This is fantastic thank you. I notice that the feed rate is not copied for every line. That is not an issue? I know marlin uses the last feed rate input as the current feedrate but I thought I read somewhere that its important to have the feed rate on every command line.
1 Like
The big danger is this:
G1 X100 F3600
G0 Z5
Because Marlin treats G0 the same as G1, so lifting the Z to the clearance plane will be at the same speed as the G1 in X. The Z can’t move that fast, so it will be likited by the max firmware settings.
A similar issue is when switching from XY moves to plunge. There needs to be a speed on those lines.
An annoying, but less dangerous situation is this:
G1 X100 F3600
G0 Z5 F300
G0 X0
Because the CAM knows it is clear of the work, so it asks for a rapid. But Marlin treats them the same, so it will go super slow.
In estlcam, there is a setting for adding it to every line, which is how these issues go away. It is just easier than trying to decide which scenarios have to have feedrates.
2 Likes
I will look into it and see if something can be done about it.
Regards
Roger
Just messing around with the post processor a bit.
It does look like it adds the feed rate to the first plunge which is good. The G0 speed would just be the last known speed while I was homing the machine (not ideal but manageable).
G0 X27.882 Y232.882 Z5.000
G1 Z-6.667 F180.0
G1 X28.010 Y232.758 F2100.0
G1 X28.145 Y232.639
G1 X28.285 Y232.525
At the end of the code though it does doe a Z travel at the feed rate speed (2100) which is not great. I’m thinking a work around would just be to turn the max Z speed down in the firmware to throttle the machine a bit.
G1 X27.758 Y233.010
G1 X27.882 Y232.882
G0 Z5.000
G0 Z20 F300
G0 X0.0000 Y0.0000 F1200
M00 STOP Spindle
I have not run any of this on the actual machine. Just playing around with the PP and software while trying to understand the options here:
2 Likes
At the moment, as Jeff said, I think that’s the best idea 
There is a github repository with marlin pp files that are in mm and inch and they are working for me with a bit of adjusting.
Marlin MM and inch PP for vcarve or aspire
So guys, have made a pp for aspire.
Have 2 versions:
Normal: with no altered rapid speeds.
Rapid: has modified rapid speeds.
These also have tool changes that shift to X0Y0 and Z to 10mm, also has a Z-probe on tool change and at beginning. Z probe set to 0.5mm thick.
Also has fan outputs that turn on/off in case users use these outputs to turn router/vacuum etc (tested on SKR Pro v1.2)
These were made & tuned for the lowrider V3
I have tried both versions.
Doing 2 identical cuts with same toolpaths etc, to compare.
The normal version took 3min, while the rapid shaved it down to 2min both at F900 cuts.
May not seem like much, but would be a big deal on longer prints.
Another eg, doing 3x struts for the lowrider under normal it took 2hs 47, rapid took 2hrs 3 mins. Both files had 2 paths at F500 for pilot holes using 1/16inch bit to secure strut and tool change which had 4 paths at F900 for cutting using 1/8inch endmill.
Purely for testing times purposes.
Normal version:
Rapid version:
Let me know your thoughts 
3 Likes
I see there are named “LowRider Marlin…”. They will also work for Primo, correct?
genius, just what i need it, also the reminders before it prints love it
Glad you like it