Hole Contouring

[Guest]

Just curious, does any one here actually trust their tooling enough to contour mill a hole with an endmill? I have a +- .001" and among other ways have considered just using an endmill... think accuracy can be guarunteed? (Based on new cutters and such...)

[?Mark]

Do it daily here with +-.0002" tolerances.

 

Mark

[Guest]

Heck we do +/-.0002 like Mark and hold tight true positions.

[robk]

I feel comfortable holding +/-.0002 on dia's with an end mill as long as I am using helical interpolation and not just contouring at a constant depth. Most end mill manufacturers put a back-taper on their tooling. I prefer to bore, but I know that most of our machines are worthy of holding that kind of tolerance.

[Thad]

What kind of machines are you guys using? We *might* be able to do that on our Fadals.....if you took away one of those zeros! Not to mention, we're lucky if we get a cutter back the cutter grinder with less that .001 taper.

 

Thad

[?Mark]

quote:

---

as long as I am using helical interpolation

---

Helical interpolation is your best friend in this application

+1000

 

Mark

[Guest]

Circle Mill is your friend

 

[Chris Rizzo]

I hold .0003 on a haas.

 

I like to use pocket routine/true spiral just for the sake of having the spring pass option.

[Guest]

quote:

---

I like to use pocket routine/true spiral just for the sake of having the spring pass option

---

In circle mill

Multiple passes

rough 0

finish 2

spacing .000

 

[?Mark]

quote:

---

circle mill

---

For very shallow holes maybe

For deeper, helical is the way.

 

quote:

---

What kind of machines are you guys using?

---

Thad,

Rob, John and myself are Mori users

 

Mark

[HevyMetl]

I use circle and threadmill and love it. I also use ramp contour on holes that are for counterbores and whatnot. Tolerances are not a problem.

 

Thad, that was one of the reasons I think Storky was calling them crap in a post a while back. They get the job done, just not how you want it sometimes.

 

I am running Makinos by the way

[Guest]

I have 2 Fadals, I just don't use them for anything that HAS to be there.

 

Though I just had to use one of them for an 8 piece job with a +/-.0002 hole, guy just comes in and tell me he had to go around the hole 6 times to cut and hold size.

 

Wants me to change the program to reflect this, I says ahhh, noooo. We run them on the Moris next time it won't have to be cut like that.

[Chris Rizzo]

quote:

---

spacing .000

---

no $hit...a guy learns something new every day.

[Guest]

[WeGrok69]

On older machines if holes are egg shaped out at the 45's you can sometimes true it up by taking a conventional cut (g42) for a spring pass. It seems to even out the slop in the machine.

Can you get post to output cutter comp in

circle mill? I didn't think so is why I never use it.

I figured out a formula to force the cutter down the center of a hole and just use contour.

Any one need the formula?

[flippinjig]

I helical too. I like to use a back draft style cutter.

oldirish, I'd sure like to have your formula. Save me alot of time guessing!

 

Thanks, Mark

[HevyMetl]

Tim,

 

With a contour toolpath you can use ramp, and have a helical lead in and out with comp as well. Ramp in countour is very powerful. You can use any type of cutter comp as well with cicle mill. Check the parameter page #2 of the operation.

 

I don't know how many have noticed, but lead in lead out now has a value for helix height which allows you a z drop value on your lead in and out. I just noticed this the other day. HTH

[Guest]

quote:

---

Can you get post to output cutter comp in

circle mill? I didn't think so is why I never use it.

I figured out a formula to force the cutter down the center of a hole and just use contour.

---

Yes, you can use cutter comp, most machines you have to check perpendicular entry and it works fine. Start at the center is easy, just check start at center

 

If you really want to enter at the center on a contour, just place a point at the center and use that as your first chained entity.

[g huns]

quote:

---

I don't know how many have noticed, but lead in lead out now has a value for helix height which allows you a z drop value on your lead in and out. I just noticed this the other day

---

Where ya been John, Ver 9 had it too. On countour at least, don't know bout circle mill.

[HevyMetl]

Well I tend to get in a hurry and don't pay attention. You get used to doing something and never look at the next selection.

[Guest]

There is no ramping ability on circle mill, if you want that kind of toolpath, Helix bore is the way to go.

 

[Guest CNC Apps Guy 1]

Ramp Comtour is the shizzle. For entry/exits, lately I've been using Tangent Line with 30% of Dia. for Length, and 20% of the Dia. for the Arc and sweeping 120 Deg. On entry and exit, overlapping .125" This gets me close enough to the center of the hole plus less problems with marks on the wall.

 

Otherwise I use Perpendicular entry, turning Arc Off, then, I take the radius of the hole and subtract the redius of the tool and this will put me dead center of a circle. If you are leaving stock, subtract the amount of stock to leave from the length of the line.

 

JM2C

[WeGrok69]

Mark,

Hole Dia minus Cutter dia divided by 2

(That is your toolpath radius)

times Tangent of 22.5 deg (.4142)

This number will be your line length AND your

Radius

Set your:

entry/exit to: tangent

Sweep to 135 deg.

It will put you within a tenth of center every time.

-tim

[Guest CNC Apps Guy 1]

Nice Irish. I never took the time to figure the formula.

 

James teh copy and paste to cheat sheet.

[WeGrok69]

Another point is NOT to have the post set to

180 deg. arcs and Radius instead of I's and J's

With 180 deg arcs and Radius output You can cut a hole .0035 out of round on a .03005 rad arc

because of rounding error. If you tried to squeese a .0601 dia hole between 2 points .06 apart the center is .00173 off axis.

That is what you would get if you tried to cut a .5601 dia hole with a .500 endmill and output 180 deg arcs and used "R" instead of "I and J".

I always make sure the tool path radius hasn't been rounded from .00005 to .0001.

I have this drawn up if someone doesn't believe me. - tim