The restart position changes the speed of the bit in version 1.4.11 and 12. My ipm for bit is 60. on restart it changes to less than 3. Up dated to version 11 in late December 2024 and had the issue. Upgraded to .12 on March 13 2025 and the issue is still there.
When I use the start from line feature, it goes to the correct line, but it moves at 3.1 inches per minute. This has been happening since the last build. Iām using 1.4.12 now on a windows 11 laptop.
Am I doing something wrong?
Is anyone else dealing with this?
Adding to the post.
On some projects, I need to stop the carve and go over a small area an extra time or two. Everything runs smoothly until I use the āStart from Lineā feature. When I do, it jogs to the selected line normally, but once it resumes the toolpath, the feed rate drops to 3.1 inches per minute.
Is there any other information needed?
Following. Same issue.
Running latest gsender (just downloaded prior to mishap). Altmill 4x4.
This has happened 3 times since new version download 3 days ago. When selecting start from line, travels to start location and runs at 1 inch/minute. Have tried shutting down everything. Rebooting laptop, restarting application.
Have tried starting from XY Zero, and XY location nearer start point. Spindle travels to correct location, and runs at 1 inch/minute.
Have tried starting from different lines. Will only start from line 1 at normal speeds and feeds.
The cut Iām working on is 575,000 lines.
1 Like
Sorry youāre dealing with it too, but Iām glad Iām not the only one experiencing this issue.
Iām back in the shop, and it still happens. Iām running a small test gcode. I click the button that ācopies the last 50 lines from the terminal.ā Does it tell anybody anything? Any thing else I should copy and post to help with this
ok
G0 Z0.5
ok
G21
ok
G90
ok
G0 X0 Y0
ok
ok
G20
ok
G90 G0 Z0
ok
G21
ok
G0 G90 G21 Z35.56
ok
M3 F80 S15000
ok
G0 G90 G21 X142.875 Y34.925
ok
G0 G90 G21 Z-2.540
ok
G20 G90 G91.1 G54 G17
ok
G1
ok
G4 P1
ok
X1.3750
Y16.6250
X16.6250
Y1.3750
X12.3750
X12.3750Y10.5740
G3X9.0000Y13.9490I-3.3750J0.0000
ok
ok
ok
ok
G3X5.6250Y10.5740I-0.0000J-3.3750
ok
ok
G1Z-0.1500F40.0
G1Y1.3750F80.0
!
\x18
ok
Grbl 1.1h [ā$ā for help] LongMill build Feb 25, 2020
Here is the full Gcode if someone else wants to try or look at it. It is a profile cut, 15"x15" archway. 126 Lines
03-28-25 TEST start from line.gcode (2.6 KB)
My exported gsender settings
gSender-settings-3_28_2025-1_06_00 PM.json (70.8 KB)
my export firmware
gSender-firmware-settings-3_28_2025-1_08_06 PM.json (556 Bytes)
Iām not really sure why it would be doing that but GSender is not converting the feed rate.
Itās using the imperial value of 80in to set the feed rate when the controller is set to metric at the time, so the feed rate ends up being 80mm or 3.15in.
I would try switching the CAM post processor to mm and see if that solves this issue.
2 Likes
Thanks for the idea; Iāll try it out tomorrow.
@cjm It worked. I couldnāt wait until tomorrow. Thank you. @EDWoodcraft The fix for me was changing from UGS GRBL inch to UGS GRBL mm. Hopefully, it works for you, too.
I wonder why it only affected it when using the start from line feature in Gsender.
2 Likes
@Swinly If you donāt mind, Lonnie, what CAM application are you using to generate the toolpaths?
Iām using Carveco maker plus
@Swinly Tks much, Lonnie
1 Like
Yes. Reported twice but no reply
@Allen761 Assuming youāre using the same post processor I was, UGS GRBL Inch, have you tried switching to UGS GRBL mm? That solved the issue for me. Iām not sure why or why it only affected the start-from-line feature. I could have sworn I was told the Inch/mm post processor didnāt matter, but I must have misunderstood something.
1 Like
same problem hereā¦very very very slow when stopping a carve then starting at a line in the code approx. where the carve was stoppedā¦Sienci needs to fix this problem.
I just experienced the same thing using v1.4.11. I backed off to v1.4.10 and it works like a champ.
1 Like
When I restart a job mid-file, lets say āLine 600,ā the router is moving at a snails pace. Crawling until it goes like for 3 minutes. Maybe to a certain line. And then it resumes at full speed. Happens on many files of mine. Am I the only one? No issues in the past.
Gsender 1.4.12
More than likely your gcode does not request a speed change right after you restart the job. When it finally gets another speed change request it returns to normal operation.
You can (donāt know if it is practical) insert a speed command into the gcode file or, and I donāt know if that works, insert a speed command on the console before you restart.
@Clt49er Iām not at all sure that I have a solution, but I do have a question. What post processor are you using to create the gcode?