G91.1

G91.1

Postby Dclifton2 » Thu Jun 20, 2013 1:28 am

Aspire addes a g91.1 in their gcode in the Mach arc inch pp. but I can't find a reference to what it's for. Can anyone explained its use
Thank
Don C
Dclifton2
Vectric Wizard
 
Posts: 320
Joined: Sat Feb 13, 2010 9:41 pm
Location: Port Orange Fl.
Model of CNC Machine: home built shopbot clone. CNC lathe

Re: G91.1

Postby PaulRowntree » Thu Jun 20, 2013 2:11 am

The linux cnc guide site is pretty good for codes ...

http://linuxcnc.org/docs/html/gcode/gco ... 90_1-G91_1

G91.1 - incremental distance mode for I, J & K offsets. G91.1 Returns I, J & K to their default behavior.
Paul Rowntree
WarpDriver, StandingWave, Topo and gadgets available at PaulRowntree.weebly.com
PaulRowntree
Vectric Wizard
 
Posts: 1687
Joined: Sun Oct 24, 2010 7:28 pm
Location: Guelph, Ontario
Model of CNC Machine: homebuilt 4'x2' (Mach3+G540)

Re: G91.1

Postby Dclifton2 » Thu Jun 20, 2013 3:00 am

Thanks Paul, I don't understand why you would do incremental moves in an arc or why aspire produces a g90 and then a g91.1 in the next line of code?
Thanks for your help
Don Clifton
Dclifton2
Vectric Wizard
 
Posts: 320
Joined: Sat Feb 13, 2010 9:41 pm
Location: Port Orange Fl.
Model of CNC Machine: home built shopbot clone. CNC lathe

Re: G91.1

Postby PaulRowntree » Thu Jun 20, 2013 3:25 am

G90 is setting absolute positioning, so that a g0 or g1 command really sends the tool to the specified x,y,z coordinates.

The incremental arc is one of the two ways to define an arc, and it turns out to be the more accurate way. Both go from the current position to some new position, but the absolute mode uses I,J = (Xc, Yc) to identify the centre of the arc, while incremental uses I,J = (dX, dY) as offsets from the current position to identify the centre of the arc. Absolute is easier for humans to read, but apparently incremental is less subject to round off errors with the typical 3-4 digits of precision, so it is the preferred mechanism.

EDIT : Here is another interesting site, with a good PDF file download at the top http://machmotion.com/cnc-info/g-code.html
Paul Rowntree
WarpDriver, StandingWave, Topo and gadgets available at PaulRowntree.weebly.com
PaulRowntree
Vectric Wizard
 
Posts: 1687
Joined: Sun Oct 24, 2010 7:28 pm
Location: Guelph, Ontario
Model of CNC Machine: homebuilt 4'x2' (Mach3+G540)

Re: G91.1

Postby Dclifton2 » Thu Jun 20, 2013 3:52 am

Thanks that and the other sites are very usefull but what I'm trying to do is get ride of the choppy motion and have a smoother cut. I can't seem to get aspire to do IJ's except on perfectly round circles on ovals it just does the point to point moves which give a choppy cut.
Thanks for the help
Don Clifton
Dclifton2
Vectric Wizard
 
Posts: 320
Joined: Sat Feb 13, 2010 9:41 pm
Location: Port Orange Fl.
Model of CNC Machine: home built shopbot clone. CNC lathe

Re: G91.1

Postby PaulRowntree » Thu Jun 20, 2013 5:04 am

Ok, then that is the issue. Vectric uses arcs for true circles in a plane, but all other motion is made from g1 moves. But this shouldn't be an issue. If you look at the gcode you can see the distance that the tool moves along the straight segments, and I expect it is very short distances.

How do the previews look?

Are you using Constant Velocity mode on your controller software? CV will smooth out the motion, and is available on mach3 and other systems. Proper use may require tweaking the acceleration settings somewhat to match your machine's capabilities.

My guess is that you will find the issue on the machine side, not Vectric's, and not in the gcode itself.
Paul Rowntree
WarpDriver, StandingWave, Topo and gadgets available at PaulRowntree.weebly.com
PaulRowntree
Vectric Wizard
 
Posts: 1687
Joined: Sun Oct 24, 2010 7:28 pm
Location: Guelph, Ontario
Model of CNC Machine: homebuilt 4'x2' (Mach3+G540)

Re: G91.1

Postby Dclifton2 » Thu Jun 20, 2013 1:10 pm

Thanks, you might be right. I'll take a look at my settings.
Thanks again for the help.
Don Clifton
Dclifton2
Vectric Wizard
 
Posts: 320
Joined: Sat Feb 13, 2010 9:41 pm
Location: Port Orange Fl.
Model of CNC Machine: home built shopbot clone. CNC lathe

Re: G91.1

Postby Adrian » Thu Jun 20, 2013 2:20 pm

Something else that might be worth looking at is the Fit Curves to Selected Vectors tool in Aspire. This will convert (if possible) parts of your design to pure arcs within tolerances that you set.
User avatar
Adrian
Vectric Archimage
 
Posts: 9828
Joined: Thu Nov 23, 2006 2:19 pm
Location: Surrey, UK
Model of CNC Machine: ShopBot PRS Alpha 96x48

Re: G91.1

Postby Dclifton2 » Thu Jun 20, 2013 4:24 pm

Thanks, I have never used that function. I'll give it a try
Thanks
Don
Dclifton2
Vectric Wizard
 
Posts: 320
Joined: Sat Feb 13, 2010 9:41 pm
Location: Port Orange Fl.
Model of CNC Machine: home built shopbot clone. CNC lathe

Re: G91.1

Postby jzarski » Fri Jun 21, 2013 1:19 am

I am experiencing the same issues Don is talking about. No matter where or how I set CV I get the same results. Is there another PP that I can use to help this?

I have tried the following.
G code
G code arc inch
Mach2/3 arc inch

Is there any other one I can try? I find it hard to believe that this is not happening to others. If I type a simple "&" in Vcarve pro and tool path it I get very poor machine results. The machine jerks at every point, no matter how CV is set.

I Need Help :?

John
jzarski
 
Posts: 2
Joined: Wed Sep 21, 2011 10:20 pm
Model of CNC Machine: widgetmaster

Re: G91.1

Postby kilrabit » Fri Jun 21, 2013 1:50 am

In your general config settings, make sure that the distance mode is absolute, and the IJ mode is inc.

Also turn your look ahead lines to 200 or even 400 if using a smooth stepper. This can also improve your CV.

Try turning you shuttle accel to .0004, if your machine used any backlash compensation this will speed up the movements of compensation.




Roy
kilrabit
Vectric Wizard
 
Posts: 487
Joined: Thu Feb 26, 2009 4:04 am
Location: Uvalde Texas

Re: G91.1

Postby jzarski » Fri Jun 21, 2013 8:41 pm

I got it all figured out.

I would like to personally thank Don (dclifton) for taking the time to help me figure it out.
Also thank you to Roy, the look ahead is what I think fixed the problem. Here is what we did to get it going smooth.

-PP was Mach2/3 Arc inch
-CV was on but nothing else checked in the CV box in general config.
-Set look ahead to 200 (this I think is the key to the issue)
-Set my Accel to 13 from 20. 20 was good when you manually jog but when running a file 13 seemed to be the ticket. This setting is contingent on your machine. I highly recommend playing with it to see what best suits your machine.

Hope this helps someone out. Again thank you Don for all your help. :lol:

John
jzarski
 
Posts: 2
Joined: Wed Sep 21, 2011 10:20 pm
Model of CNC Machine: widgetmaster


Return to Control Software related questions

Who is online

Users browsing this forum: No registered users and 3 guests