Fusion 360 G3 errors SOLVED

More
06 Jan 2019 04:29 #123581 by Roland2161
Good evening,

I just purchased a linux converted magnaturn lathe that runs wonderful. I am having a problem using fusion 360 post processing. When I hit run program I get an error saying "Near line xxx radius is to short to reach next point". I have tried everything I can think of to correct the problem and I am now lost. Any guidance would be great. Program posted below.

File Attachment:

File Name: 1003.txt
File Size:4 KB


The part was drawn and tool path made in fusion 360.
Attachments:

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

More
06 Jan 2019 09:27 #123592 by Hakan
Replied by Hakan on topic Fusion 360 G3 errors SOLVED
Tried the code on my lathe, it worked fine. Though with metric setup.
Also tried in ncviewer.com without any complaint.

In the file you attached, on which line does the problem appear?

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

More
06 Jan 2019 11:24 #123597 by tommylight
That might be due to tool size not being the same on Fusion 360 and Linuxcnc.

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

More
06 Jan 2019 14:30 - 06 Jan 2019 14:32 #123606 by Roland2161
After seeing that it worked on someone else's machine, the lathe seems to be the issue then. I just got it, I didn't build it. I'm running the machine with The Enhanced Machine Controller. That is what it says when it starts up. I am able to run a g3 if I type it in MDI. for example starting from 0,0 if i type g3 X.5Y.5 R.25 it will run. So if it would be tool size differences how do I check that? On the haas machine there are tables that can be accessed. Here I'm lost. Links to manuals or tutorials for linuxcnc would be appreciated.

I purchased this machine to start a home shop and because it was the cheapest running cnc machine I could find that would suit my needs. Any further help would be appreciated.
Last edit: 06 Jan 2019 14:32 by Roland2161. Reason: more info

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

More
06 Jan 2019 15:05 - 06 Jan 2019 15:06 #123607 by Hakan
Replied by Hakan on topic Fusion 360 G3 errors SOLVED
Tool size could defintely be a thing. But there are more things.
There is almost nothing in the preamble of the file, so the machine could be
in almost any state.

Just as comparison, here is the preamble for my lathe. Not that you should copy it,
but more to see that there are a few things set to put it into a know state.
G7
G18
G21
G54
G40
G90

; Tool: 1  ID Boring 
;   Op: Profile5
T1 M6 G43
G96 S45 D2000 M3
G0 ....
It may not even be correct, it is what the post processor I use give me.

Have a look at what post processor you have selected in F360.
I am not even sure there is a turning post processor for Linuxcnc included in F360.
Last edit: 06 Jan 2019 15:06 by Hakan.

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

More
06 Jan 2019 15:08 - 06 Jan 2019 15:13 #123608 by OT-CNC
Replied by OT-CNC on topic Fusion 360 G3 errors SOLVED

g3 X.5Y.5 R.25


If it's a lathe there should be no Y. Try programming with X and Z.

Sorry, I just saw the attached text file which seems the correct format.
Last edit: 06 Jan 2019 15:13 by OT-CNC. Reason: missed looking at the attachment

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

More
06 Jan 2019 16:00 #123610 by Roland2161
I am a mill guy I just threw Y in there by mistake my program is correct. I am still researching how linuxcnc works to get up to speed. I have a linux mill as well that I am diving into too.

As far as the pre format code I had put that stuff in before running the program. Cutter comp could very well be the issue, i just need to figure out how it works on this machine before I go further it seems. How do I view what is currently in the machine for cutter comp? Is there a list that can be brought up? I am running emc2 it what it says on the main screen.

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

More
06 Jan 2019 16:30 #123614 by Roland2161
No 360 does not have a lathe processor for linuxcnc, it does however have one for mill though. What cam software do you use Hakan?

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

More
06 Jan 2019 19:01 #123618 by Hakan
Replied by Hakan on topic Fusion 360 G3 errors SOLVED
I use Fusion 360 for milling and turning. Don't remember where I got the lathe post processor from.
I'll attach it here. It has worked fine for me for a long time. Disclaimer, etc.

File Attachment:

File Name: Linuxcnc_L....cps.txt
File Size:88 KB
Attachments:

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

More
06 Jan 2019 21:11 #123643 by andypugh
G3 radius and and point will be wrong if the machine is not in the correct radius / diameter mode. G7 / G8
You also need to be in the correct plane (XZ plane) G18
And, finally, the relative / absolute arc centre needs to be correct. G90.1 / G91.1

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

Moderators: Skullworks
Time to create page: 0.109 seconds
Powered by Kunena Forum