russtuff wrote:
With the new update to CAM for turning in Fusion 360 I assume there are more posts on the way. I use LinuxCNC for a Grizzly G0602 I converted to CNC myself. I've been trying to use the Generic Fanuc post but so far haven't gotten any good code to try. Any idea if/when a LinuxCNC post will be released?
Thanks.
Scott Moyse
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
RevOps Strategy Manager at Toolpath. New Zealand based.
Co-founder of the Grumpy Sloth full aluminium billet mechanical keyboard project
Achim wrote:
The best posts for milling for LinuxCNC should be "emc.cps" or "eding.cps".
JanHouwers wrote:
Hello,
I am using a Wabeco Lathe with LinuxCNC and i have been spending some time to change the Haas Turning Postprocessor in a way that is ouputs code that LinuxCNC understands. This is very alpha.. So check carefully the code that is being produced.
Cheers, Jan
tomae wrote:
I've been using the Tormach PathPilot turning post discussed here:https://camforum.autodesk.com/index.php?topic=7452.msg35637#msg35637 on my Linux-based Emco lathe. It works fine other than the tool change dialog. I have to hand edit that. PathPilot is based on the latest Linuxcnc and should be very very close. I will probably change the tool change dialog at some point so I don't have to hand edit it.
-Tom
tomae wrote:
The Tormach post outputs a tool change in some strange (to me) syntax like: T0505
tomae wrote:
The Tormach post outputs a tool change in some strange (to me) syntax like: T0505
tomae wrote:
The Tormach post outputs a tool change in some strange (to me) syntax like: T0505
I changed my version of the post at this line:
writeBlock("T" + toolFormat.format(tool.number * 100 + compensationOffset));
To be instead these three lines:
writeBlock("G53 G0 X0");
writeBlock("G53 G0 Z0"),
writeBlock("M6 T" + toolFormat.format(tool.number) + " G43 H" + toolFormat.format(tool.number));
And now it writes:
G53 G0 X0
G53 G0 Z0 (to send my turret to the change position)
M6 T0005 G43 H0005
HOWEVER, this is a complete hack-job. I don't know what compensationOffset is doing or why it is added ("+") to the toolnumber multiplied by 100....? So buyer 😉 beware! No warranties expressed or implied 😛
I can say that there is no difference in the posted code (other than the tool change lines) between using the original post and my hacked post for the several parts I have used it with.
Also, the Tormach post doesn't use G76 for threading according to Linuxcnc documentation (http://linuxcnc.org/docs/2.6/html/gcode/gcode.html#sec:G76-Threading-Canned). Not sure why - looks more like a Fanuc maybe? Anyway, the threading code that the Tormach lathe post put out wouldn't run on my Linuxcnc (ver 2.7) controller. I would love for someone to modify the post to implement the correct syntax for the Linuxcnc G76 canned cycle!!
-Tom
andypugh wrote:
tomae wrote:
The Tormach post outputs a tool change in some strange (to me) syntax like: T0505
Tormach use a modified version of LinuxCNC that accepts both tool and wear offsets in the T-word and does not require an M6.
This is reasonably standard in lathes where you can not normally pre-fetch a tool.
There is a sample config (sim / axis / remap / lathe-fanucy ) which remaps the T-command to work this way with the normal, unmodified LinuxCNC. You might find it convenient to configure your own lathe this way, so that a toolchange is T05 rather than M6 T5 G43.
Rob Lockwood wrote:
I'm actually a little curious how your setup works, using an H# on turning.. A mill "needs" just one offset measurement, length. A lathe NEEDS both an X offset and a Z offset to be of much use.. does the turning version of LinuxCNC contain two offset registers for the H value? It's odd to me that linuxcnc wouldn't have followed convention here, as they're usually pretty good.
I would definitely like to see a linuxcnc turning post. I'm trying to cut my first thread since the upgrade to see if I succeeded and found that the g76 is wrong with the tormach post. I tried unchecking the "use cycle" box and then it failed to post at all.
I am working on a LinuxCNC lathe post for Fusion360 as I haven't seen an official one yet. I'd say it's alpha level now, needs a lot more testing (which I will do as my lathe build progresses). Currently all the movements work, tool change code is ok, and G76 canned cycle should be allright as well. That is for the manual type lathe I have converted. For other types, I have no idea and no way to test.
Patches welcome, of course.
Thanks. Could you put the G30 back in without the z#5... Being able to have a safe tool change position was one of the reasons I wanted to upgrade to linuxcnc. Anyway I didn't make it to the g76 because I got a following error. I haven't got the settings quite figured out for that yet. At least it didn't give me any errors that made it refuse to run.
I'll see what I can do with the G30.
Does the G30 goes before every tool change and at the end of the program? Are there any params that need to be configured with it as well, like X or Z moves that G30 can take?
It looks like I don't need those G30s. I was just reading the linuxcnc gcode reference and it says it will move to G30 when M6 is programmed if you add the line TOOL_CHANGE_AT_G30=1 to the [EMCIO] section of the ini file. I just tested it with mdi and it works. Thanks.
Can't find what you're looking for? Ask the community or share your knowledge.