Internal splines on a Okuma Genos L300E-M ( Broaching effect)

[Cjonk]

Good afternoon everyone,

I need help/advice regarding the title of my thread above....

I wrote the program and I'm reasonably confident it is correct, its the execution at the end of the day that is letting me down!

There is 10 teeth on the ID at 36 degree intervals for about 60mm long.(attached is drawing)

The special tool (that I have gotten made by Iscar), goes to the start position in front of material, and stops there on the line where my fees and length of got is ( G1 Z-60 F.2).

My CNC machine is giving no alarms or errors, but is not going any further than the start position mentioned above.

I have a notion the problem might be that the CNC is getting confused as neither the chuck or the live tool is not rotating.

I have looked through the manuals for maybe a code that needs to be in to bypass the problem , but sadly no success.

Any advise or assistance will be greatly appreciated!

Kind regards,

Chris Jonk
+27844421244
chris@transmine.co.za

Similar Threads:

• Need Help!- machining of spline on a GENOS L300E-M
• Internal and External Hex Broaching
• broaching splines on a cnc haas mill
• Canned cycle internal broaching?
• Cutting Internal Splines?

[deadlykitten]

hello ... god, this part is old ... still have problems with it ?

[deadlykitten]

The special tool (that I have gotten made by Iscar), goes to the start position in front of material, and stops there on the line where my fees and length of got is ( G1 Z-60 F.2).My CNC machine is giving no alarms or errors, but is not going any further than the start position mentioned above.

hey, i had foreseen this problem since your 1st thread about this :) ... rpm under fix holder :)

under M110 + G01 +G94/G95 machine does not move without rpm .. also does not raise any erros

in the moment that it stops, try to push the jog button for M axis :) it should move :)

without M110, machine moves without rpm only under G94 .... also, under G95 it requires rpm

there are other particular cases when machine just stops and it looks at you without saying errors :)

G00 X375 Z150-VETFZ
T010101 M66
G00 X40 Z5 SB=100 M13 M08 M63 ( rpm under fix holder )
( this should be your start diameter )

V1=0

NHERE
V1=V1+1
CALL OCAN V2=36*[V1-1] ( go cut each groove, one by one )
IF [ V1 LT 10 ] NHERE

M12
M146
M109
G00 bye bye

M02

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

OCAN

M146
G00 C+V2 ( index at groove angle )
M147

V3=0
NHERE
V3=V3+1
CALL OSUB V4=V3*0.3 ( V4 total cutting depth ) ( V3 cutting depth )
IF [ V3 LT 5 ] NHERE ( maximum depth = 5*0.3 )

RTS

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

OSUB

G01 X=40+2*V4 F500 G94 ( raise X with your desired cutting depth )
G01 Z-50 F... G94 ( cut )
G01 X=VSIOX-0.5 Z=VSIOZ+0.5 ( disengage from material )
G01 Z2.5 F2000 G94 ( back to front )

RTS

[deadlykitten]

... that I have gotten made by Iscar

try lower cost tools producers in your area ... 1/2price, same tool

try to make it on your own

I wrote the program and I'm reasonably confident it is correct, its the execution at the end of the day that is letting me down!

if you wish, try the sample i just wrote ... put it in step by step and change your Z zero with + 55

I have only the Mastercam drawing... ( from your previous thread )

is good to draw, but try not to ... using CAD / CAM makes you focus on the part, and not on the toolpath ... when i see parts, i see toolpaths, not geometries

try to master each operation as an individual, and split your part into such a bunch of operations ...

is faster, does not require techincal computer drawing ... well, comes with practice ... there is always a way ... CAMs behave well for 5axis, but for simple things like this, they just consume time

[deadlykitten]

you may fall also into alignment issues ... i will explain those soon

consider rough / preoperative operations to speed up those grooves ( image 01 )

if material gets stuck to tool, consider reducing cutting lenght, by going from Z- X- to Z+ X+ ( image 02 )

final tool should be 8.4mm width, while a rough tool can be a cutting / groove insert, 3 mm width ... just find / craft a holder for it

how many parts do you wish to do ? kindly !

be carefull, o42.64, insert already cuts 0.418mm ... so start at maximum o42 ( image 3 )

[OkumaWiz]

I think if you use the M808 command, it will release the cutting feed interlock. On the newer controls (P200,300), you are not allowed to feed unless either the m-spindle or main spindle are rotating. This will ignore the interlock.

Best regards,

[deadlykitten]

I think if you use the M808 command

hello mr wizard yup, M808 / 807 ... it works thank you

[Cjonk]

Hi all,

i just want to thank everyone for their input to try help me out with my problem! MUCH APPRECIATED!!!!

Attached is a pic of my sample part i did out of plastic. i started on my brass part, have to take lesser cutting depth and play around with feed, but that is minor!

End story.............i was successfull!!

[deadlykitten]

    V4 = ...   ( start diameter   )
    V5 = ...   ( end   ... ...    )
    V6 = 0.03  ( cut depth        ) 
    V9 = 7     ( how many grooves )


          ( * )


    V8 = FUP [ [ V5 - V4 ] / [ 2 * V6 ] ] ( nr of passes ) ( 59.2-40 / 0.06 = 320 )
    V7 =       [ V5 - V4 ] / [ 2 * V8 ]   ( reload depth ) ( 19.2 / 640 = 3% ...  )


    G00 X375-VETFX Z150-VETFZ
    M110
    T080808 M66
    M808 ( SB=100 M13 ) M08 G00 X=V4 Z+10 M63    


    V1 = 0


    NHERE


      V1 = V1 + 1
      CALL OMAIN V2 = 36 * [ V1 - 1 ]


    IF [ V1 LT V9 ] NHERE


    G00 Z10


    M807 ( M12 )
    M146
    M109
    G00 X375-VETFX Z150-VETFZ


M02


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


OMAIN


    M146
    G00 C+V2
    M147


    V3 = 0


    NHERE


      V3 = V3 + 1
      CALL OSUB


    IF [ V3 LT V8 ] NHERE


RTS


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


OSUB


    G01 X=V4+2*V3*V7         F50    G94
                       Z-70  F5000
    G00 X=VSIOX-0.6
    G01                Z+10  F2000


RTS

[deadlykitten]

even if program will work, please be carefull at the fact that machine will move fast during a short period of time ... this leads to overheat on your ball-screw; a lathe is not build for such operations ... in this case, for low depth, cutting force is reduced, so machine will move in a manner that is not designed to

i strongly suggest to:
...rough this operation before; use post5 as a reference
...run the program with interruptions ... for example let it work for 30 passes / zig-zags, than take a break
...don't rush into it / be carefull

if you are not sure / not certain, you may damage your ball screw
however, even if there will be no damage, you will have some wear

if you have a car, and someone asks you for it, you give it, as a nice guy ... but when you look on the window, you see that it throtles that engine too high, without moving ... also he speeds up to 60 and sudden breaks ... and reverse to 30 and sudden breaks ... i guess is enough for you to see that only 2 times ... now think about your lathe

[Cjonk]

Good morning,

Attached is my brass part. i did 5 splines when my insert gave up on me.

Awaiting delivery of more inserts from my tooling guy to carry on .

[deadlykitten]

consider crafting same end geometry on each groove ...if is ok how it is now, than leave it like that

if you cut same groove with more than 1 insert :
.... you must pay attention to alignment, so not to have interruptions on wall
.... i would rough with a smaller insert, and after i would use a finish insert ... also, if machine has Y axis you can finish with a smaller insert ... like this, you don't need to use 2 different sizes ... you can use smaller inserts without Y axis, but you need excentric alignment on your holder

[OkumaWiz]

Looks like you may be going heavy on your passes. What is your depth of cut? Also be sure that you are going completely through the part so that you don't build up a "wall" that will put high forces on the insert.

In the broaching cycle, you will not typically reach your target point in Z since your next move is retracting, so be careful. 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.

Are you using PH horn's broaching inserts? They have a decent setup for doing this, but your form may be more specialized than stock.



Best regards,

[Cjonk]

Hi,

Thank you for the feedback!

My depth of cut is 0.03mm per pass, and takes round about 4 minutes to finish 1 spline.

I retract in X-axis at the moment 0.5, before retracting in Z-axis.

[deadlykitten]

Are you using PH horn's broaching inserts? They have a decent setup for doing this, but your form may be more specialized than stock.

hy cjonk, about tool supliers, so far you tried Iscar, and as mr Wizard said, there is also PH ... i was looking for custom holders for a setup, and i found this :

Keyway broaching with EWS-Slot

on that site is a broaching holder, also 2 pdf files, one of them including PH tools ...

if you consider, i have extracted and attached that part with PH tools ... on 2nd page from end you can find recommendations about starting diameter for ID grooves

if you plan for more such operations, consider :
.....to give a chance to local carbide tools manufacturers, if any arround your position
.....specialized holders, as the one from EWS, and don't forget this one recommended by mr Wizard :

Broaching Tool for ID keyways, splines, and slotting. Live tool lathe powered. - MD Tooling

bye bye

[OkumaWiz]

Hi,

Thank you for the feedback!

My depth of cut is 0.03mm per pass, and takes round about 4 minutes to finish 1 spline.

I retract in X-axis at the moment 0.5, before retracting in Z-axis.

Depth is not bad. I usually do not go more than .06mm. Speed sounds slow though. I have done about 20 small splines in about 5 minutes in steel. What speed are you feeding at?

The suggestion about the live tool broaching unit is a good one for both speed and ease on the machine. They are expensive but may pay for itself in the long run.

You may want to retract X completely out of the material before retracting Z to make sure you are not dragging.

Best regards,

[Cjonk]

Hi,

My feed is on 20000 mm/min. i tried to increase more but got an alarm immediately, so it seems that is my max i can go

[deadlykitten]

Hi, My feed is on 20000 mm/min. i tried to increase more but got an alarm immediately, so it seems that is my max i can go

hey cjonk, 20k mm/min and 0.03cut depth is ball screw death

try to decrease feed and raise cut depth ... or at least decrease feed ... 20 m/min = 66% G00 .. fast & furious

[Cjonk]

hI,

The 20K feed sound high but in real life it is actually not that fast( my opinion might be wrong ).

i have a mp4 i took, will try load it up. did , but sofar unsuccessful

[deadlykitten]

The 20K feed sound high but in real life it is actually not that fast

on genos max rapid 25m/min ... you are @ 80%

rapid should be less than a few seconds

i have a mp4 i took, will try load it up; did , but, so far, unsuccessful

*.mp4 extension is not allowed ; please take a look at available extensions ( attached image ; image is from attachments interface )

to upload mp4, change it's extensions ( eq movie.mp4.pdf / rar / zip ) or pack it inside an archive

maximum sized files are for pdf (4gb), rar / zip (8.58mb) ... rest are 500kb