Reply with QuoteTool 4 is using the tool 3 length for the tool offset. Is that correct?
How are you measuring your tools?
Mach3 plunging cutter after tool change
I am new with running Mach3 and cnc mill as well (I got used to emc2 and 2 axis lathe). I am still learning and trying to figure out the offsets, axes etc, so please be gentle
I got a code for a part generated by Solid, and I have a few issues with it. One that concerns me the most it that when tool 1 finishes the job, and returns to machine zero for tool change, after inserted tool nr 2 plunges into material. Tool height is set properly, and I believe g54 is also set correctly (otherwise the tool 1 job wouldnt finish its path as its supposed to), and I think it has something to do with offsets. I am too tired to figure it out right now (been tweaking it and figuring it out for last week and few days more, and even if it is most likely something rather simple, I cant see it) so I am asking for help? Maybe the way the code is written has something to do with it?
Second, after the return to machine zero and tool change is made, Z axis moves slowly to some position (in last G1 speed given). I did add a line with g1 movement to speed it up (with double (( )) in the code), maybe that is messing everything up?
All suggestions and help are welcome. Thanks
Similar Threads:
Re: Mach3 plunging cutter after tool change
Tool 4 is using the tool 3 length for the tool offset. Is that correct?
How are you measuring your tools?
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Re: Mach3 plunging cutter after tool change
thank you for pointing that to me Gerry, luckily my program didnt get to that part (last chamfer pass) or there would be more mess to look out for.
I am measuring tools the simplest way I saw, tool 1 is the default tool, off the gauging surface with a piece of paper to pinch in between. after I save it, tool nr 2 is inserted, and its offset measured the same way (I am pretty positive those numbers are correct, looking in the tool library, there are a few mm differences between their offsets) and this move goes more than a 25 mm in the wrong "depth"
Re: Mach3 plunging cutter after tool change
Is your Z axis moving in the right direction? Every tool goes to Z 25 after the tool change.
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Re: Mach3 plunging cutter after tool change
it does, and then dro numbers change and it all goes south (-z direction)
Re: Mach3 plunging cutter after tool change
When the Z DRO reads 25, on the G43 lines, is the tool actually at Z 25? I'm guessing that it's not?
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Re: Mach3 plunging cutter after tool change
played with it a bit more today. rezeroed everything etc, and run a program part by part (except part 1 of the program). it seems that somehow my part offsets were wrong, because now I have a finished part, no plunging, and I havent altered the code parts.
but still, is that how common mach3 gcode should be written?
thanks
Re: Mach3 plunging cutter after tool change
Mach has a bug that causes this problem when the tool number and offset number are in the same line of code if I remember correctly. Change the code to call the H code on a separate line.
Instead of...
N0100 G0 G40 G49 G80 G21 (Initialisation)
N0102 G0 G53 Z0 (Retour aux origines machine)
N0104 G0 G53 X0 Y0
((N0105 G1 G53 X0 Y0 Z0 F200))
N0106 (Outil n° 1 - Diametre 10.0 D1 H1)
N0108 T1 M6 D1 H1
N0110 S2000 M3
N0112 M8
N0114 (F-contour)
N0116 G0 G54 X22.503 Y-17.5
N0118 G43 H1 Z25.
N0120 G0 Z0.5
N0122 G1 Z0. F30
N0124 G41 D1 G1 X27.509 Y-15.91 F35
N0126 G1 X26.771 Y-14.14 Z-0.011
N0128 G1 X25.738 Y-12.525 Z-0.023
N0130 G1 X24.439 Y-11.114 Z-0.034
Make it look like this...
N0100 G0 G40 G49 G80 G21 (Initialisation)
N0102 G0 G53 Z0 (Retour aux origines machine)
N0104 G0 G53 X0 Y0
((N0105 G1 G53 X0 Y0 Z0 F200))
N0106 (Outil n° 1 - Diametre 10.0 D1 H1)
N0108 T1 M6
N0110 D1 H1
N0111 S2000 M3
N0112 M8
N0114 (F-contour)
N0116 G0 G54 X22.503 Y-17.5
N0118 G43 H1 Z25.
N0120 G0 Z0.5
N0122 G1 Z0. F30
N0124 G41 D1 G1 X27.509 Y-15.91 F35
N0126 G1 X26.771 Y-14.14 Z-0.011
N0128 G1 X25.738 Y-12.525 Z-0.023
N0130 G1 X24.439 Y-11.114 Z-0.034
Re: Mach3 plunging cutter after tool change
Just get rid of the D1 H1. They aren't doing anything. The H1 should be with the G43, and the D1 with the G41/G42.
All you want is the T1 M6.
Then the G43 H1
And G41 D1
Gerry
UCCNC 2017 Screenset
[URL]http://www.thecncwoodworker.com/2017.html[/URL]
Mach3 2010 Screenset
[URL]http://www.thecncwoodworker.com/2010.html[/URL]
JointCAM - CNC Dovetails & Box Joints
[URL]http://www.g-forcecnc.com/jointcam.html[/URL]
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Re: Mach3 plunging cutter after tool change
thanks, I will try that!
