It never tried to move 20mm/s on the Z… but I think it did move the Z 20mm in the wrong direction.
Applied to all Gcodes post process with Notepad++ to manually add a G0 feed rate, quick hack, but I can use firmware with stock documented adjustments. Used the rest of this thread to set up tool path speeds.
[attachment file=“2019-03-22 21_50_58-Replace.png”]
X axis
Find What: G0X
Repalce with:G0F508\nG0X <----508mm/min
Z axis
Find What: G0Z
Repalce with:G0F50\nG0Z <----50mm/min
There is something with the way rapid feed rates is handled in the firmware and the way Aspire outputs commands between paths. I dont care enough to solve it but this hack works to get me working paths. Once solved Aspire becomes a pretty reasonable workflow for many existing trained CNC operators. 4
Is there a file for inches or just mm?
Is there a post processor for vectric that uses inches or just mm?
in reply to Klaus’s “Marlin_mm” upload file …
For those not sure what all this Post processing “PP” talk is about in terms of how and where to save the file Klaus has uploaded.
YOu need to place the file into Aspire’s “PP” folder you can find the folder within Aspire by going FILE >> OPEN APPLICATION DATA FOLDER inside this folder is the “PPost” folder where you will place Klaus’s “Marlin_mm” file
After this you will need to restart the Application for it to actually show up in post processor drop down list.
(As Per image )
HOPE THIS HELPS ( note: I used Klaus’s file as of 06/06/21 ) & it worked for me.
I know this is an old thread but has anyone come up with a post processor that allows for tool changes? Do you folks that need tool changes simply run multiple different files and then manually do a tool change between running each file?
I run aspire and do as you suggest running individual files for each bit. As long as you don’t power off your board, you just have to rezero Z between tool changes for each file. Pretty simple.
1 Like
I assume that means it also leaves the steppers engaged after every run? Which post processor are you using?
I do leave the steppers engaged until the last run.
2 Likes
If you find it useful:
I group all toolpaths into one file, tool changes run smoothly.
You will need to make adjustments on lines 67 and 118, the value should be set to the height of your touch plate.
I also provide the equivalent for Artcam:
In this case, the lines to be modified shall be 63 and 97.
Regards
Roger
2 Likes
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:
1 Like
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