helic holes

[Marty A]

hello all

i have a question. the owner wants to start

hard cutting dowel holes useing the helical way.

he also wants to use tool comp in the program.

its a 1/2 dowel hole and he wants to use a 1/2 em.

i don't know i can't see this working. so far my efforts have failed and he wants to do these

tomorrow am. any ideas on this. you know i'm always grateful for the help

 

 

marty

[David Czerw Triumph Gear Systems]

You should slap him upside the head . He wants to use a 1/2 endmill to generate a 1/2 dowell hole??? Suggest using a smaller endmill or a bigger hole if he wants to insist on his method.

[Rekd™]

You can't do a 1/2" circle with a 1/2" EM unless you just plunge. Try a 3/8"EM.

 

'Rekd

[mayday]

let me guess, he seen someone do this once ?

 

I guess if true position means nothing to him have at it. I do it for ruffing then ream up to 5/8 dia. anything over that I bore. do a cycle time compare, tool wear compare. you dont sound to up on the idea motty. your results will be a . But I have got to the point of ( if thats what you want thats what you get) attidude. seems to be the only way to get the point accross

[Marty A]

thanks guys yea i think he saw it some where.

if i use a smaller cutter how do i put tool comp

in a helical cut. if i can get this to work he

might buy it.thanks again

 

 

marty

[Rekd™]

The only problem here is the hole size vs the tool size. I constantly machine holes +-.0002 with end-mills. Up to 4-6 dia's deep.

 

'Rekd

[Guest CNC Apps Guy 1]

Is this guy a moron???? C'mon, I would expect that out of a green engineer but out of a shop owner??? As was stated earlier, either increase the size of the hole or make the e/m smaller. I'd suggest a 7/16 e/m or a 3/8 e/m to do the duty. See what he fails to understand is that you NEED some room to interpolate!

[Marty A]

hi Rekd

ok i will use a 3/8 cutter for this. what you do

sounds good. how do you go about programing useing

tool comp. thanks again

 

 

marty

[mayday]

Yor can do a contour with ramp and enable comp or circle mill or thread mill

[mayday]

quick example with contour ramp at 1 deg

 

 

N5 G00 G90 G54 X0. Y0. S509 M03

N6 G43 H46 Z1. M08

N7 Z.1

N8 G01 Z0. F8.

N9 G41 D46 X.25

N10 G03 X-.25 Z-.0137 I-.25 J0.

N11 X.25 Z-.0274 I.25 J0.

N12 X-.25 Z-.0411 I-.25 J0.

N13 X.25 Z-.0548 I.25 J0.

N14 X-.25 Z-.0686 I-.25 J0.

N15 X.25 Z-.0823 I.25 J0.

N16 X-.25 Z-.096 I-.25 J0.

N17 X.25 Z-.1097 I.25 J0.

N18 X-.25 Z-.1234 I-.25 J0.

N19 X.25 Z-.1371 I.25 J0.

N20 X-.25 Z-.1508 I-.25 J0.

N21 X.25 Z-.1645 I.25 J0.

N22 X-.25 Z-.1782 I-.25 J0.

N23 X.25 Z-.1919 I.25 J0.

N24 X-.25 Z-.2056 I-.25 J0.

N25 X.25 Z-.2193 I.25 J0.

N26 X-.25 Z-.2331 I-.25 J0.

N27 X.25 Z-.2468 I.25 J0.

N28 X.1844 Y.1688 Z-.25 I-.25 J0.

N29 X-.1844 Y-.1688 I-.1844 J-.1688

N30 X.25 Y0. I.1844 J.1688

N31 X.1844 Y.1688 I-.25 J0.

N32 G01 G40 X0. Y0.

N33 G00 Z1. M09

N34 M05

N35 G91 G28 Z0.

N36 G28 X0. Y0.

N37 G90

N38 M30

[Marty A]

thanks guys i am going to attempt your advice

i will get back to ya. again thanks alot

 

 

marty

[CNCme]

Good Day,

 

 

I can't see helical motion with any thing

size for size... Zero helix is a drill cycle

 

Oh... your boss (owner) said it...then it

must be possible

 

Im surprized he didnt want it yesterday

 

Tony G

Almost Employed Senior Programmer

N.E Massachusetts - Southern New Hampshire

_________________________________________

End mills and tooling are like The "AMMO"

And coolant and chips are like the enemy

Under your boots as you advance in the

Manufacturing Battle

--------------------------------------------------

[crazy^millman]

Oh but he did want it yesterday just couldn't be done. I guess you are a better man than me becuase I would have told him to show me how it is going to work. I just like it when they don't understand something but think they are experts.

 

I had the owners help me and get soem fixutres made well guess what they are worng and guess who has not got to fix them. It does help to look at the 3d info and not the 2d info when you are going to support a cone. The cross section is not what you make the part all the way down when attempting ot machine a craddle for them.

[Marty A]

well thanks everyone this is what i did

i had to go with the ramp and no comp on the 1/2

dwls. i made the hole .5015 and got it to go.

i told them it was a no go with what they wanted

i hope the ramp comes out ok i will know in the morning

 

again thanks everyone oh yea they wanted this last week, but didn't bother to tell me so i could

play around with it.

 

 

marty

[jrykrl]

My favorite is "Oh Sh!t, You did it just like I told you" Author unknown

Jer

[mold100]

last month I talked my company into doing away

with reaming and endmilling dowell pin and ejector pin holes-man I love osg drills we do quite a bit of 1/4 and 3/8 dowells now I dont even worry about them till after heat treat-the drills are expensive but my 1/4 inch drill 61.00 has already drilled aprrox 35 holes 3/4 deep in 48-50 h-13 1700 rpms 7.5 ipm thru coolant no peck hole comes out .2497 to .2503.Any one else using these drills - exocarb-max oils.

[Harryman]

quote:

---

i made the hole .5015 and got it to go

---

Sure you'll get blinky lights on the CAM screen, and code that will put the endmill below the surface of your part, but with a +-.0007" interpolation, the difference between this "helix" and a straight no peck plunge is nothing.

 

Your boss is not as smart as he thinks he is.

[Nominal]

quote:

---

Is this guy a moron????

---

Thanks for saying what I was thinking.

[G Caputo]

This isn't exactly mastercam related, but I learned this trick from an old timer. Drill the reamed hole undersize by say 1/64". Take a new drill and at the lips of the drill, grind it negative, put maybe a .005 - .010" radius on the drill. (sort of like a bullnose cutter). Hone it, so it is dull, then use that as your ream. It works sweet for me. I have always heard that drilling is the fastest way to remove material, and this tip I learned works pretty good in most cases. Just passing on an old timers trick....

 

Greg