Hello Guest it is March 01, 2021, 01:51:15 PM

Author Topic: Radius to end of arc differs from raduius to start line ...  (Read 11561 times)

0 Members and 1 Guest are viewing this topic.

Offline Sam

*
  • *
  •  987 987
    • View Profile
    • hillbillyhilton.com
Re: Radius to end of arc differs from raduius to start line ...
« Reply #10 on: April 23, 2010, 06:59:00 PM »
There is a time limit for modifying posts. This is to ensure that all post are kept for future reference, without worry that they will be deleted or modified, amongst other reasons.
"CONFIDENCE: it's the feeling you experience before you fully understand the situation."

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: Radius to end of arc differs from raduius to start line ...
« Reply #11 on: April 23, 2010, 07:54:25 PM »
I've been creating code with my AutoCAD macro for about 5 years now, and I can honestly say that I've never gotten this error before, unless the wrong IJ mode was set. And I always use 4 decimal places, never more. So the problem is not one of precision.

If Mach3 does different things on different days, you might want to do a complete uninstall and reinstall.
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html
Re: Radius to end of arc differs from raduius to start line ...
« Reply #12 on: April 23, 2010, 08:54:05 PM »
Yes my machine is configured metric that was the reason I thought the feed was slow.
I wrote some wizards that generate multiple arcs and everytime i got that error there was a problem in my maths.

According to mach docs. the acceptable distance difference from start to center and center to final is 0.0002 inch (if inches are being used) or 0.002 millimetre (if millimetres are
being used).

I use incremental I,J most of the time, I agree it is more difficult to read but apparently is more standarized

regards

Offline alenz

*
  •  137 137
    • View Profile
Re: Radius to end of arc differs from raduius to start line ...
« Reply #13 on: April 24, 2010, 01:46:02 AM »
Pete, I too have seen some unexpected results when using Absolute IJ mode. These gcode snippets all run on my machine, even tho the last two should not. Strange that Mach will error on a very small end point error while other times it will allow over ½ inch.

This cuts an arc in Absolute IJ mode, center at X0 Y0.5,  radius 0.5, as expected.

G00 X0 Y0
G01 X0 Y1
G02 X0 Y0 I0 J0.5
G01 X0 Y0
M30

Now change the J to 0.25 and it also runs, but makes a spiral;

G00 X0 Y0
G01 X0 Y1
G02 X0 Y0 I0 J0.25
G01 X0 Y0
M30

For an even more interesting curve change the Y to 0.5;

G00 X0 Y0
G01 X0 Y1
G02 X0 Y0.5 I0 J0.25
G01 X0 Y0
M30

Can anyone else get this code to run? If so maybe a neat way to cut spirals?

I’m running R3.042.027 and should mention this came up while trying to help a poster on another forum.

Al

Offline ger21

*
  • *
  •  6,289 6,289
    • View Profile
    • The CNC Woodworker
Re: Radius to end of arc differs from raduius to start line ...
« Reply #14 on: April 24, 2010, 06:39:02 AM »
Quote
If so maybe a neat way to cut spirals?


Didn't try your code, but yes, you can cut spirals with Mach3. I use this "feature" to do spiral pocketing. Here's an old mesage from Art from the Yahoo group.



Quote
From: "Art Fenerty" <fenerty@artofcnc.ca>
To: <mach1mach2cnc@yahoogroups.com>
Subject: Re: [mach1mach2cnc] Cutting a spiral
Date: Saturday, December 08, 2007 12:26 PM



Mach3 has a hidden feature that allows for
spirals that aren't to large.. A G2/G3 command does not really need to be fully an Arc, its allowed to stretch
about .5 inches in any domain, so a simple series of non arc G2/G3's is really a spiral..

for example, here is a spiral of a .5 stepout each line.. normally an illegal command,
but Mach3 will allow it up to 12.5mm's or .5 inches..

g0x.5y0

g2x1Y0I0J0
g2x1.5Y0I0J0
g2x2Y0I0J0
g2x2.5Y0I0J0
g2x3Y0I0J0
g2x3.5Y0I0J0
g2x4Y0I0J0
g2x4.5Y0I0J0
g2x5Y0I0J0
Gerry

2010 Screenset
http://www.thecncwoodworker.com/2010.html

JointCAM Dovetail and Box Joint software
http://www.g-forcecnc.com/jointcam.html

Offline kf2qd

*
  •  124 124
    • View Profile
Re: Radius to end of arc differs from raduius to start line ...
« Reply #15 on: April 24, 2010, 09:30:17 PM »
I started out in the machine shop many years ago running a LeBlond Tape Turn Regal. The GE 550T control handled errors in arcs by completing the arc and then moving to the end point. A few times i manually programmed and arc wrong and tried to make a fillet and then move through the part parallel to the spindle. Or radius the outside corner and turn the OD in 1 G02 move.

I will have to look into converting my VB code in my CAD program to produce incremental IJ.

In my experience it was some of the older controls that used incemental IJ, but the machines I have run all used IJ mode as set by G90 or G91.