Broaching in X?

[Mcam Nut]

I was wondering if there is a easier way to broach, I used to always use a drill cycle and drill multi points until final depth with a m19. but we just bought a carbide inserted broaching system, and it is recomended to have .2mm clearance on the retract. I am using a point toolpath for this, but it is starting to get hard on the head. Is there a easier way to broach?

[crazy^millman]

Well could you make a custom drill cycle to do this task? You might could use the expaned drill parameters as well.

[Mcam Nut]

what i need is a drill cycle that retracts in the x or y direction at the bottom of the key by .008" can I make a custom cycle to do this Im trying to use a g76 (fine bore with shift) the Q seems to be the shift amount. will this work? and can I control my shift direction?

[Guest]

Sorry, this is slightly off topic for your question, but I was wondering how you broach using a G76 without the spidle turning...? Obviously you wouldn't want a spinning broach...? Maybe I am not getting the whole picture.

[Mcam Nut]

no, im trying differnt things, when i use a drill cycle I remove speed and the m3 and insert a m19, this will work with a g81, or g85 but i need to have a .008" shift in x or y before retract thats why i was wondering on a g76, I havent tried it yet, but it sounds like what i want, but it does not show up in my backplot as shifting, but its worth a try i guess

[Guest]

Yuo have got my interest. Can you plunge -G1-(I presume that's what your doing) without the spindle being on? Or do you use a modified rapid speed?

 

I understand what you want with the G76, nut my concern would be that the spindle would re-orient. I know on my Haas VF6 sometimes, but not always, if the spindle is oriented and I hit the button to orient it, it will spin...as said, not always. So, if you were even a few thou into a broach and it decided 'oh let's just orient for the sake of it'...crunch.

 

I would agree with a custom peck drill that goes to full depth and retracts on the x or y instead of the z. Sounds like the easiest way to me.

 

Lots of guru's here to give some good help for something like that.

[Mcam Nut]

Well ive been broaching using spindle orient for quite a while now and so far no problems as long as the m19 is in the safety line it seems to work, and with point machining i can have a g1 for my z- moves and a g00 for my x, and y and z+ moves, but with point machining it is a fairly long process, I have my diving head set up flat and I have 8 difernt keys to cut, but I use a g81 for my home made cutters and this works well rapid up in z+ and feed z-. I may just run the same process for this new tool and see what happens, or maybe a g85 to feed back out of the hole, im just thinking of tool life on using this inserted cutter over our usual hss ground cutters, any sugestions?

[Guest]

Alternate thought...you ever though about writing a short macro to do broach? If you broach alot then it might be worth it, then you can just give the macro instructions on how deep, retract and similar.... I am very versed in macro programming yet, but it's a thought.

[Mcam Nut]

Yeah thats probally a good idea milling man, I dont know alot about making macros but i am interested in the concept, might you have a sample macro or somthing i could look at to get a few ideas of what might be needed

[chowquoe^]

quote:

 

_____________________________________________

You might could use

_____________________________________________

 

Love it

 

[crazy^millman]

Here is what I did for a back spot facing in the post:

code:

---

pdrlcst$         #Custom drill cycles 8 - 19 (user option)

#Use this postblock to customize drilling cycles 8 - 19

pdrlcommonb

#if drillcyc = 8, pcan1, pbld, n$, *sgdrlref, *sgdrill, pdrlxy, pfzout, pcout,

# prdrlout, dwell, *feed, strcantext, e$

if drillcyc$ = 8,

[

sub_prg_call = peck1$

pcan1, pbld, n$, *sg00, *sgabsinc, pfxout, pfyout, strcantext, e$

pbld, n$, "M98", *sub_prg_call, e$

]

if drillcyc$ = 9,

[

pdrlcommonb

pcan1, pbld, n$, pdrlxy, pfzout, pcout, *feed, strcantext, e$

"M00", e$

*drl_prm1$, *drl_prm2$, e$

"G1", *drl_prm3$ , *drl_prm4$, e$

*drl_prm5$, e$

"M00" , e$

*drl_prm6$, e$

pcom_movea

]

else, "CUSTOMIZABLE DRILL CYCLE ", pfxout, pfyout, pfzout, pfcout, e$

pcom_movea

---

Then defined them here:

code:

---

# --------------------------------------------------------------------------

fmt Q 2 peck1$ #First peck increment (positive)

fmt 2 peck2$ #Second or last peck (positive)

fmt 2 peckclr$ #Safety distance

fmt 2 retr$ #Retract height

fmt Q 2 shftdrl$ #Fine bore tool shift

fmt Z 2 zdrl$ #Depth of drill point

fmt Z 2 tosz$ #Drilling top of stock

fmt N 4 n_tap_thds$ #Number of threads per inch (tpi) / Pitch (mm)

fmt F 2 pitch #Tap pitch (inches per thread)

fmt R 2 refht_a #Reference height

fmt R 2 refht_i #Reference height

fmt S 4 drl_prm1$ #Back Spot Facing Spinlde Speed

fmt M 5 drl_prm2$ #Back Spot Facing Spindle Direction

fmt Z 2 drl_prm3$ #Back Spot Facing Intinal Z depth to start Clearence postion

fmt F 15 drl_prm4$ #Back Spot Facing Feedrate

fmt Z 2 drl_prm5$ #Back Spot Facing Depth

fmt Z 2 drl_prm6$ #Back Spot Facing Retract Z place for moves between places

# --------------------------------------------------------------------------

---

HTH