G-code error

allenwg2005
Offline
Elite Member

11 years 3 months ago #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.

Attachments:

Please Log in or Create an account to join the conversation.

Todd Zuercher
Offline
Platinum Member

11 years 3 months ago #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

11 years 3 months ago - 11 years 3 months ago #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.

Code:

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: 11 years 3 months ago by Todd Zuercher.

The following user(s) said Thank You: allenwg2005

Please Log in or Create an account to join the conversation.

allenwg2005
Offline
Elite Member

11 years 2 months ago #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

Please Log in or Create an account to join the conversation.

BigJohnT
Offline
Administrator

11 years 2 months ago #61104 by BigJohnT

Replied by BigJohnT on topic G-code error

allenwg2005 wrote: 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
Offline
Elite Member

11 years 2 months ago #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.

Please Log in or Create an account to join the conversation.

Time to create page: 0.169 seconds