deep boring

[dan m]

I normally don't have a problem boring deep parts but this particular one is giving me a headache. I’ll try to explain this the best I can. What I have is a taper i.d. starting at 2.495 dia. ending at 2.06 dia. going 9.887 deep. The taper starts with a .25 rad. I am drilling it with a 1 3/4 drill the trying to bore it with a 1 1/4 carbide boring bar using a cmng-432 insert. I am cutting at 250 sfm at .01 fpr. In 4340. As you can imagine I am getting all kinds of chatter. Does anyone have any suggestions?

 

Thank in advance.

Dan

 

[ 07-25-2003, 01:37 AM: Message edited by: dan m ]

[CAM-mando]

Dont know how much help can offer thats a pretty deep hole, but ...

 

I would an additional drill sizesto step the hole out first. Then I would use a shorter boring bar to rough and semi finish the larger diameter area and only use the smaller bar where I had too for rough / semi finish.

 

For finishing, you didnt say what your radial depth of cut is. In alloy steel you really need to burry at least 1/2 the nose radius to get a good cut which of course creates more load on the tool. Therefore I would use the sharpest insert that would hold up maybe .005/.007 and keep radial DOC 1/2 that. Is it regular steel shank bar ? You could try a heavy metal, Carbide or dampening bar ?

[Harryman]

Good morning Dan.

 

For sure the nose radius needs to be smaller, .015 may be small enough.

 

Did you try setting your roughing passes at a 20 degree angle? I've found that in deep holes this "funnel roughing" does a great job of clearing chips, and allows use of a slightly larger boring bar. This is one of my favorite features of MC

[McRae]

quote:

---

1 1/4 carbide boring bar using a cmng-432 insert.

---

Dan,

 

First thing I would look at is the Insert. To do this kind of boring, I would recommend a Positive Insert with something in a D or T shape. (TCMT or DCMT). The negative insert is the first thing to eliminate.

 

Second. How is that boring bar being held. Are you just using the set screws in the holder on the shank of the bar or have you manufactured a split holder that "Clamps" onto the bar. If you want to deep bore for a living, this holder is neccessary.

 

Third. Setup of the bar is important. Set the insert slightly above centre. This way when the bar deflects, the hole it machines will actually be smaller than intended. If you set the bar on centre - perfect, then when deflecting down, the bar will actually cut oversize and chatter like mad trying to relieve the pressure on a regular basis - about 250-1000Hz...

 

There are expensive antivibration boring units available from Kenna and Sandvik, if you want to bore without chatter, all day every day, buy them... We have made a pile using this tool.

[CAM-mando]

All good stuff Andrew

[McRae]

One more thought here - the lead angle of the tool while cutting a taper will also influence the deflection amout so look for something with a small angle to minimize side pressure.

[Andy]

One job I did a few months ago I made a tapered boring bar as big as would fit and allow for chips. Hole was 2" ID to .415 ID in 7". I mounted an insertable small tool holder (in this case a small bore bar .312Dia) in the end. It ended up being very rigid and no problems.

-minimum tool point radius important as stated earlier.

Hope its not HasalloyX

 

[ 07-25-2003, 06:00 PM: Message edited by: Andy ]

[Jimmy Wakeford from Barefoot CNC]

Dan,

I ran into similar problem threading one time. I tried very shallow cuts, multi finish passes, (all the the tricks).

 

What finally worked was a bigger bite. I took a .100" finish pass and was smooth as silk. The new insert required this.

 

Jimmy

[Philcott]

Lots of good ideas to think about. I would suggest you have a look at a cermet insert for finishing. You could probably run around 750 sfm. Stays sharp and allows small DOC while still giving a good finish.

 

Phil

 

[ 07-28-2003, 01:03 PM: Message edited by: PhilCott ]

[chris m]

+1 on the positive insert, small nose radius, and the cermet

 

If you already have the boring bar for the CNM, as it sounds like you do, and don't have any that'll take CCMT or TCMT inserts I'd try a CNM insert with a very positive edge prep like Sandvik's CNMP insert or somebody else's equivalent. These are typically uncoated carbide and are usually intended for Al, but if you don't have a ton of parts you might get away with it.

 

C

 

[ 07-28-2003, 03:33 PM: Message edited by: chris m ]

[crazy^millman]

+1 to the radius, the postive rake, and the ceremnt. Take a bunch of rubber bands and put as many as you can on the bar itself. I mean a box if it will not get in the way also it the parts is thin walled get some bondo and incase the outside making sure to mix it cool. Then good luck from there. Everyone has put you on the right path young luke. Have good luck with that one dont like doing those jobs but we dont what we must to get by. ...........................One other thing to think about not sure of your equipment but if you have a horizontal boring mill and center in the end of the bar use a small live center to support the end of the bar. Most machines have a back support to goes to the bed. You can also make a tapered plastic sleeve to go on the bar the acts like a support to allow the bar the be supported as it get deep and will act like a damper also.

 

[ 07-28-2003, 04:26 PM: Message edited by: Millman^crazy ]

[dan m]

Thank's for all the Ideas. I am going to play with these and I'll let you know what happens.

 

Thank's Again,

Dan