[lclee]

G01 X3 Y0
G02 X5 Y5 I0 J0

The GCode is wrong.
It begins with a radius of 3, and ends with a radius of 5.

What is the expected behavior for this code?
Is the CAM program supposed to halt on some sort of data check?
How close do the starting and ending radii have to be?

Is it supposed to run until either the X or Y coordinates match?
That won't happen in the G Code above.

What would EMC or Mach do?

Thanks
Larry

[dcoupar]

G01 X3 Y0
G02 X5 Y5 I0 J0

The GCode is wrong.
It begins with a radius of 3, and ends with a radius of 5.

What is the expected behavior for this code? What machine/control?
Is the CAM program supposed to halt on some sort of data check?What CAM program?
How close do the starting and ending radii have to be?

Is it supposed to run until either the X or Y coordinates match?
That won't happen in the G Code above.

What would EMC or Mach do?

Thanks
Larry

Can you also post a couple of program blocks before and after the 2 you posted?

[lclee]

Is this what you mean?

I'm just writing this code on the screen, it hasn't been tested.
Travel Height is a 1"
Cutting Height is 0"

G20
G90
F20
G17
G00 Z1
M03
G01 Z0
G01 X3 Y0
G02 X5 Y5 I0 J0
G00 Z1
G00 X0 Y0
M05
M30


Also to correct my original post,
I said the second radius was 5 inch,
and actually it was 7 inches.

Larry

[lclee]

The question is not really about any specific machine
or particular CAM program. It's about what the proper behavior
should be. I'm currently using KCAM, but considering moving
to EMC or Mach which is why I asked about those programs.

I always find my misteaks after I hit send!

G20
G90
F20
G17
G00 Z1
M03
G00 X3 Y0
G01 Z0
G02 X5 Y5 I0 J0
G00 Z1
G00 X0 Y0
M05
M30

[dcoupar]

The question is not really about any specific machine
or particular CAM program. It's about what the proper behavior
should be. I'm currently using KCAM, but considering moving
to EMC or Mach which is why I asked about those programs.

I always find my misteaks after I hit send!

G20
G90
F20
G17
G00 Z1
M03
G00 X3 Y0
G01 Z0
G02 X5 Y5 I0 J0
G00 Z1
G00 X0 Y0
M05
M30

"Proper behavior" is very likely machine/control dependent, which is why I asked. Some controls interpret I and J as absolute coordinates of the circle center, and some interpret I and J as an incremental distance from the start-point of the arc to the center.

My assumption is your example would produce a curve (possibly a helix) with a starting radius of 3.0 and an ending radius of 7.0711, both of which are centered at 0,0. See attached .jpg.

[lclee]

I appreciate that there aren't formal standards for G Code.

I didn't know that G02/G03 could work with anything other than a constant radius, therefore a circle or a portion of circle (arc).

Good to know.

Thanks for the information.
Larry

[dcoupar]

I appreciate that there aren't formal standards for G Code.

I didn't know that G02/G03 could work with anything other than a constant radius, therefore a circle or a portion of circle (arc).

Good to know.

Thanks for the information.
Larry

There ARE formal standards for G Code, but they were written a long time ago, and things have changed since then. Not all builders honor the standard in any case.

I'm not sure that you will get that curve on a functional CNC control. You may get a semi-circle the a line to the end point. You may get alarms. You may get vapor lock. Again, I'm sure it depends on the control.

If your post processor output this code, I'd ask for my money back.

[BobWarfield]

That code should alarm on most any control, whether in incremental or absolute IJK mode. Having a different distance from one end point to the center from the other is not permitted and is a very common alarm to encounter.

Having it be off by 5 units is quite a lot. Many controls will have a parameter that lets you set the tolerance, but I would not expect it to be productive to allow that much difference.

It's not a helix, because there is no change in Z from one endpoint to the next on the arc.

You can check this in many g-code simulators, I used G-Wizard. With a simulator, it's easy to play with different options like absolute vs relative IJK to see the effect. G-Wizard displays this information about the arc on line 9:

G02: Clockwise circular interpolation (move in a circular arc at feed speed)
Distance from last move to center = 3.0000
Distance from this move to center = 7.0711
Arc endpoint: 3.0000, .0, .0
Arc center coordinates: .0, .0, .0, radius = 3.0000 (determined by IJK)
Arc angles: .0 to .0(.0 degrees total)

Time: 03.2
ERROR: Distance from each arc endpoint to center differs by 4.0711, more than allowable tolerance.

Mach3 will flag it as an error, "Radius from end of arc differs from radius to start."

Cheers,

BW

[Mzones]

Iclee

This is a backlash issue.
First measure with a dial indicator, then reset backlash compensation in
configuration/backlash. Also enable circle backlash compensation.
This appears to be mostly in the X axis.
You either have end play in the drive screw, and/ or the nut is worn.
Hope this helps you

Mike

[Khalid]

This may be Z-axis less stiffness or tool deflection. so must see these two things too...

[Mzones]

I don't know what's happening but this is not the thread I posted my reply.
Also kahlid's response to my previous post wasn't posted here either.
kahlid Sure these could be part of the problem.
The main problem if you can find what we looked at last night, or
remember. In the last two attachments it was obvious that that particular
example was cut CCW.

Hi, I also have an SX3 that just recently converted to CNC and am seeing the same issues with circles (arcs), I don;t know if it is a mechanical issue or a Mach3 issue. The tolerances between the straight contours in some of the pockets are good +/- 0.02mm but when it comes to doing circles, arcs, ellipses or anything round there is something really wrong. The error seems to be symmetric or when there is a change in direction but in different quadrants (1-3 or 2-4), I replaced the stepper couplings to helical zero-backlash with no luck, still see the same issue.

This was posted at least 3 times 2 came from Australia and 1 from here in the USA
They were the exact same post. Posted by different people different people.


Maybe one of these posts, and got deleted.

[Fredasiong]

Mike,

How and where do you adjust the backlash in emc2. See attached photos:

Attachment 233290


Thanks

[TRMInt]

@op G-code - Wikipedia, the free encyclopedia as others have said not everyone works to this.

G01 linear move to 3,0
G02 Circular move - explanations all over but this is good enough - G-Code Tutorial: Arcs With G02 and G03