers are low you are basically telling LinuxCNC "This machine can't make fast corners"
The following user(s) said Thank You: Roman Simon

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

More
27 May 2022 17:30 #244007 by cmorley
I always wondered why we don't set g64 to reasonable defaults.
This is an on going user problem.

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

More
27 May 2022 17:40 #244010 by Todd Zuercher
In the CNC world this isn't unusual. Fanuc controls behave in a similar manner without even having the option to add the P tolerance to fix it, unless their G08 or G05 options are installed and activated (options you must pay a hefty price for by the way.)

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

More
27 May 2022 17:43 #244011 by robertspark
People need to learn a bit of gcode and read the manual (yes I know I sound like an arogant $%%^^) but.....
if you set a "reasonable" default.... it may not be reasonable to that application like plasma or mill or lathe or metric or imperial or whatever.

I tend to use a G61 finishing cut (with mill router and lathe....)

And G64 for roughing cuts....

Ang obviously G64 with plasma but a rather lax settings

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

More
27 May 2022 17:46 #244012 by roland
It would be nice if the G64 values were an entry in the ini.
These values could then be overwritten in the gcode if needed

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

More
27 May 2022 18:06 - 27 May 2022 18:06 #244014 by PCW
You can set initial gcodes in the ini file, the downside is that
this is only done once when LinuxCNC starts so any program you
have run since LinuxCNC started can change these and you
will not know. That's why it's better in general to have these modal
settings in the gcode itself.
Last edit: 27 May 2022 18:06 by PCW.

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

More
27 May 2022 22:16 #244031 by cmorley

robertspark post=244011 userid=23480People need to learn a bit of gcode and read the manual (yes I know I sound like an arogant $%%^^) but.....
if you set a "reasonable" default.... it may not be reasonable to that application like plasma or mill or lathe or metric or imperial or whatever.

I tend to use a G61 finishing cut (with mill router and lathe....)

And G64 for roughing cuts....

Ang obviously G64 with plasma but a rather lax settings

Sounds like you set the g64 in your gcode, so defaults wouldn't bother you.
Having the planner default to following the gcode path closely seems much friendlier then having it diverge unexpectedly.

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

More
27 May 2022 23:47 #244033 by robertspark
Thats actually a good point, yes they are set in my gcode.

Probably a new user who does not understand gcode would not be bothered by them until they started to understand that maybe there was a better way.

{maybe I'm just a sad git who reads the manual and loves re-reading the g/m/o codes sections.....}

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

Time to create page: 0.233 seconds
Powered by Kunena Forum