somewhere from vcarve pro to the grbl is wrong. I can carve just fine from easel but when I have to send Gcode from Chilipeppr or UGS the toolpath goes off the reservation. (both do close to the same thing) It looks like its trying to carve the basic shape of the project but all in all its an EPIC FAIL. Any info on this would help and please remember I know nothing about software and coding.
It sounds like you might be shifting between mm and inches.
I use VCarve Pro and UGS all the time with no problem,
I thought that was the problem too but the project was drawn in inches and then the toolpath was saved in inches. (x carve (inch) *.gcode). is there something I need to change in UGS?
Open up the gcode file in a text editor and make sure somewhere at the beginning, before the cutting starts, there is a G20 code. The G20 tells the gcode sender to use inches.
@BillArnold @ErikJenkins thank you! Ill give it a try in the morning and get back to you.
1 Like
You may need to edit / change the post processor you are using to generate your G Code.
You want to make sure you have it set your units
G20 (inch)
G21 (mm)
and your addressing mode
G90 (absolute)
G91 (incremental)
I have noticed that when using UGS to manually control the XC it does so in incremental mode.
So if your G-code filed does not switch it back to absolute mode the cut will go off the rails pretty quickly.
Ok here is the update:: I did make sure everything was in inches by using the g20 code and that helped a lot. Now its running like its supposed to for a small amount of time and then it just starts dropping the z and cutting too deep for the bit to keep up. Is there a difference between grbl.gcode and xcarve .gcode? I have tried them both ad they seem to act the same. I will try the G90 command next. thank you @AaronMatthews
That is not good. Changing mid cut should not be a setting / post processer issue.
(I would still throw a G90 in your header just to be safe)
That sounds like it is missing steps when it is raising the z axis up.
V wheels could be too tight. You may need to lube the acme screw.
Or bump the current on your z axis.
Are you using a collet adaptor? The first collet adaptor I got for mine was no good so as it cut the bit would slip and stick out longer as the cut went on.
FYI here is the modified VCarve post processor I am using:
(I run mine in metric so mm are used instead of inches)
+================================================
+
- Vectric machine output configuration file
+================================================
+
- History
- Who When What
- ======== ========== ===========================
- Tait L. 05/07/2015 Written
- L2Hench 17/08/2015 Added G90 (Absolute Addressing) to header
- L2Hench 19/08/2015 Added M05 (Spindle Stop) to footer
- L2Hench 19/08/2015 Added M09 (Coolant Stop) to footer
- L2Hench 03/02/2016 Removed T1M6 (Tool Change) from header
+================================================
POST_NAME = “Kaiju_Carve (mm) (*.gcode)”
FILE_EXTENSION = “gcode”
UNITS = “MM”
±-----------------------------------------------
- Line terminating characters
±-----------------------------------------------
LINE_ENDING = “[13][10]”
±-----------------------------------------------
- Block numbering
±-----------------------------------------------
LINE_NUMBER_START = 0
LINE_NUMBER_INCREMENT = 10
LINE_NUMBER_MAXIMUM = 999999
+================================================
+
- Formating for variables
+================================================
VAR LINE_NUMBER = [N|A|N|1.0]
VAR SPINDLE_SPEED = [S|A|S|1.0]
VAR FEED_RATE = [F|C|F|1.1]
VAR X_POSITION = [X|C|X|1.4]
VAR Y_POSITION = [Y|C|Y|1.4]
VAR Z_POSITION = [Z|C|Z|1.4]
VAR ARC_CENTRE_I_INC_POSITION = [I|A|I|1.4]
VAR ARC_CENTRE_J_INC_POSITION = [J|A|J|1.4]
VAR X_HOME_POSITION = [XH|A|X|1.4]
VAR Y_HOME_POSITION = [YH|A|Y|1.4]
VAR Z_HOME_POSITION = [ZH|A|Z|1.4]
+================================================
+
- Block definitions for toolpath output
+================================================
±--------------------------------------------------
- Commands output at the start of the file
±--------------------------------------------------
begin HEADER
“G17”
- XY Plane selection +
“G21”
- Programming in millmeters (mm) +
“G90”
- Absolute Programing +
“G0 [ZH]”
- Rapid Move Z axis to Start Position +
“G0 [XH] [YH] [S] M3”
- Rapid Move X axis to Start Position, Move Y axis to Start Position, Speed (RPM), Spindle ON +
±--------------------------------------------------
- Commands output for rapid moves
±--------------------------------------------------
begin RAPID_MOVE
“G0 [X] [Y] [Z]”
±--------------------------------------------------
- Commands output for the first feed rate move
±--------------------------------------------------
begin FIRST_FEED_MOVE
“G1 [X] [Y] [Z] [F]”
±--------------------------------------------------
- Commands output for feed rate moves
±--------------------------------------------------
begin FEED_MOVE
“G1 [X] [Y] [Z]”
±--------------------------------------------------
- Commands output for the first clockwise arc move
±--------------------------------------------------
begin FIRST_CW_ARC_MOVE
“G2 [X] [Y] [I] [J] [F]”
±--------------------------------------------------
- Commands output for clockwise arc move
±--------------------------------------------------
begin CW_ARC_MOVE
“G2 [X] [Y] [I] [J]”
±--------------------------------------------------
- Commands output for the first counterclockwise arc move
±--------------------------------------------------
begin FIRST_CCW_ARC_MOVE
“G3 [X] [Y] [I] [J] [F]”
±--------------------------------------------------
- Commands output for counterclockwise arc move
±--------------------------------------------------
begin CCW_ARC_MOVE
“G3 [X] [Y] [I] [J]”
±--------------------------------------------------
- Commands output at the end of the file
±--------------------------------------------------
begin FOOTER
“G0 [ZH]”
- Rapid Move Z axis to Start Position +
“G0 [XH] [YH]”
- Rapid Move X and Y axis to Start Position +
“M05”
- Spindle Stop +
“M09”
- Coolant OFF +
“M30”
- End of program +
i went back to easel and everything is still cutting fine so it don’t seem to be the V wheels. Easel runs it a lot slower then V carve pro so I tried to slow down the feed rate ( in vcarve pro) but it didn’t seem to slow it down. Let me look to see what a good feed rate is and how to change it.
What feed speeds are you using in VCarve?
Because it uses a screw the max speed on the Z axis is much slower than for the X and Y
The max plunge speed is 500mm/min (19.685 inch/min)
I was running mine way too high. I am not sure if GRBL is smart enough to ignore feed rates that exceed the machine’s max but I adjusted all my tool setting anyway.
ok I finally had a good test run. I was on the default setting for feed rate that was 100mm/sec. I changed that all the way down to 5 inches/min and it did not seem any slower and still had a bad test run. I was cutting .25 inch depth over 2 passes. I changed that to .25 inch over 4 passes and that seem to fix it. Im sure this dewalt 611 should be able to handle more then that though. still not sure whats wrong but now I think its the machine or the feed rate and not the code.
@ErikJenkins @BillArnold @AaronMatthews Ok finally got it running smooth. I cant thank you guys enough for the help. I don’t think I could have done it without you.
2 Likes