Fusion 360 Milling post with G64 Pn

More
24 Mar 2019 11:46 #129467 by spangledboy
Thanks for pointing that out Marty. I actually somehow hadn't noticed that neither G61 nor G64 appear to be implemented in the default post - unless your machine has a default G61 in the ini file, then you end up with G64 with no applied tolerance, which is pretty much the worst case scenario.

My take away from this is to firstly update my ini file so there's a G61 in there and then to look at a good way to implement G61 & G64 switching along with tolerance changes on an operation by operation basis.

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

More
24 Mar 2019 12:24 #129468 by MartyJ
Yes, the g64 with no P value makes some pretty wonky parts on my machine, since most of my operations are 250-450 ipm.

BTW I really like your tool change comment implementation. I have HSMworks comments stating the diameter, type, and intended feed rate in the tool library, so on tool change during a long production run I don't forget where I was in the process. It's saved me several wrecked parts already. Thanks.
The following user(s) said Thank You: Lcvette

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

More
24 Mar 2019 12:58 #129469 by spangledboy
I've submitted a request on the Autodesk HSM/Fusion360 Idea board for G61 & G64 to be properly implemented in the post processor. Please vote for it/add comments there as you see fit.

forums.autodesk.com/t5/hsm-post-processo...g-with/idi-p/8679566

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

More
24 Mar 2019 13:03 #129470 by spangledboy
Glad to hear I've been of some use! Getting a notification of what to put in next is always helpful for those of us without automatic tool changers....

Somehow I've got away without being badly affected by the sloppy G64 in my machine - I guess it's down to my low speed moves as I mostly work in steel and aluminium. The realisation dawned when I noticed some inside corners being less sharp than they should be in my latest job.

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

More
24 Mar 2019 16:27 #129487 by pl7i92
there are now so many linuxcnc posts around and in this forum
that people are strugeling to get the right one

so many people turning from "mach" here are with G53 and linuxcnc dont like this files

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

More
26 Mar 2019 14:50 #129693 by andypugh
Fusion360 puts in a G53 G0 Z0 before each tool change.
This is OK, and LinuxCNC compatible, but ony if 0 is the top of Z travel.
(But that would be just as much of a problem with any other controller)

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

More
06 Feb 2020 21:33 #156655 by Lcvette

OK all, here's what I ended up doing.
I was going to start with Spangled's post, because I was going to have an overall G64 P0.0x value, combined with a per-operation G64 P0.0x value based on if the operation has a "smoothing" parameter applied.

But then I thought, that's not really what the smoothing is for. What we're really talking about is the overall tolerance of the operation, and a lot of operations which may need tight tolerance machining at high speeds may not have a Smoothing parameter, or you may not want to use Smoothing just to get your machine to not round corners under acceleration.

So I made it post out a G64 P0.0x block on every operation, which inherits the Tolerance value from that operation. (I am aware that this will actually result in a tolerance zone of double the input tolerance value. I'm fine with that, though it will undoubtedly cause some confusion. Fine for my purposes, I'll just put a conservative tolerance zone in there.)

I'm going to try using it like this for a bit, I haven't used it to run a machine yet, so keep yer finger on the E-stop button until you've run a test program.


@MartyJ,

this is great ive been searching all over for a solution to the tolerance vs G64 P value and this is a wonderful idea you have put together!

Have you run it on the machine? if so, what was your result? it wold be nice if fusion had a separate box for the G64 output per operation as i think it would be better if the tolerance and smoothing could be set lower and let linuxcnc motion planner deviate from per operation tolerances which i think may result in an actual smoother machine movement. but i'm just starting to try and understand how it all works together currently so I could of course be off base. have you done anymore playing with the post since this was put up? any other tips or tricks you wouldn't mind passing along?

Thanks in advance!

Chris

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

More
06 Feb 2020 23:09 - 06 Feb 2020 23:11 #156664 by MartyJ
@LCvette, yes, I've run production with this post for almost a year and it works well. I just set the smoothing (correction: tolerance) value to half of what I normally would to allow for the doubling effect of the G64. I've run it doing adaptive clearing and profiling at up to 500 IPM (12k MMPM).
Next step I want to do is have it set up so G00 moves get a large P value, could be cool. But not really necessary.
Last edit: 06 Feb 2020 23:11 by MartyJ.

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

More
07 Feb 2020 03:40 #156673 by Leon82
G90 G0 G53 Z0 will solve any errors in Linux CNC.for some reason it wants it like that I have noticed

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

More
07 Feb 2020 08:36 #156685 by bbsr_5a
Thanks
on multiaxis the G53 Zero is offen when not at all into the Part
this is why i asked here

CAN somone tell me the Part of the Postprocessor at Fusion to change to get rid of this G53 Z0
im lost in the Syntax

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

Moderators: Skullworks
Time to create page: 0.106 seconds
Powered by Kunena Forum