Hi. I’m Adrian. I’m polish and I’ve got my xcarve a month. I did some successful cuts already. I make my projects in ArtCam and I love it 
Last project i made. Carving was ok, no issue, but when router goes from home to place when it starts cutting it goes with speed about 10 mm/s ten it speeds up when it starts carving, acts normally.
I send toolpaths from ArtCam to easel so I cant change any settings in easel. Is it an issue with toolpaths in ArtCam? See the picture below.
All works fine if I make a project in easel.
What post processor do you use with ArtCAM?
Check this thread:
https://discuss.inventables.com/t/artcam-post-processors-for-x-carve/33540
I’m using those post processors
Can you post the first 20 lines of the G-code file here?
And your grbl $$ output.
G17
G21
G90
G0 Z11.9720
G0 X0.0000 Y0.0000
M3 S15000
G0 X0.0000 Y0.0000 Z5.0000
G1 X19.6510 Y109.0486
G1 Z-2.4300 F3000
G1 X19.9665 Y108.5971 F2400
G1 X20.0665 Y108.5159
G1 X20.2696 Y108.4061
G1 X21.0550 Y108.2974
G1 X21.6778 Y108.3795
G1 X21.7238 Y108.3956
G1 X21.8249 Y108.4496
G1 X21.9742 Y108.5672
G1 X22.3437 Y108.9877
G1 X22.5198 Y109.3324
G1 X22.6795 Y110.1318
G1 X22.5342 Y110.7267
G1 X22.3784 Y111.0077
G1 X22.0467 Y111.3522
G1 X21.6108 Y111.6325
G1 X20.9760 Y111.7216
G1 X20.3421 Y111.6370
G1 X19.7717 Y111.2680
How to get it? from UGS?
In the Commands tab enter $$ and carriage return. That will display the parameters.
This is the first movement that uses the feed rate, but a feed rate has not been set, so whatever the feed rate happened to be when you started sending the file was in effect.
Most likely the feed rate was not defined (ie 0) and grbl returned an error. UGCS ignores the error and continues to send the file. If there happened to be a slow feed rate set then moving to the first point would be slow and then after the next line is executed the speed of the carve would return to normal.
Once the feed rate gets set in the line G1 Z-2.4300 F3000 then everything returns to normal which is why your carve works ok, however it starts with the second point if the first point was not executed by grbl because there was an error on that line.
It appears that there is an error in the way that ArtCAM generated the G-code as the first G1 line should have had a feed rate associated with it.
1 Like
Thanks for help. It means that my problem has been explained.
Does it mean that next time i generate a toolpath in artcam i need to make sure first movement line has got feedrate value for example G1 X19.6510 Y109.0486 F3000 . Right?
this is the Xcarve post processor in Artcam. is there any way to make it work right?
;
; G - Code configuration file
;
; History
;
; Who When What
; === ======== ========================================
; TM 13/05/99 Written
; BEM 20/05/99 Removed line numbers
; bem 21/03/00 Added DESCRIPTION and FILE_EXTENSION fields
; lem 01/31/2017 Modified for the Inventables X-carve
;
DESCRIPTION = “Xcarve G-Code Arcs (mm) (*.txt)”
;
FILE_EXTENSION = “txt”
;
UNITS = MM
;
; Cariage return - line feed at end of each line
;
END_OF_LINE = “[13][10]”
;
; Block numbering
;
LINE_NUM_START = 0
LINE_NUM_INCREMENT = 10
LINE_NUM_MAXIMUM = 999999
;
; Set up default formating for variables
;
; Line numbering
FORMAT = [N|@|N|1.0]
; Spindle Speed
FORMAT = [S|@|S|1.0]
; Feed Rate
FORMAT = [F|#|F|1.0]
; Tool moves in x,y and z
FORMAT = [X|#|X|1.4]
FORMAT = [Y|#|Y|1.4]
FORMAT = [Z|#|Z|1.4]
; Arc Center Coords
FORMAT = [I|@|I|1.4]
FORMAT = [J|@|J|1.4]
; Home tool positions
FORMAT = [XH|@|X|1.4]
FORMAT = [YH|@|Y|1.4]
FORMAT = [ZH|@|Z|1.4]
;
; Set up program header
;
START = “G17”
START = “G21”
START = “G90”
START = “G0 [ZH]”
START = “G0 [XH] [YH]”
START = “M3 [S]”
;
; Program moves
;
FIRST_RAPID_RATE_MOVE = “G0 [Y] [Z]”
;
FIRST_FEED_RATE_MOVE = “G1 [Y] [Z] [F]”
FEED_RATE_MOVE = “G1 [Y] [Z]”
;
FIRST_CW_ARC_MOVE = “G2 [Y] [I] [J] [F]”
CW_ARC_MOVE = “G2 [Y] [I] [J]”
;
FIRST_CCW_ARC_MOVE = “G3 [Y] [I] [J] [F]”
CCW_ARC_MOVE = “G3 [Y] [I] [J]”
;
; End of file
;
END = “G0 [ZH]”
END = “M5”
END = “G0 X0 Y0”
END = “M30”
If you always want the first move to be at a particular rate then yes. This is a workaround just so you don’t have to change the files. The correct solution would be for ArtCam to be fixed to work correctly.
There may be a setting in ArtCam that you don’t have setup correctly. Since I don’t use the program I can’t speak to that issue.
Change the post processor by adding this line START = “F3000” (or whatever value you pick) as shown below:
START = “G17”
START = “G21”
START = “G90”
START = “G0 [ZH]”
START = “G0 [XH] [YH]”
START = “F3000”
START = “M3 [S]”
1 Like
It Works finally 
Thanks for help It will speed up every next carve
1 Like