G-code error
- allenwg2005
-
Topic Author
- Offline
- Platinum Member
-
Less
More
- Posts: 327
- Thank you received: 4
31 Jul 2015 23:13 #61070
by allenwg2005
G-code error was created by allenwg2005
Hey folks!
Got a question.
Below are two gcode files of a .500 diameter circle, one with a lead-in and one without.
Neither file will load into LCNC.
Error= "Rijk words all missing for arc"
What's the fix for this?
Try and stay cool out there.
Thanks in advance for your help.
Got a question.
Below are two gcode files of a .500 diameter circle, one with a lead-in and one without.
Neither file will load into LCNC.
Error= "Rijk words all missing for arc"
What's the fix for this?
Try and stay cool out there.
Thanks in advance for your help.
Please Log in or Create an account to join the conversation.
- Todd Zuercher
-
- Offline
- Platinum Member
-
Less
More
- Posts: 5007
- Thank you received: 1441
01 Aug 2015 02:23 #61075
by Todd Zuercher
Replied by Todd Zuercher on topic G-code error
Your first G2 line only has an I term, then you have a lot of G2 lines without any I or J. I think the I and J need to be specified on every G2 line even if they are 0 or unchanged from the last line.
The following user(s) said Thank You: allenwg2005
Please Log in or Create an account to join the conversation.
- Todd Zuercher
-
- Offline
- Platinum Member
-
Less
More
- Posts: 5007
- Thank you received: 1441
01 Aug 2015 02:46 - 01 Aug 2015 02:47 #61076
by Todd Zuercher
Replied by Todd Zuercher on topic G-code error
This might work better, you also had a bunch of problems with cutter comp and your lead-in size(s). You might also need to add a lead out.
N1G54G17G20G40G80G90G99
N2G0X0Y0Z1.
N3T1M06
N4(*** T1 *** .250 Carbide Endmill ***)
N5G00X-.25Y0S5200M03
N6G43Z1.H1T1
N7Z.13
N8G1Z0F208.M08
N9G42X0Y0Z-.03F733.4
N9G1X0.125Y0Z-.03F733.4
N10G2X.125Y0I-.125
N11G1X.125Y0
N12Z-.06F208.
N13X.125Y0F733.4
N14G2X.125Y0I-.125
N15G1X.125Y0
N16Z-.09F208.
N17X.125Y0F733.4
N18G2X.125Y0I-.125
N19G1X.125Y0
N20Z-.12F208.
N21X.125Y0F733.4
N22G2X.125Y0I-.125
N23G1X.125Y0
N24Z-.15F208.
N25X.125Y0F733.4
N26G2X.125Y0I-.125
N27G1X.125Y0
N28Z-.18F208.
N29X.125Y0F733.4
N30G2X.125Y0I-.125
N31G1X.125Y0
N32Z-.21F208.
N33X.125Y0F733.4
N34G2X.125Y0I-.125
N35G1X.125Y0
N36Z-.24F208.
N37X.125Y0F733.4
N38G2X.125Y0I-.125
N39G1X.125Y0
N40Z-.27F208.
N41X.125Y0F733.4
N42G2X.125Y0I-.125
N43G1X.125Y0
N44Z-.3F208.
N45X.125Y0F733.4
N46G2X.125Y0I-.125
N47G1X.125Y0
N48Z-.33F208.
N49X.125Y0F733.4
N50G2X.125Y0I-.125
N51G1X.125Y0
N52Z-.36F208.
N53X.125Y0F733.4
N54G2X.125Y0I-.125
N55G1X.125Y0
N56Z-.39F208.
N57X.125Y0F733.4
N58G2X.125Y0I-.125
N59G1X.125Y0
N60Z-.42F208.
N61X.125Y0F733.4
N62G2X.125Y0I-.125
N63G1X.125Y0
N64Z-.45F208.
N65X.125Y0F733.4
N66G2X.125Y0I-.125
N67G1X.125Y0
N68Z-.48F208.
N69X.125Y0F733.4
N70G2X.125Y0I-.125
N71G1X.125Y0
N72Z-.5F208.
N73X.125Y0F733.4
N74G2X.125Y0I-.125
N75G1G40X.125Y0
N76G0Z1.M09
N77G00G49Z5.M05
N78G90X0Y0
N79T1M06
N80M30
Last edit: 01 Aug 2015 02:47 by Todd Zuercher.
The following user(s) said Thank You: allenwg2005
Please Log in or Create an account to join the conversation.
- allenwg2005
-
Topic Author
- Offline
- Platinum Member
-
Less
More
- Posts: 327
- Thank you received: 4
01 Aug 2015 21:16 #61101
by allenwg2005
Replied by allenwg2005 on topic G-code error
Thanks Todd,
I didn't realize LCNC didn't recognize comp insertion with a zero move, most NC machines do.
The lead-in was just me trying dramatic things to see if it would help.
Thanks again, Allen
I didn't realize LCNC didn't recognize comp insertion with a zero move, most NC machines do.
The lead-in was just me trying dramatic things to see if it would help.
Thanks again, Allen
Please Log in or Create an account to join the conversation.
01 Aug 2015 23:21 #61104
by BigJohnT
In order to arrive at the compensated position from the uncompensated position you need to move longer than the tool diameter. I can't imagine how a NC machine can do that without moving and still be in position at all times.
www.linuxcnc.org/docs/2.7/html/gcode/too...:cutter-compensation
JT
Replied by BigJohnT on topic G-code error
Thanks Todd,
I didn't realize LCNC didn't recognize comp insertion with a zero move, most NC machines do.
The lead-in was just me trying dramatic things to see if it would help.
Thanks again, Allen
In order to arrive at the compensated position from the uncompensated position you need to move longer than the tool diameter. I can't imagine how a NC machine can do that without moving and still be in position at all times.
www.linuxcnc.org/docs/2.7/html/gcode/too...:cutter-compensation
JT
Please Log in or Create an account to join the conversation.
- allenwg2005
-
Topic Author
- Offline
- Platinum Member
-
Less
More
- Posts: 327
- Thank you received: 4
01 Aug 2015 23:50 #61107
by allenwg2005
Replied by allenwg2005 on topic G-code error
JT,
Thanks for the reply.
According to other CNC forums, a 0 comp isn't an issue with most machine controls, it's been asserted that this is a LinuxCNC "thing".
I'm no authority on any of this, it's just what I've been told.
Not that it's any big deal, any software will have it's proclivities.
Thanks for the reply.
According to other CNC forums, a 0 comp isn't an issue with most machine controls, it's been asserted that this is a LinuxCNC "thing".
I'm no authority on any of this, it's just what I've been told.
Not that it's any big deal, any software will have it's proclivities.
Please Log in or Create an account to join the conversation.
02 Aug 2015 02:19 #61109
by BigJohnT
Replied by BigJohnT on topic G-code error
Not disputing the "CNC" experts on other forums but my old DX-32 control and IIRC (I'm too lazy to look) my even older Anilam 1100M control require you to make a "approach" move into the compensated path. The DX-32 the "approach" move is the next line after G41/42 and must be equal to or larger than the tool diameter. So it is definitely not a LinuxCNC "thing".
JT
JT
Please Log in or Create an account to join the conversation.
- Todd Zuercher
-
- Offline
- Platinum Member
-
Less
More
- Posts: 5007
- Thank you received: 1441
02 Aug 2015 03:06 #61111
by Todd Zuercher
Replied by Todd Zuercher on topic G-code error
I'll be honest I don't really use cutter comp. CAM takes care of all that for me. If I were coding by hand I would almost certainly use it alot. But I still think proper lead-ins and lead-outs are necessary on most if not all controls to get a proper cut (without gouges) when using cutter comp. Most controls may not require them, to run the code, but they still are needed to make a proper part. Maybe Linuxcnc is trying to be too clever in its attempts to save us from ourselves.
Please Log in or Create an account to join the conversation.
02 Aug 2015 03:24 #61113
by BigJohnT
Replied by BigJohnT on topic G-code error
I'd rather it be clever when I'm being not so clever. It does make sense that the first move after G41/42 has to be at least big enough to get into the compensated position.
JT
JT
Please Log in or Create an account to join the conversation.
- allenwg2005
-
Topic Author
- Offline
- Platinum Member
-
Less
More
- Posts: 327
- Thank you received: 4
02 Aug 2015 07:49 #61116
by allenwg2005
Replied by allenwg2005 on topic G-code error
Speaking for myself, LCNC can have all the quirks it likes!
The fact that it's so flexible and can be adapted to so may different machines makes it worth every dime.
Oh that's right; it's completely free!
I'll put up with whatever “thing” it comes up with for the trade off on the price tag.
Thanks again guys, Allen
The fact that it's so flexible and can be adapted to so may different machines makes it worth every dime.
Oh that's right; it's completely free!
I'll put up with whatever “thing” it comes up with for the trade off on the price tag.
Thanks again guys, Allen
Please Log in or Create an account to join the conversation.
Time to create page: 0.078 seconds