G18 & G19 problems

itsallkuhlmann · Jan 16, 2018

Hi all,

Is there any real advantage to G18,G19 on a 3 axis machine?

I'm getting software limit faults, K values too high for the Z travel on the machine I have. (50mm usable - ish)

N10595 X4.631 Z0 <- stops here with soft limit fault Z axis
N10600 G18 G03 X2.646 I-1.001 K44.931 <- i'm assuming because the K value is too high??
N10605 G01 X2.408 Z-0.355 F50

I've all ready pissed the option off in the post, files aren't that much bigger, but at least they work.

Got me stuffed, am I missing something?

Cheers

machtool · Jan 16, 2018

You should really declare you have some odd ball Kuhlmann Router (Part of your name).With some thing called an Andron 2060 controller.

http://www.e-engraving.com/machines/kuhlmann/Kuhlmann_P25SP.htm

Chance's of finding any one here that's familiar with that controller are slim.

Are there not router Kulmann Forums?

Because your jacking every one off, thinking that's a Fanuc or other commercial control. When you ask a generic G18 / G19 question.

itsallkuhlmann · Jan 16, 2018

machtool said:
You should really declare you have some odd ball Kuhlmann Router (Part of your name).With some thing called an Andron 2060 controller.

http://www.e-engraving.com/machines/kuhlmann/Kuhlmann_P25SP.htm

Chance's of finding any one here that's familiar with that controller are slim.

Are there not router Kulmann Forums?

Because your jacking every one off, thinking that's a Fanuc or other commercial control. When you ask a generic G18 / G19 question.

G18 G19. Its standard G code yeah? Pull ya head in. I've got no patience for dickheads.

SeaMoss · Jan 16, 2018

itsallkuhlmann said:
Is there any real advantage to G18,G19 on a 3 axis machine?

I'm getting software limit faults, K values too high for the Z travel on the machine I have. (50mm usable - ish)

N10595 X4.631 Z0 <- stops here with soft limit fault Z axis
N10600 G18 G03 X2.646 I-1.001 K44.931 <- i'm assuming because the K value is too high??
N10605 G01 X2.408 Z-0.355 F50

I've all ready pissed the option off in the post, files aren't that much bigger, but at least they work.

Got me stuffed, am I missing something?

G02 and G03 need both X and Z values for the endpoint, at least on all the controls I have used. (Or X and Y if you are in the other plane.)

Bobw · Jan 16, 2018

SeaMoss said:
G02 and G03 need both X and Z values for the endpoint, at least on all the controls I have used. (Or X and Y if you are in the other plane.)

Shouldn't need both if you are coming back to the value you are starting at..
Like a helix... You get a whole bunch of this
G3 I1. Z-.1
G3 I1. Z-.2... No X or Y needed.

Is there any real advantage to G18,G19 on a 3 axis machine?

Advantage??

It changes the reference plane.. If you want to do an arc in XZ you NEED G18.
if you want to do an arc in YZ you NEED G19..
Just like if you want to do an arc in XY you NEED G17, though G17 is probably
default and is most likely already in your safety block at the beginning of the
program.

One other problem.. Those points don't work, assuming Z is coming back to zero.
You are .017 off.. Which may or may not work depending on how big of a fudge factor
your control is set up to take.

Also, what are you trying to do? Is that supposed to be an XZ arc at that point?

G3 is *generally* a CCW arc and would put your Z at somewhere around +87.??? at the high
point of the arc.

Mike1974 · Jan 16, 2018

itsallkuhlmann said:
G18 G19. Its standard G code yeah? Pull ya head in. I've got no patience for dickheads.

Welcome to the forum... :rolleyes5:

machtool · Jan 16, 2018

itsallkuhlmann said:
G18 G19. Its standard G code yeah? Pull ya head in. I've got no patience for dickheads.

http://www.practicalmachinist.com/vb/cnc-machining/andron-controller-passwords-reset-343922/

I wasn't the dick head that needed a password, for the ever so popular Andron 2060. Nor called themselves "Its All Kuhlmann".

Any reason, why you don't declare, you have the ever so popular Andronic 2060. How hard would that be?

ALL I FUCKING SUGGESTED, if you have such an odd ball controller, it would be best to declare it. There's no such thing as Standard G-Code, when it comes to the mighty Andronic 2060.

Truth be known. Aren't you some Harry Home Shop Type, that's bought a reject Kuhlmann engraving machine, and want to turn it into a back yard milling machine?

I wasn't the one that wrote this on the initial post.

Is there any real advantage to G18,G19 on a 3 axis machine?

You do know they are different planes? But maybe not. What could the "real" advantage be I wonder. Apart from working in X-Z or Y-Z Planes. Give or take it can only be 90 deg's out. For you Home Shop Harry types, might not make a difference.

Remind us again, how you only have 50mm / 2 inches of Z travel, given the nature of the router you have bought?

All I said was declare that. You have some of the World's best App's Engineers sitting on your door step. Hell bent on wasting their time?

You'd be better off over at CNC Zone. They love this shit.

SeaMoss · Jan 16, 2018

Bobw said:
Shouldn't need both if you are coming back to the value you are starting at..

Old habits die hard ... Had several controls that could only do 90* arcs

And then one that if you were off a couple tenths would continue around in circles forever, getting farther and farther away from where it was supposed to be. Like a lost calf looking for its mommy

I'm not sure what the heck kind of 360* arc our op could be doing in xz tho ?

machtool · Jan 16, 2018

SeaMoss said:
Old habits die hard ... Had several controls that could only do 90* arcs And then one that if you were off a couple tenths would continue around in circles forever, getting farther and farther away from where it was supposed to be.

Perhaps your paper tape's were dirty?

You must be at least 85 for the shit you tell.

itsallkuhlmann · Jan 16, 2018

SeaMoss said:
G02 and G03 need both X and Z values for the endpoint, at least on all the controls I have used. (Or X and Y if you are in the other plane.)

Thanks.
I think I see the problem now. Had a second read of the manual, and yep if no endpoints are set, the control does a full circle. It looks like an issue with the post program.

cheers

SeaMoss · Jan 16, 2018

machtool said:
Perhaps your paper tape's were dirty? You must be at least 85 for the shit you tell.

I kinda like paper tape. Gotta stack of crashed hard drives in the corner that I keep meaning to ddrescue, that never happened with tape ... Hate to spill the beans but I know there's a couple people here who have even older controls than me. Allen-Badley, hydraulic servos, hahahahahahaha :eek:

but I won't fink 'em out

(Actually, what they couldn't do was cross over a quadrant. I think that was fairly common once upon a time)

itsallkuhlmann · Jan 16, 2018

Bobw said:
Shouldn't need both if you are coming back to the value you are starting at..
Like a helix... You get a whole bunch of this
G3 I1. Z-.1
G3 I1. Z-.2... No X or Y needed.

Advantage??

It changes the reference plane.. If you want to do an arc in XZ you NEED G18.
if you want to do an arc in YZ you NEED G19..
Just like if you want to do an arc in XY you NEED G17, though G17 is probably
default and is most likely already in your safety block at the beginning of the
program.

One other problem.. Those points don't work, assuming Z is coming back to zero.
You are .017 off.. Which may or may not work depending on how big of a fudge factor
your control is set up to take.

Also, what are you trying to do? Is that supposed to be an XZ arc at that point?

G3 is *generally* a CCW arc and would put your Z at somewhere around +87.??? at the high
point of the arc.

Sorry mate, I meant advantage as in using g18, g19 interpolation of arcs, rather than having the post processor do it the other way.(lots of code - little lines, don't know the technical term). Is there a difference in quality, finish etc.

I've changed the post file so G18, G19 are no longer used. G17 is not an issue.

sinha · Jan 16, 2018

Arcs can be made on three orthogonal planes only, on a 3-axis machine. G17/G18/G19 selects the plane.
It is not a question of advantage, it is a matter of requirement.

Vancbiker · Jan 16, 2018

@OP..

It is important to state the control type when asking this sort of question. While G17-G19 are fairly "standard", the definition of address values used G02 and G03 vary in some control types.

Some controls define I,J,K as incremental values from the start of the radius to the center.
Some controls define I,J,K as incremental values from the center of the radius to the start point.
Some controls define I,J,K as incremental values from the start of the radius to the center when in incremental mode and as absolute values when in absolute mode.

Without stating your control type can you see that you may get conflicting answers or suggestions?

rainman · Jan 16, 2018

SeaMoss said:
Hate to spill the beans but I know there's a couple people here who have even older controls than me. Allen-Badley, hydraulic servos, hahahahahahaha

but I won't fink 'em out

I'm one of those couple. The first NC (not CNC) machines I ran (Cincinnati) used tape, had no CRT, no keyboard, no Z axis (hydraulic quill, using cams to control depth), manually dialed-in spindle speed (not in program), hydraulic servos, and no feed hold. Only way to stop was to use single block, or hit E-stop.

itsallkuhlmann · Jan 16, 2018

sinha said:
Arcs can be made on three orthogonal planes only, on a 3-axis machine. G17/G18/G19 selects the plane.
It is not a question of advantage, it is a matter of requirement.

Except that it's not.

I have disabled G18 and G19 in the post.

The program for arcs on x,z and y,z are now worked out some other way without using G18,G19. (non interpolating?)
machine works, it's all good, i'm happy. but....

Question was - what advantage have I given up by disabling the generation of these two codes?

Kleinfeldt · Jan 16, 2018

Sometimes a picture helps

%
O0
G18 G40 G80 G90
(TOOL BIT)
()
T1 M6
S1000 M3
G0 G90 G54 X1.3 Y0
G43 Z1. H1
G0 Z0.1
G1 Z0 F8.
G1 X0
G3 X0.7246 Z-1.3315 I0 K-0.87
G2 X0.9918 Z-1.9551 I0.3083 K-0.237
G0 X1.3
Z2.
M9
M30
%

Knob - YouTube

Vancbiker · Jan 16, 2018

itsallkuhlmann said:
.....Question was - what advantage have I given up by disabling the generation of these two codes?

Having your CAM system generate arcs from a large number of short linear moves usually results in a lower quality surface finish than using circular interpolation. Depending on the CNC's memory, you may run into program size limitations and if block processing speed is slow, you might run into feedrate limitations.

Bobw · Jan 16, 2018

Vancbiker said:
Having your CAM system generate arcs from a large number of short linear moves usually results in a lower quality surface finish than using circular interpolation. Depending on the CNC's memory, you may run into program size limitations and if block processing speed is slow, you might run into feedrate limitations.

But if you have a long enough line length, you can get a really cool faceted look.

sinha · Jan 17, 2018

itsallkuhlmann said:
Except that it's not.

I have disabled G18 and G19 in the post.

The program for arcs on x,z and y,z are now worked out some other way without using G18,G19. (non interpolating?)
machine works, it's all good, i'm happy. but....

Question was - what advantage have I given up by disabling the generation of these two codes?

Any specific reason for disliking G18/G19?

G18 & G19 problems

Plastic

Diamond

Plastic

Banned

Diamond

Diamond

Diamond

Banned

Diamond

Plastic

Banned

Plastic

Titanium

Diamond

Cast Iron

Plastic

Plastic

Diamond

Diamond

Titanium

Similar threads