V27 Thread Milling Help - No Z code posting

Printable View

03-06-2015, 06:18 PM
hawkeyeammo

V27 Thread Milling Help - No Z code posting

I'm doing a simple thread milling operation and can't seem to get BobCam to post any Z values in the G02 posting routines.

This is a simple 1.2" deep 1/2-13 thread operation. I don't get it. There should be a Z offset for each of the arc operations. What am I doing wrong.

It even shows the z helical interpolation in the graphic on the screen and in the on screen simulation but the posted G Code has no Z offsets in it so the threadmill goes toward the top of the hole and just spins around there! Pulling hair out! Help.

BobCam settings.

Feature: Mill Thread
Diameter: .50
Top of Feature: 1.2
Total Depth: 1.2

Posting
Arc Moves

Thread Mill
Diameter: 0.3720
Protrusion Length: 1.5

Patterns
Top Down
Inside

Parameters
Right Hand
Thread Diameter: 0.5000
Thread Height: 0.0666
Thread Pitch: 0.0769
Threads Per Revolution: 1
Threads Start Angle: 0
Depth: 1.2000

Leads
Lead-In/Lead-Out
Circular
Radius: 0.0500

Resulting GCode

(Machine Setup - 1 Mill Thread)
(FEATURE MILL HOLE - 0.5000)

N18898 T17
N18899 S5140 M03
N18900 G90 G54 X-2.5938 Y-2.625
N18901 G43 H17 D17 Z2.2 M08
N18902 G00 Z1.4
N18903 Z1.3
N18904 G01 Z1.2 F59.11
N18905 X-2.5798 Y-2.575
N18906 G17 G02 X-2.5298 Y-2.625 I0. J-0.05
N18907 X-2.6578 Y-2.625 I-0.064 J0.
N18908 X-2.5298 Y-2.625 I0.064 J0.
N18909 X-2.6578 Y-2.625 I-0.064 J0.
N18910 X-2.5298 Y-2.625 I0.064 J0.
N18911 X-2.6578 Y-2.625 I-0.064 J0.
N18912 X-2.5298 Y-2.625 I0.064 J0.
N18913 X-2.6578 Y-2.625 I-0.064 J0.
N18914 X-2.5298 Y-2.625 I0.064 J0.
N18915 X-2.6578 Y-2.625 I-0.064 J0.
N18916 X-2.5298 Y-2.625 I0.064 J0.
N18917 X-2.6578 Y-2.625 I-0.064 J0.
N18918 X-2.5298 Y-2.625 I0.064 J0.
N18919 X-2.6578 Y-2.625 I-0.064 J0.
N18920 X-2.5298 Y-2.625 I0.064 J0.
N18921 X-2.6578 Y-2.625 I-0.064 J0.
N18922 X-2.5298 Y-2.625 I0.064 J0.
N18923 X-2.6578 Y-2.625 I-0.064 J0.
N18924 X-2.5298 Y-2.625 I0.064 J0.
N18925 X-2.6578 Y-2.625 I-0.064 J0.
N18926 X-2.5298 Y-2.625 I0.064 J0.
N18927 X-2.6578 Y-2.625 I-0.064 J0.
N18928 X-2.5298 Y-2.625 I0.064 J0.
N18929 X-2.6578 Y-2.625 I-0.064 J0.
N18930 X-2.5298 Y-2.625 I0.064 J0.
N18931 X-2.6578 Y-2.625 I-0.064 J0.
N18932 X-2.5298 Y-2.625 I0.064 J0.
N18933 X-2.6578 Y-2.625 I-0.064 J0.
N18934 X-2.5298 Y-2.625 I0.064 J0.
N18935 X-2.6578 Y-2.625 I-0.064 J0.
N18936 X-2.5298 Y-2.625 I0.064 J0.
N18937 X-2.6444 Y-2.5859 I-0.064 J0.
N18938 X-2.5743 Y-2.5769 I0.0396 J-0.0306
N18939 G01 X-2.5938 Y-2.625
N18940 G00 Z1.4
N20274 Z2.2
N20275 M09
N20276 M05
N20277 G91 G28 Z0.
N20278 G91 G28 X0. Y0.
N20279 M02
03-06-2015, 07:11 PM
MikeC8

Re: V27 Thread Milling Help - No Z code posting

Under the posting tab, change countour ramping output to line moves, default is arc moves.
03-06-2015, 07:26 PM
hawkeyeammo

Yuck! That's not helical interpolation. That's doing it by hand. That's what you do when you have a mill that doesn't support G02 or G03. Is there a bug that keeps bobcad from putting the appropriate Z moves when you use G02 and G03?
03-06-2015, 08:37 PM
hawkeyeammo

I think I figured it out guys. There seems to be a bug in the post processor downloaded from Bob Cad's website. I replaced this line...

64. Arc move XY.
n,g_arc_plane,g_arc_move,x_f,y_f,arc_center,feed_r ate

with this line...

64. Arc move XY.
n,g_arc_plane,g_arc_move,x_f,y_f,z_f,arc_center,fe ed_rate

and voila the Z interpolations are there! Hope this helps some other people.
03-06-2015, 08:50 PM
The Engine Guy

Re: V27 Thread Milling Help - No Z code posting

You are correct, that is the reason :D :D

Here is the code I get using the standard BCx3x.MillPst, seems spot on to me :D

(FIRST MACHINE SETUP - Machine Setup - 1)

N01 G00 X0. Y0.
N02 Z5.
N03 Z1.
N04 G01 Z0.375 F53.821
N05 X5. Y5.
N06 G17 G02 X10. Y0. Z0. I0. J-5.
N07 X-10. Y0. Z-0.75 I-10. J0.
N08 X10. Y0. Z-1.5 I10. J0.
N09 X-10. Y0. Z-2.25 I-10. J0.
N10 X10. Y0. Z-3. I10. J0.
N11 X-10. Y0. Z-3.75 I-10. J0.
N12 X10. Y0. Z-4.5 I10. J0.
N13 X-10. Y0. Z-5.25 I-10. J0.
N14 X10. Y0. Z-6. I10. J0.
N15 X-10. Y0. Z-6.75 I-10. J0.
N16 X10. Y0. Z-7.5 I10. J0.
N17 X-10. Y0. Z-8.25 I-10. J0.
N18 X10. Y0. Z-9. I10. J0.
N31 M05
N32 G91 G28 Z0.
N33 G91 G28 Y0.
N34 G90
N35 T1 M06

(END OF FILE)
N36 M30

(END OF PROGRAM)
%

Regards
Rob
:rainfro: :rainfro::rainfro:
03-06-2015, 10:58 PM
hawkeyeammo

Dang Rob, those are some big ass threads. :)
03-06-2015, 11:12 PM
The Engine Guy

Re: V27 Thread Milling Help - No Z code posting

Quote:

Originally Posted by hawkeyeammo

Dang Rob, those are some big ass threads. :)

Errr, not really, it`s a 30mm dia hole with an internal thread of 1.5mm pitch 10mm dia thread mill, pretty normal sort of job for the boys on the shop floor to attack :D :D :D

Not much to "screw" up there if you pardon the pun :D :D

We all got "metricised" back in `72 and yes it hurt :( :( :(

Regards
Rob
:rainfro: :rainfro: :rainfro:
03-07-2015, 12:11 AM
jrmach

Re: V27 Thread Milling Help - No Z code posting

Quote:

Originally Posted by The Engine Guy

Errr, not really, it`s a 30mm dia hole with an internal thread of 1.5mm pitch 10mm dia thread mill, pretty normal sort of job for the boys on the shop floor to attack :D :D :D

Not much to "screw" up there if you pardon the pun :D :D

We all got "metricised" back in `72 and yes it hurt :( :( :(

Regards
Rob
:rainfro: :rainfro: :rainfro:

Metric Suks :)