machining problem

[Catman]

Hi everybody there, I visit this forum from time to time and today I need some help.

 

I am running production right now. What I work on is mild steel. The part is quite simple: you make a 2” bore with plus minus ten thousandths tolerance, two taps and mill an edge. The boring bar has two inserts: one for roughing, the other for finishing.

 

The problem is that boring is not stable, I mean the tool life for the inserts is very short and varies a lot, sometimes you can get ten parts from one insert and sometimes you get one or two. Whatever you do with the feed rate and RPM, things are still the same.

 

I know the spindle is not good. If you hold the tool that is on the spindle and push and pull it you can feel it plays. I ask my boss to have it fixed, for some reason he can’t.

 

Thanks in advance

[PE @ IHS]

A worn spindle bearing will definitely affect tool life, though I don't think that explains your problem. (since your spindle runout is constant, the tool life should also be constant.)

 

Make sure that your boring bar is on center, ensure that the bar is only as long as needed (no overhang), and increase the drill size. With such an open tolerance, I wouldn't even bother with a boring head; just mill it with an indexable carbide endmill.

[mold100]

I agree with Peter,+/-.010 thats a ballpark,I would drill it then circle mill it.Also

is your insert the best choice for the material,all insert manufactuers have differant

coatings and geometry for all applications.Also what RPM, feedrate and part thickness?Mild

steel like 1018 or 1030?just curious.

[Catman]

Hi, Peter and Mold100, thanks for your helpful replies.

 

The boring bar is indeed longer than necessary, but it is the only one that I have. We produce these parts in high volume, so a faster way is needed, that’s why we are using a boring bar.

 

The material is QT100 ASTM, part thickness is 1 inch, RPM around 950, feedrate is 8inches per minute.

 

First thing we flamecut a hole of 2 inches in diameter, then open it up to 2.18 inches with +/-.010 tolerance by a boring bar. After flamecut the material is hardened a lot.

[Team Ferret]

As I was reading down the thread, I was thinking you have steel with hard spots, then I read the flamecut part of the process. That is the reason tool life is inconsistant. I would say that some control on the flamecutting process is needed. Slowing the cooling or annealing would help.

 

Dave

[Mick]

How deep is this bore? If its through, whats the thickness of the plate? I'd say the best way would be to rough it, using a ramp contour with a round insert milling cutter, then finish it with a stright edged milling cutter.

We mill a lot of steel and stainless steel, and have to bore a lot of holes to the same tolerance, and thats the method we use.

[TheePres]

Consider if ur flaming is actually being cost-effective if causing so much problem. personally i would drill and rough-mill.

[mold100]

You could buy a 2.0 sandvik coromill,run it in your machine I am guessing an older well

used mill at around 1100 rpms feed it 60 ipm using 2d ramp machining,this will be a helical

cut,by depths,.05 in a pretty quick cycle with no predrilling, o.k finish easily held +/- .01.for

alot cheaper than a good boring head.With the cost savings of no flame cutting,and

cutting out your drilling cycle,maybe you can justify the cost?

 

[ 05-16-2002, 07:53 AM: Message edited by: mold100 ]

[Scott Bond]

Hi all

quote:

---

As I was reading down the thread, I was thinking you have steel with hard spots, then I read the flamecut part of the process.

---

I am also convinced the problem starts here.

I would center drill ,drill ,and contour ramp.

If I still had a problem, I would check

the machine,

the tools,

or the stock.