[deadlykitten]

Hi, my feed is on 20000 mm/min. My depth of cut is 0.03mm per pass, and takes round about 4 minutes to finish 1 spline.

if possible, ask a veteran to make a tool from a tap / tool stell / etc ; ( 8..10..12k mm/min ) x ( 0.05..0.07..0.08 mm/stroke) should work

now you go fast on feed, and low on depth, because carbide asks for it

go viceversa, with classic tool

[tea hole]

Something about records and straightness.

Use who you like for broaching, PH Horn is a good resource, i've also used a CNCBroach.com tool to mild success, though failure mechanism on this tool is generally catastrophic for many reasons. Kennametal pitched me a tool with a top notch holder in position to cut a keyway, which I liked the best, but ultimately I didn't get that work so Oh well.
However, I broach a lot in lathes.
There are all kinds of macros out there to do this. Feel free to macro to your heart's content, however, the extremely light DOC and entire lack of side load on the part leaves me to use a different route.
I will say 20000mm/m (787"/min) may be on the high side, especially if you want to use the machine for more than a few parts. that's a lot of back and forth and ultimately, a pretty big damn turret for a ball screw in an L300 genos on box ways.
Typically i stay around 400"/m (10000mm/m). Yes it's slower. But I don't have much in the way of blown inserts either, or machine failure, so whichever.
What i use pretty much exclusively is a G85 LAP cycle. This is proven code below I've used countless times. Your machine is an M machine so you can command M19 C=360/10 to get it to index to the correct spindle angle.
Enough talking.
G50S50
M41
M5
T010101
G94
M109
G0 Z.2
X1.156
M19
G85 NBRCH D.002 F400.0 U0 W0
NBRCH G81
G0 X1.375
G1 Z-2.8
X1.0
G80
G0 Z1
X30
Z30
G95
M2
Obviously in inch mode.
depending on how in depth you wish to get, you can do a macro or just add lines. See below. (not tested, but you get the idea)
G50S50
M41
M5
T111111
NBRCH G81
G0 X1.375
G1 Z-2.8
X1.0
G80
G94
M109
G0 Z.2
X1.156
M19
G85 NBRCH D.002 F400.0 U0 W0
M19 C=36*1
G85 NBRCH D.002 F400.0 U0 W0
M19 C=36*2
G85 NBRCH D.002 F400.0 U0 W0
M19 C=36*3
G85 NBRCH D.002 F400.0 U0 W0
M19 C=36*4
G85 NBRCH D.002 F400.0 U0 W0
M19 C=36*5
G85 NBRCH D.002 F400.0 U0 W0
M19 C=36*6
G85 NBRCH D.002 F400.0 U0 W0
M19 C=36*7
G85 NBRCH D.002 F400.0 U0 W0
M19 C=36*8
G85 NBRCH D.002 F400.0 U0 W0
M19C=36*9
G85 NBRCH D.002 F400.0 U0 W0
G0 Z1
X30
Z30
G95
M2
Since these are running in lathe mode with a spindle index, dimensions are diametrical, not radial.

[deadlykitten]

hy teahole, good to see you

failure mechanism on this tool is generally catastrophic for many reasons >>> please, do you have time to explain this a bit ? thx

what i use pretty much exclusively is a G85 LAP cycle

it works, but :
.... when tool reaches travel end, it will retract a bit; this beat depends; if lap as in :
............ example 1, radial_bit = 0.05; 0.05 is 0.1/2, where 0.1 is default G85 tool disengage from material; can this value be controled from parameters ? it would help
............ example 2, radial_bit = 0.05 + cutting_depth; no dependable on " some_value "
............ in bought cases, there is also Z+0.1 tool disengage
............ how travel end is after groove end, so travel is longer, some humans may consider Z+0.1 unnecessary, and also they may preffer to retreat more on X, so to avoid friction between tool and material .... mr Wizard is human for example like you and me and others

.... after a stroke, tool comes back to Z_front, on X = X_start + depth*k - radial_bit, and it goes to next position in 2 steps :
............ X is increased by 2*radial_bit, so it becames equal with last X_toolpath
............ X is increased by depth, so it becames equal with next X_toolpath
............some humans may consider this 2 steps approach unnecessary

Unnecessary movements, wherever they occur, is an issue ... please, take a look at attached *.pdf, from mr Wizard ...
This aspect is taken official by Okuma, since they release such solutions ...

NBRCH G81 ( example 1 ; not like the one you posted )
G0 X = V1
G1 Z...
G80

NBRCH G81 ( example 2 ; like the one you posted )
G0 X = V1
G1 Z...
   X = V1 - some_value
G80

kindly ! now stay tuned for next post

[deadlykitten]

this post is only a modest example; nothing more ...

( . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . )

this little *ssb uses G85

it comes with :
........ default variables : start & end diameter; cut depth, nr of grooves
........ in cycle restart variable : groove to begin with
........ alignment variable : angular shift, if needed
........ cycle reduction
........ restart skip

OS01

 ( main     values )    V1 = 29        ( start diameter   )
                        V2 = 29+1      ( end   ... ...    )
                        V3 = 1/6       ( cut depth        )
                        V4 = 4         ( how many grooves )

 ( auxiliar values )    V9 = 300       ( angular shift        )
                        V10= 3         ( groove to begin with ) 

       ( * )


   IF [ VRSTT NE 0 ] NEND

   V8 = FUP [ [ V2 - V1 ] / [ 2 * V3 ] ] ( nr of passes      )
   V7 =       [ V2 - V1 ] / [ 1 * V8 ]   ( reload depth      )
   V5 = 360 / V4                         ( angular increment )

   G00 X=VSIOX Z150-VETFZ
   T010101 M66
   M19 C = MOD [ V9 + V5 * [ V10 - 1 ] , 360 ] G00 X=V1 Z10 M63 ( Z_start )

   G94
   V6 = V10 - 1

   NHERE

       V6 = V6 + 1
       CALL OQ01

   IF [ V6 LT V4 ] NHERE

   M18   ( also trigerred by M02 )   

   G00 X375-VETFX Z150-VETFZ

   NEND

RTS

 ( . . . . . . . . . . . . . . . . . . . . . . . . . )

OQ01

   IF [ V6 EQ V10 ] NSKIP

       M19 C = MOD [ V9 + V5 * [ V6 - 1 ] , 360 ]

   NSKIP

   G85 NEXT D+V7 F2000                    ( feed )
       NEXT G81
                  G00 X=V2
                  G01              Z-70   ( Z_end )
                  G01 X=VSIOX-2*2         ( retreat on previous X toolpath )
            G80

RTS

on my lathe, M19 does not create a rigid holding, since i can rotate the chuck by hand for a few degrees

also, i believe that M19 was developed for other purpose, like to orient spindle with a jaw under material, when material auto-advances and is heavy so to be sustained

thus C axis + break is more trustful

this code does just that ... please notice that there is a delay after M147, because sometimes break confirmation is a bit to fast ... not always, but chuck can be rotated by hand a bit after M147, in a small interval window, until breaking mechanism fully engaged

effort to rotate chuck after M147, until breaking is 100%, is much higher than effort needed to spin under M19

OS02

 ( main     values )    V1 = 29        ( start diameter   )
                        V2 = 29+1      ( end   ... ...    )
                        V3 = 1/6       ( cut depth        )
                        V4 = 4         ( how many grooves )

 ( auxiliar values )    V9 = 300       ( angular shift        )
                        V10= 3         ( groove to begin with ) 

       ( * )


   IF [ VRSTT NE 0 ] NEND

   V8 = FUP [ [ V2 - V1 ] / [ 2 * V3 ] ] ( nr of passes      )
   V7 =       [ V2 - V1 ] / [ 1 * V8 ]   ( reload depth      )
   V5 = 360 / V4                         ( angular increment )

   G00 X=VSIOX Z150-VETFZ
   T010101 M66
   M110 M808
   G00 C = MOD [ V9 + V5 * [ V10 - 1 ] , 360 ] X=V1 Z10 M63 ( Z_start )

   G94
   V6 = V10 - 1

   NHERE

       V6 = V6 + 1
       CALL OQ02

   IF [ V6 LT V4 ] NHERE

   M807
   M146
   M109

   G00 X375-VETFX Z150-VETFZ

   NEND

RTS

 ( . . . . . . . . . . . . . . . . . . . . . . . . . )

OQ02

   IF [ V6 EQ V10 ] NSKIP

       M146  
       G00 C = MOD [ V9 + V5 * [ V6 - 1 ] , 360 ]

   NSKIP

   M147

   G04  F1 ( wait 1 second for the breaking mechanism to engage )

   G85 NEXT D+V7 F2000                    ( feed )
       NEXT G81
                  G00 X=V2
                  G01              Z-70   ( Z_end )
                  G01 X=VSIOX-2*2         ( retreat on previous X toolpath )
            G80

RTS

and here : headquarters ; call what you need

 ( intro )

   G270
   VSZOZ = 450
   VSZOC = 0
   G50 S2100

   M867 ( cas          : off )
   M216 ( rapid ignore : on  )

 ( GO )

 ( CALL OS01 )  ( grooves with M19 index )
   CALL OS02    ( .. ... ...   C   index )

 ( outro )

 ( M84  )
 ( SP=1 )
 ( M215 ) ( rapid ignore : off )
   M866   ( cas          : on  )
   M02

[tea hole]

The Genos L300M has a rapid in the Z axis of 20000mm/min. The X axis has 25000mm/min.
Whatever works for you. I have never had issues with M19 before.
Different broaching strokes for different folks.

[deadlykitten]

The Genos L300M has a rapid in the Z axis of 20000mm/min. The X axis has 25000mm/min

or viceversa generally, Z rapid is greater than X rapid ... or at least when Z is horizontal

I have never had issues with M19 before.

after M19 try to rotate the spindle by hand ... you may have no problems if cutting effort is less than what it takes to spin it

[tea hole]

My mistake.
My note on my desk was listed backwards.

[deadlykitten]

hello i would like to share my latest thoughts on this :

1) attached excel file+images help computing start diameters, in such a way that interference are omited, thus being sure that groove tool will start cutting smooth ( no stress on 1st cut );

2) carefull with lube setting for such operations; you may consider :
...... reducing off timer #2
...... also :

You should check #3 on this page in order to reduce the amount of lube you use. This will enable lubing the axis only when the axis are moving rather than all the time - even when parked and not running a program

3) check droop value for X axis; program shared in this post activates droop only when X axis is positioned for the cut; how cutting depth ( radial ) is equal with a few hundreds, it may help considering droop control; otherwise, remove G64 and G65 from the code, and maybe consider repeating last pass if clearance is low and feed is high

4) about the program :

  ( main     values )    V1 = 41.2   ( start diameter   ) ( for internal grooves : V1 < V2 )
                         V2 = 59.38  ( end   ... ...    ) ( for external grooves : V1 > V2 )
                         V3 = 0.03   ( radial cut depth ) ( >0 )
                         V4 = 10     ( how many grooves )
                         V5 = 5      ( Z start )          ( Z start > Z end ) 
                         V6 = -73    ( Z end   )
                         V7 = 9      ( turret post )
                         V8 = 0.6    ( X axis disengage; input 0 to return @ start diameter ) ( >=0 )

...... allows cutting od or id grooves;
......... for internal grooves : start diameter < end diameter ( V1 < V2 )
......... for external grooves : start diameter > end diameter ( V1 > V2 )
...... a variable ( V3 ) will be initialized with desired radial cutting depth ( =t ) ; if |end_dia-start_dia|/2 is not a multiply of "t", than "t" is recalculated in such a manner, that new_value is never higher than desired value ( new_t <= t )
...... simply declare the turret post used ( V7 ); is not needed to change tool corection inside the program
...... V8 delivers custom behaviour for retreat path :
......... if V8=0 than tool will always retreat at X=start diameter, avoiding tool friction during retreat movement
......... if V8>0 than tool will always retreat at X=X_cut±V8
............ if V8>0 and V1 < V2, tool will always go X- after the cut
............ if V8>0 and V1 > V2, tool will always go X+ after the cut
............... thus V8 represent the clearance in absolute value; if it is zero, than tool will always return at start diameter
............... i input this option after remembering this reply from mr Wizard :

It may also be a good idea to move back toward centerline so that the insert is not dragging on the way back out. Carbide doesn't like that very well

  ( auxiliar values )    V9 = 1      ( groove to begin with ) ( default = 1 )
                        V10 = 0      ( angular shift        ) ( default = 0 )

this ones allow more control :
... V9 is self explanatory : for example if something happened at an intermediate groove, you may simply change the insert and continue the program from the next groove, without changing C_zero
... V10 inputs same behaviour as editing C_zero : it shifts the grooves position with a specific angle; how the program crafts all angles inside a 360arch, thus a polygon inside a circle, this may help alligning the grooves with whatever geometry you consider

default values for these variables are written in paranthesys

also some infos are written after programs end ( like a delay after M147 )

OS01 ( broaching internal / external grooves ) ( some infos @ bottom )

  ( main     values )    V1 = 41.2   ( start diameter   ) ( for internal grooves : V1 < V2 )
                         V2 = 59.38  ( end   ... ...    ) ( for external grooves : V1 > V2 )
                         V3 = 0.03   ( radial cut depth ) ( >0 )
                         V4 = 10     ( how many grooves )
                         V5 = 5      ( Z start )          ( Z start > Z end ) 
                         V6 = -73    ( Z end   )
                         V7 = 9      ( turret post )
                         V8 = 0.6    ( X axis disengage; input 0 to return @ start diameter ) ( >=0 )

  ( auxiliar values )    V9 = 1      ( groove to begin with ) ( default = 1 )
                        V10 = 0      ( angular shift        ) ( default = 0 )

  ( * )

  ( G270 ) (*1)
    G00 X+LVXP-VETFX Z150-VETFZ
    M110 T+V7*101 M66 M08 M808 G94

    V6 = V5 - V6                                  ( full travel ) 
    IF [ [ [ V8 GT 0 ] AND [ V1 GT V2 ] ] EQ 1 ] NJUMP
             V8 = -V8                             ( adjust sign for X disengage )
                    NJUMP
    V11 = DROUND [ ABS [ V2 - V1 ] / [ 2 * V3 ] ] ( nr of passes : with 3 digits )
    V11 = FUP    [ V11 ]                          ( nr of passes : natural )
    V12 =              [ V2 - V1 ] / V11          ( diameter cut depth )
    V13 = V9 - 1

    NINCC V13=V13+1 G65
          G00 X+V1+V12 Z+V5 C+MOD[V10+360/V4*[V13-1],360]
          M147 G64
          G04 F1 (*2)
          V15=0 G01 F123.456
          IF [ V8 EQ 0 ] NINCX2
              G91
        (*3)  NINCX1 Z-V6      F5000             ( Z- : cut )
                     X+V8      F50               ( X disengage )
                     Z+V6      F5000             ( Z+ : back @ clearance )
                     V15=V15+1
                     IF [ V15 EQ V11 ] NGOOUT
                     G65                         ( droop on  ) 
                     X+V12-V8  F50               ( X for next pass at small ipw )
                     G64                         ( droop off )
              IF [ V15 LT V11 ] NINCX1           ( increment X axis, version 1 )

              NINCX2 Z+V5-V6   F5000             ( Z- : cut )
                     X+V1      F6500             ( X disengage )
                     Z+V5                        ( Z+ : back @ clearance )
                     V15=V15+1
                     IF [ V15 EQ V11 ] NGOOUT
                     X+V1+V12*[V15+1] G65        ( X for next pass + droop on )
                     X+VSIOX   F50               ( repeat X to assure small ipw )
                     G64                         ( droop off )
              IF [ V15 LT V11 ] NINCX2           ( increment X axis, version 2 )

          NGOOUT M146 G90
    IF [ V13 LT V4 ] NINCC                       ( increment C axis )

    G00 X+LVXP-VETFX Z150-VETFZ M807 M109

RTS ( . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . )

 ( adjust linear speeds with caution )
 ( do not exceed maximum rapids when tool is going back to Z start, even if movement is in feed )
 ( consider a limit, like rapids * 50% for example )

 (*1)
 ( unblock G270 to prevent possible errors when program begins )

 (*2)
 ( delay, so the breaking mechanism will fully engage )

 (*3)
 ( NINCX1 : is executed when X disengagement is always constant, thus return movements are paralel )
 ( NINCX2 :  ... ... ... ... ... ... ... ... ...   not constant,  ... ... ... ... ... ...  coaxial )

program is called from the headquarters :

  ( intro )

  ( VSZOZ = ... + 0 )
  ( VSZOC = ... + 0 )
    G50 S1900
    M867 ( cas          : off )
    M216 ( rapid ignore : on  )
    LVXP = VPVLX - VBZOX

  ( main )

    CALL OS01

  ( outro )

  ( M84  )
  ( G195 SP=1 )
  ( M215 ) ( rapid ignore : off )
    M866   ( cas          : on  )
    M02

optimized to the teeth kindly !

[Cjonk]

Hi all,

Attached is a short clip of my part and a pic of the finished product.https://youtu.be/4Gx1ZfCHCRc,

[pfp]

Hi mate I know this was a few year ago but would you be able to share your code for this operation. cheers

[tea hole]

Hi mate I know this was a few year ago but would you be able to share your code for this operation. cheers

There are multiple code examples in the string below.

I’d advise using those.

[pfp]

There are multiple code examples in the string below.

I’d advise using those.

Hi I would prefer to use yours as a test as I have seen it working unlike the other bits of code posted.
I would then be sure what I am going to do will work.

[deadlykitten]

hy pfp, i have an optimized code for osp300, that requires some initial values, shared below; if you wish, i can help you to use it / kindly

$ ( main     values )    V1 =  42.28    ( start diameter   ) ( for internal grooves : V1 < V2 )
$                        V2 =  60.40    ( end   ... ...    ) ( for external grooves : V1 > V2 )
$                        V3 =  0.032    ( radial cut depth ) ( >0 )
$                        V4 =  8        ( how many grooves )
$                        V5 =  5        ( Z start )          ( Z start > Z end ) 
$                        V6 =  -73-5    ( Z end   )
$                        V7 = LINK      ( turret post )
$                        V8 =  0.6      ( X axis disengage; input 0 to return @ start diameter ) ( >=0 )
$
$ ( auxiliar values )    V9 =  1        ( groove to begin with ) ( default = 1 )
$                       V10 =  0        ( angular shift        ) ( default = 0 )