Hello Guest it is March 29, 2024, 02:43:50 AM

Author Topic: The Arc Command  (Read 12421 times)

0 Members and 1 Guest are viewing this topic.

Re: The Arc Command
« Reply #10 on: February 23, 2016, 01:08:38 PM »
Two things have me confused about the G90 and G91.1 commands. I see these parameters are set in Mach3 using Config|General Config... It is my understanding that these parameters are superseded by the G-code. So if I leave out either of these commands, wouldn't Mach3 just default to the Config page?

I'm also still confused about the difference between G90 and G91.1. It appears they do different things so are not in conflict. G90 is for axis movement. G91.1 is for IJK movement.

Help!

Rick

Offline ger21

*
  • *
  •  6,295 6,295
    • View Profile
    • The CNC Woodworker
Re: The Arc Command
« Reply #11 on: February 23, 2016, 01:27:24 PM »
Quote
So if I leave out either of these commands, wouldn't Mach3 just default to the Config page?
Yes. But if your code is expecting something other than what's in the config page, then what Mach3 cuts won't be what you were expecting.

Quote
It appears they do different things so are not in conflict.

They are in the same modal group, so the g-code interpreter only reads on of them per line. It's not that they confict, but rather, one of them is ignored. If they are on separate lines, they work fine.

G90
G91.1
Works fine.

G90 G91.1
does not.
Gerry

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

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

Offline stirling

*
  • *
  •  2,188 2,188
  • UK
    • View Profile
    • www.razordance.co.uk
Re: The Arc Command
« Reply #12 on: February 23, 2016, 01:41:35 PM »
Quote from: Tweakie.CNC link=topic=32004.msg222712#msg222712
They are both used in LinuxCNC as well.

Again - happy to be corrected but I think I'm right in saying that Mach3 and LinuxCNC share some of the same code base (particularly I think - the interpreter) so that's probably why.

I'm also still confused about the difference between G90 and G91.1. It appears they do different things so are not in conflict. G90 is for axis movement. G91.1 is for IJK movement.

This is what I was trying to get at in Reply #6. I think it's just a Mach3 (and possibly LinuxCNC) cockup. i.e. they've ended up in the same modal group but they shouldn't be.

Gerry's mention that they are NOT in the same group in Mach4 would tend to back this up.

Offline BR549

*
  •  6,965 6,965
    • View Profile
Re: The Arc Command
« Reply #13 on: February 23, 2016, 01:45:41 PM »
HIYA Rick You also need to understand that the G90.1 and G91.1 are modal . If you set it once it will stay there until you reset it . The config page values are just for startup modes so that MACH# will startup in a preconfigured mode as you define it to be.

A cam or OP can program arcs in many different ways so WHen you DO you also have to specifc to MAch3 in Gcode teh Modes you used to do teh arc be it INC or ABS or Inc IJ or Abs IJ or any combination of teh mentioned modes.  When you program the arc YOU also have to tell teh control HOW you did it so it understands how to MOVE as you intended.

As long as you never CALL to change it it will always be the same as config. But once you call it in a program it switches to the Called mode as they are modal calls.

The problem with G90 G91.1 is there were BOTH internally placed in teh same modal GROUP. This was actual a BUG that was never fixed. So that being you cannot call both on the same line as one will be ignored.

(;-) TP
Re: The Arc Command
« Reply #14 on: February 23, 2016, 04:37:14 PM »
I'm a bit slow on the uptake, but now do understand the concept of Modal. I also proved to myself that with G90 and G91.1 in the same block, G90 causes Distance Mode to be set Absolute but then it is put back to the default value when Mach3 finds G91.1. Since my default values were Distance Mode: Absolute and IJ Mode: Incremental, it all worked for the wrong reason. I'm correctly the article now and will publish the update soon.

Thanks to all that helped me understand this bowl of spaghetti!

Rick
Re: The Arc Command
« Reply #15 on: February 23, 2016, 04:59:44 PM »
OK, I have updated the article. Please let me know if I got anything wrong.

Thanks!

Rick

http://rick.sparber.org/ARC.pdf

Offline BR549

*
  •  6,965 6,965
    • View Profile
Re: The Arc Command
« Reply #16 on: February 23, 2016, 06:30:41 PM »
If I may make a comment when you write gcode as an example it is always best to define teh values in teh normal format and order.  Yes it is OLD school AND some controller can ONLY take a certain format but it does read  much better in my opinion.

Now teh controller will load in Line elements in the order it was programmed to do so to IT order does not mean much But for reading purposes it makes it more clear.

You articles are very good by the way. And will be very helpful to new users.

G02 X0.000 Y0.000 I0.000 J0.000  F123

Instead of

G2 X0 Y0 I0 J0 F123

Just a thought, (;-) TP
Re: The Arc Command
« Reply #17 on: February 23, 2016, 06:46:29 PM »
Not saying its wrong, but .....

Mach3 doesn't put it anywhere. Its skipped over and left in whichever state it is currently in. Could be the default, but not necessarily.

Absolute, or Incremental because that is its current state


Re: The Arc Command
« Reply #18 on: February 23, 2016, 07:03:13 PM »
Hopefully I am moving closer to the truth. Here is the corrected text: http://rick.sparber.org/ARC.pdf

Thanks,

Rick
Re: The Arc Command
« Reply #19 on: February 24, 2016, 02:31:34 PM »
I continue to learn about arcs and now see that there is NOT a bug in Mach3 related to the XZ plane. See page 3 of http://rick.sparber.org/ARC.pdf for details.

Rick