G41/G42 discussion.

Post anything you want to discuss with others about the software.

Re: G41/G42 discussion.

Postby Battwell » Wed Feb 28, 2018 4:21 pm

lovely to see no gouge- on the original code i posted.- so far- the only "hobby" software ive seen to get this right . well done
getting there!!!
Battwell
 
Posts: 233
Joined: Sun Sep 25, 2016 7:39 pm

Re: G41/G42 discussion.

Postby cncdrive » Wed Feb 28, 2018 11:16 pm

Thanks. :)
cncdrive
Site Admin
 
Posts: 1862
Joined: Tue Aug 12, 2014 11:17 pm

Re: G41/G42 discussion.

Postby Vmax549 » Tue Mar 13, 2018 5:20 pm

Somethings are just a work of ART.

That is a G42 Spiraling ARC leadin . Then spiral down the circle and cleanup pass then spiral back up . Finishing with an inspiring Spiral ARC leadout.

I would say that is about a 10 in the art world.

Thanks Balazs. :D

G0 X0 Y0 Z1 F20
G0 X2 Y2
G0 X3 Z1
G42 D1
G2 X4 Y2 Z-.1 R.5 F20
G2 X4 I-2 J0 F40 Z-.2
G2 X4 I-2 J0 F40 Z-.3
G2 X4 I-2 J0 F40 Z-.4
G2 X4 I-2 J0 F40 Z-.5
G2 X4 I-2 J0 F40 Z-.5 ( cleanup)
G2 X4 I-2 J0 F40 Z0.000
G40
G2 X3 Z1 R.5 F20
G0 X2Y2
M30


(;-) TP
Attachments
G42_ARC_Spiral_leadin_leadout.jpg
Vmax549
 
Posts: 922
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: G41/G42 discussion.

Postby Vmax549 » Wed Mar 14, 2018 1:09 pm

G41/42 and Run From Here.

Be carefull here as teh RFH does not fully understand restarting with G41/42. It will restart without Tool Comp then recomp as it goes. So be warned if you try it.

(;-) TP
Vmax549
 
Posts: 922
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: G41/G42 discussion.

Postby Vmax549 » Wed Mar 14, 2018 2:47 pm

OK teh solutions for using RFH with tool Comp.

You must go back to the last G41/42 called and restart from that point. That way the ToolComp is applied correctly and all is well.

(;-) TP
Vmax549
 
Posts: 922
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: G41/G42 discussion.

Postby ger21 » Wed Mar 14, 2018 3:04 pm

I was going to say that there's no way the Run from here can work without going back. :)
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 960
Joined: Sat Sep 03, 2016 2:17 am

Re: G41/G42 discussion.

Postby Vmax549 » Wed Mar 14, 2018 3:33 pm

Actually it will run BUT it applies the Tool Comp corrections during the current block motion which causes an OOPs.

I think it can be corrected so it DOES work correctly from the current block but that is up to UCCNC.

It WOULD be nice if it worked correctly.

(;-) TP
Vmax549
 
Posts: 922
Joined: Sun Nov 22, 2015 3:25 am
Location: USA

Re: G41/G42 discussion.

Postby Dan911 » Sun Mar 25, 2018 12:35 pm

g42 prob.JPG


Is this a bug???


I created a simple part with my plugin, I used G42 for tool compensation on first cut for a square than code gives a G40 and continues with pocketing a circle and a canned cycle for 4 holes in each corner.

If I remove the G42 the code runs fine but with no tool compensation for square.
if I remove the canned cycle the code runs fine.
if I use absolute mode for canned cycle code runs fine.

If I scroll through the code it shows the way I expected, but running the code the canned cycle follows glitch path.

The active line shows G40 model at canned cycle.

Code: Select all
( Quick Cam Wizards Version 1.003)
G00G17G90G40G49G80

( Create a Part or Path Wizard 1.003)

X1.75 Y1.75
G1 G42 D1 X2 Y2 F200
M6( Tool 1 Diameter .25 )
S12222 M3
Z-0.25 F100
G1  F200
G91
G1X12 Y0
G1X0 Y12G1X-12 Y0
G1X-0 Y-12
G40G90
G0 Z1

( Cut or Pocket a Circle Wizard 1.003)

G1X8 Y8 F222
M6(Tool Diameter .25)
S12222 M3
G91
G1 Z-1.25F123
G1 Y0.125 F222
G3 Y0 I0  J-0.125
G1 Y0.125 F222
G3 Y0 I0  J-0.25
G1 Y0.125 F222
G3 Y0 I0  J-0.375
G1 Y0.125 F222
G3 Y0 I0  J-0.5
G1 Y0.125 F222
G3 Y0 I0  J-0.625
G1 Y0.125 F222
G3 Y0 I0  J-0.75
G1 Y0.125 F222
G3 Y0 I0  J-0.875
G1 Y0.125 F222
G3 Y0 I0  J-1
G1 Y0.125 F222
G3 Y0 I0  J-1.125
G1 Y0.125 F222
G3 Y0 I0  J-1.25
G1 Y0.125 F222
G3 Y0 I0  J-1.375
G1 Y0.125 F222
G3 Y0 I0  J-1.5
G1 Y0.125 F222
G3 Y0 I0  J-1.625
G1 Y0.125 F222
G3 Y0 I0  J-1.75
G1 Y0.125 F222
G3 Y0 I0  J-1.875
G1 Y0.125 F222
G3 Y0 I0  J-2
G1 Y0.125 F222
G3 Y0 I0  J-2.125
G1 Y0.125 F222
G3 Y0 I0  J-2.25
G1 Y0.125 F222
G3 Y0 I0  J-2.375
G3 Y0I0  J- 2.375F
G0 Z1.25
G1Y-2.375
G1 Z-1.5F123
G1 Y0.125 F222
G3 Y0 I0  J-0.125
G1 Y0.125 F222
G3 Y0 I0  J-0.25
G1 Y0.125 F222
G3 Y0 I0  J-0.375
G1 Y0.125 F222
G3 Y0 I0  J-0.5
G1 Y0.125 F222
G3 Y0 I0  J-0.625
G1 Y0.125 F222
G3 Y0 I0  J-0.75
G1 Y0.125 F222
G3 Y0 I0  J-0.875
G1 Y0.125 F222
G3 Y0 I0  J-1
G1 Y0.125 F222
G3 Y0 I0  J-1.125
G1 Y0.125 F222
G3 Y0 I0  J-1.25
G1 Y0.125 F222
G3 Y0 I0  J-1.375
G1 Y0.125 F222
G3 Y0 I0  J-1.5
G1 Y0.125 F222
G3 Y0 I0  J-1.625
G1 Y0.125 F222
G3 Y0 I0  J-1.75
G1 Y0.125 F222
G3 Y0 I0  J-1.875
G1 Y0.125 F222
G3 Y0 I0  J-2
G1 Y0.125 F222
G3 Y0 I0  J-2.125
G1 Y0.125 F222
G3 Y0 I0  J-2.25
G1 Y0.125 F222
G3 Y0 I0  J-2.375
G3 Y0I0  J- 2.375F
G0 Z1.5
G90
 
(Rectangular Hole Pattern Wizard 1.03 )
(Width X=11 Length Y=11)

G0 Z1
G0 X2.5Y2.5
M6
G91
S12000 
G98 G81 Z-.5 R.125 F15000
Y11
X11
Y-11

G80G90
G0 Z1


Dan
Dan911
 
Posts: 305
Joined: Mon Oct 31, 2016 1:22 am
Location: USA

Re: G41/G42 discussion.

Postby ger21 » Sun Mar 25, 2018 1:22 pm

The picture you show looks different from what I see, as I see two comped toolpaths in yours, but I only see one?
But yes, the drilling goes out into space.

You have a formatting issue in there on this line, which should be two lines.

G1X0 Y12G1X-12 Y0
Gerry
UCCNC 2017 Screenset - http://www.thecncwoodworker.com/2017.html
ger21
 
Posts: 960
Joined: Sat Sep 03, 2016 2:17 am

Re: G41/G42 discussion.

Postby dezsoe » Sun Mar 25, 2018 1:28 pm

Dan,

There are two lines with syntax error:

Code: Select all
(line 64)
G3 Y0I0  J- 2.375F

(line 106)
G3 Y0I0  J- 2.375F
dezsoe
 
Posts: 420
Joined: Sun Mar 12, 2017 4:41 pm
Location: Csörög, Hungary

PreviousNext

Return to General discussion about the UCCNC software

Who is online

Users browsing this forum: No registered users and 3 guests