conversational input

Hi John

I think what he is talking about is that if you use a sub twice, with 'Create Next Feature' it runs them one after another.

However the answer to this is to get rid of the NGCGUI_OPTIONS = nonew noremove line in your .ini file

You can then create a new instance of the subroutine, in which case ngcgui runs the subs in the order that you initialise them,
as intended

regards

sounds excellent! i'll give it a try today.

thanks


just tried it, it throws a few pickles into the mix, but i'll work on it and see what happens....

it said it couldnt find some values etc...

just tried it, it throws a few pickles into the mix

Yes there are some potential problems, something the second instance of the sub relies upon, could be changed by the first instance when that runs.

It may help to know that you can also start with multiple
tabs for the same subroutine, for example:

...
NGCGUI_SUBFILE = /tmp/tmpngc/one.ngc
NGCGUI_SUBFILE = /tmp/tmpngc/two.ngc
NGCGUI_SUBFILE = /tmp/tmpngc/one.ngc
...

These tab pages will be named: "one", "two", and "one-1"

With this configuration, you could create multiple features for each tab
and then arrange the order of the tabs. If you order them
one-1, two, one
then all the features for "one-1" will be executed, then the features
for "two", then the features for "one"

Avoid the use of _globals within subroutines or use them with
much caution.

-which is why i will eventually have to come up with another gui, i have 16 tabs on my screen -Right now!

....and that is just for od cycles.....

following is a acme threading cycle for external/external threading, usung a squre sided grooving tool.
if not used with the "conversational cycles" i use, you will have to add a tool number input and drop the tool change code.

HAVE FUN!

(info: ACME threading with sq tool)
o<acme> sub
; some random notes
#<ToolNumber> = #1 (= 25 Tool Num)
#<Speed> = #2 (= 300 Rpm)
#<Thd_Dia> = #3 (= 25.0 Final Dia)
#<Drv_Dia> = #4 (= 30.0 Start Dia)
#<Pitch> = #5 (= 6.35 Pitch)
#<Thd_Angle> = #6 (= 29.0 Inc Angle)
#<Cut_Depth> = #7 (= 0.1 Cut Depth)
#<Tool_Width> = #8 (= 1.6 Tool Width)
#<z_start> = #9 (= 5.0 Z Start)
#<z_end> = #10 (= -15.0 Z End)
#<Coolant> = #11 (= 8 9 is off)

(LOGOPEN,AcmeLog)
; internal/external calc
O120 if [#<Thd_Dia> LT #<Drv_Dia>] ; External thread
#<Thd_Type> = 1
#<Thd_Height> = #<Drv_Dia> / 2] - [#<Thd_Dia> / 2 ; height of thd
#<Cut_Dia> = [#<Drv_Dia> - [#<Cut_Depth> * 2]]
#<Drv_Dia> = [#<Drv_Dia> + 0.2]
O120 else ; Internal Thread
#<Thd_Height> = #<Thd_Dia> / 2] - [#<Drv_Dia> / 2 ; height of thd
#<Thd_Type> = 0
#<Cut_Dia> = [#<Drv_Dia> + [#<Cut_Depth> * 2]]
#<Drv_Dia> = [#<Drv_Dia> - 0.2]
O120 endif

; do tool width error calc and depth ratio

#<Ratio_calc_1> = [#<Thd_Angle> / 2] ; half of thread included angle
#<Ratio> = tan[#<Ratio_calc_1>] ; tan value

(log,TanRatio = #<Ratio>)
#<Ratio_calc_2> = [#<Ratio> * #<Thd_Height>] ; width of 1 side relative to total depth.
#<Bottom_width> = [#<Pitch> - [#<Ratio_calc_2> * 2]/2]

O121 if [#<Tool_Width> GT #<Bottom_width>] ; tool is too wide
(MSG,Tool is too #<Tool_Width>Wide!)
(log,ToolWidth = #<Tool_Width>)
(log,BottomWidth = #<Bottom_width>)
M30
O121 else ; All is well!

O121 endif

; Tool change
O122 if [#<_Tool:Number> NE #<ToolNumber>]
; Change Tool
M09 ; coolant off
O123 if [#<_Tool:Number> LT 20] ; front turret
G00 Z#<_Frontchange:Z>
G00 X#<_Frontchange:X>
O123 else ; Rear turret
G00 Z#<_Rearchange:Z>
G00 X#<_Rearchange:X>
O123 endif
G49 ; cancel toolength offset
T#<ToolNumber> M06
G43 G7 G97 S#<Speed>
M03
M#<Coolant>

#<_Tool:Number> = #<ToolNumber>
O122 else ; No tool change -continue.
G43 G7 G97 S#<Speed>
M03
M#<Coolant>
O122 endif

; Toolpath stuff below here

O127 if [#<Thd_Type> EQ 1] ; Thread is external
o101 while [#<Cut_Dia> GT #<Thd_Dia>]
#<mod_Z_start> = [[#<Cut_Dia> - #<Thd_Dia>]/2]
#<mod_Z_start> = [#<mod_Z_start> - #<Thd_Height>]
#<mod_Z_start> = [#<mod_Z_start> * #<Ratio>]
G00 X#<Cut_Dia>
#<Mod_Z_point> = [#<z_start> + #<mod_Z_start>] ;modZstart is negative
Z#<Mod_Z_point>
(log,Zpoint #<mod_Z_point>)
G33 Z#<z_end> K#<Pitch>
G00 X#<Drv_Dia>
G00 Z#<z_start>
(log,Zstart #<mod_Z_start>)
#<Current_Width> = #<Pitch> + [#<mod_Z_start> * 2/2]
(log,CurrentWidth = #<Current_Width>)

G00 X#<Cut_Dia>
#<Z_fin> = [[#<z_start> - #<Current_Width>] + #<Tool_Width>]
G01 Z#<Z_fin> F0.3
(log,Zfin #<Z_fin>)
G33 Z#<z_end> K#<Pitch>
G00 X#<Drv_Dia>
G00 Z#<z_start>

#<Cut_Dia> = [#<Cut_Dia> - [#<Cut_Depth> * 2]]
O125 if [#<Cut_Dia> LT #<Thd_Dia>] ; maximum cut
#<Cut_Dia> = #<Thd_Dia>
O125 else

O125 endif

o101 endwhile
O127 else ; Thread is internal
o102 while [#<Cut_Dia> lt #<Thd_Dia>]
#<mod_Z_start> = [[#<Cut_Dia> - #<Thd_Dia>]/2]
#<mod_Z_start> = [#<mod_Z_start> - #<Thd_Height>]
#<mod_Z_start> = [#<mod_Z_start> * #<Ratio>]
G00 X#<Cut_Dia>
#<Mod_Z_point> = [#<z_start> + #<mod_Z_start>] ;modZstart is negative
Z#<Mod_Z_point>
(log,Zpoint #<mod_Z_point>)
G33 Z#<z_end> K#<Pitch>
G00 X#<Drv_Dia>
G00 Z#<z_start>
(log,Zstart #<mod_Z_start>)
#<Current_Width> = #<Pitch> + [#<mod_Z_start> * 2/2]
(log,CurrentWidth = #<Current_Width>)

G00 X#<Cut_Dia>
#<Z_fin> = [[#<z_start> - #<Current_Width>] + #<Tool_Width>]
G01 Z#<Z_fin> F0.3
(log,Zfin #<Z_fin>)
G33 Z#<z_end> K#<Pitch>
G00 X#<Drv_Dia>
G00 Z#<z_start>

#<Cut_Dia> = [#<Cut_Dia> - [#<Cut_Depth> * 2]]
O125 if [#<Cut_Dia> LT #<Thd_Dia>] ; maximum cut
#<Cut_Dia> = #<Thd_Dia>
O125 else

O125 endif
(log,CutDia = #<Cut_Dia>)

o102 endwhile

O127 endif

M09
(LOGCLOSE)
o<acme> endsub

An updated set of lathe cycles, with many bugfixes.

Feel free to remove the auto toolchange calc, and use as a standalone cycle.

only works with 2.5 -due to tool nose radius calcs, and auto calc of toolchange point. (variables)

- i use these cycles daily, but! always check toolpath, -Trust nothing!

-had an error in the taper rough/finishing sub, here is the fixed version.

a new update, now rough/finish cycles do both boring/turn od, the material diamater vs the diameter for final size determines boring/od.