V10.5 Feedrate missing

[brrian]

I installed V10.5 & set up my first program to run on my Workbee, using the Grbl (Inch) post processor, same as I always used. I loaded & ran the program in OpenBuilds CONTROL & it popped up an error about a feedrate missing. To ensure it was caused by the version change, I went back, set up & ran the program in V10.0 & it ran fine.

Both files are in the attached zip file. V10-5.gcode was created in V10.5 & seems to be missing feedrates - the first (F25.0) is missing about 10 lines in.

Any ideas? Thank you,

Brian

[mtylerfl]

Hi Brian,

Are you certain you are using the exact same Post Processor for 10.5 as you are using in version 10?

[Adrian]

I'm not 100% sure if it's an error but where I would expect to see [F] for feedrate variables there are [P] for power ones instead. That isn't the same on other base post processors.

[brrian]

I'm sure it's the same post processor. I installed 10.5, migrated my settings, set up my cut & saved my toolpath with the Grbl (inch) post processor.

I'm using an OpenBuilds Workbee & just to see what would happen, I saved using the OpenBuilds GRBL (Inches) post processor & here's what the start of that file looks like (in case it's of some use?). It also appears to be missing the feedrate that's in my V10.0 file.

T1
G17
G20
G90
G0Z1.5000
G0X-3.0000Y23.0000
M3S21000
G4 P1.8
G0X0.1875Y-0.1845Z0.5000
G0Z0.3750
G1Z0.0000
G1Z-0.0019
G1Z-0.0250
G1X0.1593Y0.5373F38.0

[brrian]

...just thought to try this: I copied the "Grbl_inch.pp" post processor from my 10.0 installation & pasted it into the My_PostP folder for my 10.5 installation. then I saved my toolpaths using it, and the missing feedrates are there.

During migration i left "Copy My Post Processors" checked, if that's helpful to know...

[Adrian]

It's as I said in my post above. The v10 GRBL post processor has feed rates in each of the sections. The 10.5 one has power (laser) settings instead. I don't know if that's intentional or not but going by the problems you're having I'd guess not. When you migrate the post processors it won't overwrite updated ones.

[Kinger]

I'm having the same problem luckily job stopped and spindle shutdown
How do I fix this ?

Thanks Stephen

[mohamed]

Could you send the project file itself please for us to investigate? The current GRBL post should work with laser and non-laser toolpaths. Power [P] will only output if it's applicable (i.e. it's a laser tool). As far as I can see, we haven't removed any [F]s. Perhaps, also attach the post-processor you're using (the one you're having issues with) just so we're on the same page. You could either do this here or send us on support@vectric.com

Thank you

[Adrian]

Apologies, I didn't spot that the arc moves were commented out in the v10 version which is where the F's used to be.

[garymkrieg]

I.m not sure if anything was sent into support for this or this has been resolved but I am at Vcarve Pro 10.503 and am getting the no feed rate message.

Here are the Gcode files for the same toolpath

Vcarve Pro 10.022
T1
G17
G20
G90
G0Z0.2000
G0X0.0000Y0.0000S16000M3
G0X-0.1900Y-0.1295Z0.2000
G0Z0.0197
G1Z0.0000F10.0
G1X11.3150F200.0
G1Y0.1705
G1X-0.1900
G1Y0.4705
G1X11.3150
G1Y0.7705
G1X-0.1900
G1Y1.0705
G1X11.3150
G1Y1.3705
G1X-0.1900

Vcarve Pro 10.503
T1
G17
G20
G90
G0Z1.0000
G0X0.0000Y0.0000
S16000M3
G0X-0.1900Y-0.1295Z0.2000
G0Z0.0197
G1Z0.0000
G1X11.3150F200.0
G1Y0.1705
G1X-0.1900
G1Y0.4705
G1X11.3150
G1Y0.7705
G1X-0.1900
G1Y1.0705
G1X11.3150
G1Y1.3705
G1X-0.1900

I'm no Gcode expert but there is a difference I see a "G1Z0.0000F10.0" in the tool path that works and a "G1Z0.0000" in the one that gives the "No feed rate" message. I am using GRBL (inch) (*.gcode) for both tool paths.

Gary

[brrian]

Zipped and attached: my project file, the Grbl_inch post processor (that either came with 10.5 or was migrated from 10.0), and the Grbl inch post processor that I manually moved over from 10.0. Let me know if you need anything else...

** Edit: Adrian, I reread your post & you said "When you migrate the post processors it won't overwrite updated ones.". So if you updated the Grbl post processor in 10.5, when I migrated, it would have kept that new one, not overwritten it, right? & that explains why the old version I copied over works... because it's not the same.

Is it safe to use the 10.0 post processor until this is figured out? I don't use a laser.

[garymkrieg]

Did some more snooping and looked at the 10.0 GRBL (inch).pp and the 10.5 GRBL (inch).pp they are definitely different. What concerns me the History of what programmer changed what and when are the same with the last recorded update on 11/2/2015. Having been a programmer for almost 30 years that concerns me.

[ictdesignsco]

I have had the same problem using GRBL generic. I’m running a MillRightCNC Mega V with UGS. I will try copying my post processor from 10.0 to 10.5 to see if that resolves it.

What I noticed between the two is that the 10.0 gcode has the first feed command on the first G1 line, immediately after the first Z position command. The 10.5 gcode has the first feed command a few lines down after the first Z position command

[AdamJ]

Is it safe to use the 10.0 post processor until this is figured out? I don't use a laser.

Absolutely, it is fine to use your 10.0 post processor.

Thanks,
Adam

[brrian]

Adam - I'm curious if you guys have figured anything out with this?