Hello Guest it is October 22, 2019, 11:18:32 PM

Author Topic: Mach3 4.0 Rev Update  (Read 43314 times)

0 Members and 1 Guest are viewing this topic.

Re: Mach3 4.0 Rev Update
« Reply #40 on: August 16, 2009, 10:02:50 PM »
Where can I find MY very own G-Code expert?   ;D  Nice to see you back here Brian!!!

Sid

Offline cnc-it

*
  •  153 153
    • View Profile
Re: Mach3 4.0 Rev Update
« Reply #41 on: September 05, 2009, 05:08:09 PM »
On the subject of cutter comp with the new version of Mach, will it only work on linear lead in/out or can I use arc lead in/out with G41 G42..?
My Fanuc machines will do cutter comp on linear and arc leads..

Thanks, John
Re: Mach3 4.0 Rev Update
« Reply #42 on: September 05, 2009, 08:02:20 PM »
I have not added the arc lead in and out as I can find NO docs on how it should be done.. if you can show me how it should work in a fanuc manual I will think about adding it.. I think you will find that they add a move to get to the right Rad and then just do an Arc.. The Comp is not taken out in the arc move.. (that would be a spiral not an arc.. )

Thanks
Brian
Fixing problems one post at a time ;)

www.newfangledsolutions.com
www.machsupport.com

Offline cnc-it

*
  •  153 153
    • View Profile
Re: Mach3 4.0 Rev Update
« Reply #43 on: September 06, 2009, 06:23:28 AM »
Yes I think you are right Brian now I come to think of it..I will have a look through my Fanuc manuals and put some of my code up later..
Beacause I always put arc lead in/out on my Cadcam I was presuming thats where it puts the G41/ G42  but I will check for sure..

John.
Re: Mach3 4.0 Rev Update
« Reply #44 on: September 06, 2009, 08:57:09 AM »
Great :)  I like looking at code.. it is my thing LOL
Fixing problems one post at a time ;)

www.newfangledsolutions.com
www.machsupport.com

Offline cnc-it

*
  •  153 153
    • View Profile
Re: Mach3 4.0 Rev Update
« Reply #45 on: September 06, 2009, 09:58:29 AM »
Brian here is some of my code with the G41 and the  D23 which is the radius offset I put in my Fanuc tool offset menu in slot 23.
It looks like it is doing the offset on X,Y before doing the radius as you thought ;)

The cadcam only does cutter comp on finish passes. It produces the finish path on the centre line of the tool and lets the Fanuc move the tool over as is the norm.

For the rough path it offsets the tool by using the tool radius set in the cadcam tool library and also leaves the correct ammount which I have chosen for the finish pass ie. 0.1mm.

For me the rough pass doesn't have to be spot on so if my tool is set a bit big or small in the cadcam it won't matter.

Fanuc 6MB11

N1695G1X-40.483Y-16.697F400.
N1700G3X-31.563Y-18.01I6.758J14.954F293.
N1705G2X9.197Y-19.243I16.617J-124.99F400.
N1710G1G41D23X7.68Y-25.077
N1715G3X8.774Y-25.367I2.929J8.811F200.
N1720G2X40.497Y-36.576I-23.719J-117.633F400.
N1725G3X48.404Y-26.545I3.003J5.765F200.
N1730X38.917Y-20.391I-15.466J-13.455F283.
N1735G2X38.917Y6.391I4.083J13.391F400.
N1740G3X48.404Y12.545I-5.979J19.609F283.
N1745X40.497Y22.576I-4.904J4.266F200.
N1750G2X8.109Y11.236I-55.442J106.424F400.
N1755X6.298Y11.446I-0.576J2.944
N1760G1X-37.499Y31.237
N1765G3X-42.852Y19.391I-2.677J-5.923F200.
N1770G2X-53.148Y-3.391I-5.148J-11.391F400.
N1775G3X-58.501Y-15.237I-2.677J-5.923F200.
N1780G1X-42.991Y-22.247F400.
N1785G3X-30.76Y-24.047I9.266J20.504F294.
N1790G2X11.258Y-25.896I15.814J-118.953F400.
N1795G3X12.375Y-26.075I2.027J9.06F200.
N1800G1G40X13.363Y-20.129F400.
N1805G0Z5.0
N1810G28G91Z0M19
N1815G30G91X0Y0T7M6
N1820G0G90X-8.767Y-7.322S3800M3
N1825G43Z5.0H7M8
N1830Z-4.5
N1835G1Z-5.633F29.

The reason for the slow feeds before the D23 is that it is finishing the bottom of the feature  without cutter comp before the G41  D23 is called to do the wall pass.



John.
« Last Edit: September 06, 2009, 10:02:20 AM by cnc-it »
Re: Mach3 4.0 Rev Update
« Reply #46 on: September 06, 2009, 10:16:17 AM »
Good :) So the code is good as it is.. That is what we like to hear! I took months reading anything and everything I could find on cutter comp. Pleased to see it was not tilting at windmills.
Thanks
Brian
Fixing problems one post at a time ;)

www.newfangledsolutions.com
www.machsupport.com

Offline cnc-it

*
  •  153 153
    • View Profile
Re: Mach3 4.0 Rev Update
« Reply #47 on: September 06, 2009, 10:23:07 AM »
Just looked at the Fanuc 16MB manual and it also has three dimensional cutter comp (hope i'm not opening a can of worms here!!)

I'll quote from the manual:

"Three Dimensional Tool Compensation (G40,G41)

In cutter comp C, two-dimensional offsetting is performed for a selected plane.In three-dimensional tool compensation, the tool can be shifted three-dimensionally when a three dimensional offset direction is programmed.

Start 3d cut comp:

When the following command is executed in cutter comp cancel mode, 3D tool comp is set:

G41 Xp_Yp_Zp_I_J_K_D

Xp: X axis or a parallel axis
Yp: Y axis or a parallel axis
Zp: Z axis or a parallel axis

When cancelling 3D tool comp mode and tool movement at the  same time:

G40 Xp_Yp_Zp_;
or
Xp_Yp_Zp_D00;

When only cancelling the vector

G40;
or
D00 "

John

Re: Mach3 4.0 Rev Update
« Reply #48 on: September 06, 2009, 10:28:22 AM »
No can of worms here.. I am doing 2D not 3d.. If you would like to have 3d comp you will need to use your Cam system...  :)

Thanks
Brian
Fixing problems one post at a time ;)

www.newfangledsolutions.com
www.machsupport.com

Offline cnc-it

*
  •  153 153
    • View Profile
Re: Mach3 4.0 Rev Update
« Reply #49 on: September 06, 2009, 10:29:35 AM »
You're welcome Brian any time. Just looking forward too the new release, it will be great to have the  cutter comp  ;D