Fusion 360 G3 errors SOLVED
- Roland2161
- Offline
- Junior Member
-
Less
More
- Posts: 36
- Thank you received: 0
07 Jan 2019 22:58 #123730
by Roland2161
Replied by Roland2161 on topic Fusion 360 G3 errors
All this is accomplished. Problem has been narrowed to the cutter comp, tool tables. G7 G8 could also be an issue but will focus on that next. Once I get these programming errors solved this machine should be 100% functional.
Please Log in or Create an account to join the conversation.
- Roland2161
- Offline
- Junior Member
-
Less
More
- Posts: 36
- Thank you received: 0
07 Jan 2019 23:00 #123731
by Roland2161
Replied by Roland2161 on topic Fusion 360 G3 errors
How do I pull up the tool tables to see what is in them?
I changed tool nose radius in 360 to .008 and set radius error to .000000001 and now I passed the radius error and I got a gouging error which, after what I just read in the manual could be caused by improper tool offsets, radius etc.
I changed tool nose radius in 360 to .008 and set radius error to .000000001 and now I passed the radius error and I got a gouging error which, after what I just read in the manual could be caused by improper tool offsets, radius etc.
Please Log in or Create an account to join the conversation.
- tightmopedman9
- Offline
- Senior Member
-
Less
More
- Posts: 69
- Thank you received: 7
07 Jan 2019 23:14 #123732
by tightmopedman9
Replied by tightmopedman9 on topic Fusion 360 G3 errors
I encountered this issue when a tool offset in the tool table was added. Changing the offset back to 0 fixed the issue.
Please Log in or Create an account to join the conversation.
07 Jan 2019 23:44 #123736
by Hakan
Replied by Hakan on topic Fusion 360 G3 errors
Yes, tool offset and/or nose radius should either be in linuxcnc or in Fusion. Not both.
If you haven't changed anything in Fusion it will do toolpaths after the tool setting in Fusion.
Nose radius should be zero in linuxcnc then.
It should be possible to do the other way, it is an active choise in one of the tabs.
If you haven't changed anything in Fusion it will do toolpaths after the tool setting in Fusion.
Nose radius should be zero in linuxcnc then.
It should be possible to do the other way, it is an active choise in one of the tabs.
Please Log in or Create an account to join the conversation.
- Roland2161
- Offline
- Junior Member
-
Less
More
- Posts: 36
- Thank you received: 0
07 Jan 2019 23:50 #123738
by Roland2161
Hakan how do I access the tool table in emc2? I need to set the radius in the machine to 0.
Replied by Roland2161 on topic Fusion 360 G3 errors
Yes, tool offset and/or nose radius should either be in linuxcnc or in Fusion. Not both.
If you haven't changed anything in Fusion it will do toolpaths after the tool setting in Fusion.
Nose radius should be zero in linuxcnc then.
It should be possible to do the other way, it is an active choise in one of the tabs.
Hakan how do I access the tool table in emc2? I need to set the radius in the machine to 0.
Please Log in or Create an account to join the conversation.
08 Jan 2019 00:14 - 08 Jan 2019 00:14 #123740
by Hakan
Replied by Hakan on topic Fusion 360 G3 errors
I assume you use the "axis" gui? There should be an item "Edit tool table..." in the File menu. An assumption though, I use another gui.
Last edit: 08 Jan 2019 00:14 by Hakan.
Please Log in or Create an account to join the conversation.
- Roland2161
- Offline
- Junior Member
-
Less
More
- Posts: 36
- Thank you received: 0
08 Jan 2019 01:05 - 08 Jan 2019 01:07 #123741
by Roland2161
I think I figured out the tool table. But I am still having problems with the program. Program attached.
It says "near line 265 arc radius to small to reach end" so I deleted that radius down, and the program will run without the last bit of program. What gives? Any idea? Just a bad design then?
Replied by Roland2161 on topic Fusion 360 G3 errors
I assume you use the "axis" gui? There should be an item "Edit tool table..." in the File menu. An assumption though, I use another gui.
I think I figured out the tool table. But I am still having problems with the program. Program attached.
It says "near line 265 arc radius to small to reach end" so I deleted that radius down, and the program will run without the last bit of program. What gives? Any idea? Just a bad design then?
Attachments:
Last edit: 08 Jan 2019 01:07 by Roland2161. Reason: wrong program
Please Log in or Create an account to join the conversation.
08 Jan 2019 04:24 #123747
by OT-CNC
Replied by OT-CNC on topic Fusion 360 G3 errors
Have you tried diameter mode G7? Also try outputting the g code with I and k.
I recall having a similar issue a while back using radius format arcs. R in G2/G3.
I recall having a similar issue a while back using radius format arcs. R in G2/G3.
Please Log in or Create an account to join the conversation.
- Roland2161
- Offline
- Junior Member
-
Less
More
- Posts: 36
- Thank you received: 0
13 Jan 2019 01:59 - 13 Jan 2019 03:51 #124060
by Roland2161
Replied by Roland2161 on topic Fusion 360 G3 errors
I have tried everything. This is my latest program an it is still saying arc radius to small to reach end point. Or arc radius different at end point. I found tool.tbl in my computer and set the x z both to +0. The only entries in it were for x z. Unless the table is set up wrong I am at a loss. No idea. If I put a program in by hand it will cut a radius, but it won't from 360. I have attached the latest program I tried. Can someone please check to see if this runs in there machine?
What else am I missing? Could someone send me a program to see if I can put it in my machine?
What else am I missing? Could someone send me a program to see if I can put it in my machine?
Attachments:
Last edit: 13 Jan 2019 03:51 by Roland2161.
Please Log in or Create an account to join the conversation.
13 Jan 2019 10:22 #124068
by andypugh
Replied by andypugh on topic Fusion 360 G3 errors
Looking through the code one thing that looks odd is that there are lots of G40 and G42 commands, but at no point does it load a tool or set a tool diameter.
Which postprocessor are you using in Fusion?
I am not currently anywhere near Fusion or LinuxCNC, but is there a way to set Fusion to do the tool compensation in the postprocessor rather than in the control, as a first step?
My suspicion is that Fusion is using the wrong control point for the offset. Do the tool orientations and diameter match exactly between the Fusion360 tool table and the LinuxCNC tool table?
(And do LinuxCNC and Fusion even agree on how tool orientation and control point are defined?)
Doing radius comp In the control is techically better as you can tweak the offset to compensate for wear or if you change to a different insert. But generally on a lathe you can nearly always ignore tool radius as long as you don't care about fillet radiuses being spot-on. Diameters and lengths come out correct regardless (unless using tool orientation 0) and in fact I hardly ever bother with it for the parts I make.
Which postprocessor are you using in Fusion?
I am not currently anywhere near Fusion or LinuxCNC, but is there a way to set Fusion to do the tool compensation in the postprocessor rather than in the control, as a first step?
My suspicion is that Fusion is using the wrong control point for the offset. Do the tool orientations and diameter match exactly between the Fusion360 tool table and the LinuxCNC tool table?
(And do LinuxCNC and Fusion even agree on how tool orientation and control point are defined?)
Doing radius comp In the control is techically better as you can tweak the offset to compensate for wear or if you change to a different insert. But generally on a lathe you can nearly always ignore tool radius as long as you don't care about fillet radiuses being spot-on. Diameters and lengths come out correct regardless (unless using tool orientation 0) and in fact I hardly ever bother with it for the parts I make.
Please Log in or Create an account to join the conversation.
Moderators: Skullworks
Time to create page: 0.185 seconds