helixbore in steel

[ken wong]

Hi! everybody

anybody have any idea to make a hole with dia=2"+/-0.0005 deep 2.5" but without boring bar. I use e.m with G02 but it come very bad (taper and not round) i want to try helix bore but i don't know what feed , speed , pitch and use inset E.M or solid E.M and does helix bore make good finishing?

[HevyMetl]

The taper and not round has more to do with your machine and programming parameters. I use the thread mill cycle alot to do deep l-d bores with releived solid endmills and it works well. Countor ramp also gives you the same result, but it allows you to make multiple passes.

 

We would need much more information on the material you are cutting, the machine and its capabilities and what its state is. I wouldn't expect much out of fadal unless you ran it really slow and it was fairly new, but a Makino or Mori could fly thorugh this with no problems. HTH

[Tom Szelag]

I'd think this would be heavily influenced by whatever machine tool you have. Unless you have a high end machine and your circular interpolation is outstanding, that close of a diameter (and thus form) tolerance would require a boring head.

 

Like John was saying any lower end machine might just not be able to cut it (no pun) by just arcs/helixes.

[Joels]

How about a reamer?

[robk]

quote:

---

How about a reamer?

---

Ouch... A 2" reamer? ROI on that kind of a tool better be pretty good.

As long as your machine is capable than you shouldn't have a problem holding that tolerance. Try slowing down your feed rate if the machine will not keep up around corners. Use one cutter to rough and another to finish.

[?Mark]

quote:

---

does helix bore make good finishing?

---

Yea, very good.

 

quote:

---

I use e.m with G02 but it come very bad (taper and not round)

---

Other then what was mentioned in above posts, this is your problem.

You need to climb mill (G3) to get a good finish.

With bad finish you can't even measure roundness and size correctly.

Also for finishing a deep hole like this you should consider using em with recessed neck.

 

Mark

[cblythe3d]

A lot depends on your machine and setup. A ball bar test at more than one point on your table will tell you about your machine accuracy. On the cheap, mill a boss or hole on a test piece then spin it with a .0001 test indicator in spindle at a few table locations.

 

The roughing/finishing method takes advantage of end cutting insert mills taking a finish cut on the way back up. The milling equivalent of a lathe spring cut dragging the tool backwards and making use of the unused side of the cutter.

 

If you have more than one or many bore diameters it becomes an essential component in tool management, reducing tool count and simplifies operator inspection as the tightest diametrical tolerance controls the other holes.

 

Take note of the fact that actual feed rate is not the feedrate you program. Actual feedrate is tangental. If you use a 1 inch tool to bore a 1.062 hole the outside of the tool will travel aprox 3 inches(1.062*3.14). While back at the ranch the center of the tool is only moving .190 thousandths.

 

In addition the insert will rub more than cut with no space for chips. I try to use a tool not larger than 1/2 bore diameter and almost never more than 75% bore dia.

 

External loc/Internal loc = feedrate division/multiplication factor

 

3" /.2" = 15 that is a feedrate at center of this cutter of 1 IPM is actually 15 IPM tangentally

 

At 1/2 bore dia the feedrate multiplier is an even 2.

 

With a small DOC radially, large Z pitch values act like a wiper insert making for fast reliable smooth finish.

 

Charles

AKA Luke Otta Vindoo (new deli weatherman)

[Guest]

You also did not mention the what type of steel you are attempting to do this on, as well as the type of endmill you are using and the diameter of the tool.

 

If this is an 1018, carbide combination and your machine is capable of holding such a tolerance you'll get one thing but if you're trying to reach 2.5" deep with a 1/2" 2FL HSS endmill you'll have problems all day long.

 

So any more information you can provide will go a long way to helping you achieve the desire result.