Boring bar overhang 2

[4AXIS]

I am looking for any guidlines or references on bore diameter to length ratios. Our sales dept is having difficulty quoting jobs properly. They take orders for parts that have extreme bore diameter to length ratios. In the manufacturing dept we try to stick with a 3x ratio for steel boring bars and up to a 7x ratio for carbide boring bars. However we are constantly getting orders for parts with up to a 10x diameter to length ratio with .001" tolerance and a 63 finish. Any help or advice would be greatly appreciated.

 

[funnelguy]

My advice would be to change the incentive system for sales from gross sales to an incentive tied to profitability. Your sales department might not think they work for you...

The ratios sound OK to me. Perhaps other methods would get you to your finish and geometry requirements with less hassle. Hone? Ream? Burnish?

 

[mrainey]

funnelguy is right on the mark.

 

[Nate101]

Suggest to your estimators to try quoting gun drilling the deep holes. I've used Thompson in Ca. for some deep holes Ø1.00x22.00". They're quality is very good. I've gone as high as 10x, but on low quantities and cramming the biggest carbide bar I could in the hole. Most of the time having to leave a few thousandths for honing. A lot depends on the hole diameter and material being drilled.

 

[steveh]

The post about gundrilling is right on target. We gundrill to 40 X diameter with good results. There are some shops around that will gundrill your parts if you dont' want to make the large investment required.

 

[4AXIS]

I am very interested in all the responses about gungrilling. What kind of tolerance and surface finish can this process hold. Are there many vendors out there that provide this service and if so at what cost and turn around time?

 

[unclesyd]

In looking at producing deep holes you should also look at deep hole boring, trepanning along with gun drilling.

The following two sites have some good information and some shops who can do the different work.

http://gundrilling.tripod.com/

http://www.business-seek.com/Busine...achine_Shops/Trepanning__Gundrilling__Boring/

 

[Mechineer]

Will gun drilling hold the ±.001" tolerance and 63 finish?

 

[unclesyd]

Mechineer,

What is the diameter, length, and material?

 

[4AXIS]

The part that started this thread has a 12.250" L.T.B. with a 1.689" bore dia ±.0005" and hold a 63 finish. The material is 4340 pre heat treat 28-32.

 

[funnelguy]

4AXIS,
This sounds like a horizontal boring mill or machining center operation. Is that correct? Could you provide details about the spindle/quill and coolant available?

What are the conditions at the bottom of the hole? Drill point? Flat bottom? Undercut?

Gun drilling coupled with honing would certainly get what you want for depth, size and finish. The only concern I would have would be the straightness of the hole relative to some other datum on the part. The gun drillers and trepan houses I worked with would usually quote a .001"/1.00" depth straightness allowance. This could be in the form of either staight line misalignment or a "rainbow" type effect.

Also, gun drilling can sometimes leave "rings" in the bore where a chip jams between the part and the drill. Trepanning gave me a better hole than gundrilling. This was more than 10 years ago, so my info may be dated. I would NOT say that either process will give you a perfect 63 end to end.

My vote would be to drill the hole about .060 to .080 undersize and then bore it .002 to .004 undersize trying for a 125 finish with no rings in the bore and hone for finsh off machine. Honing a blind bore requires a bit more care, but should be a piece of cake on these specs. Talk to Sunnen.

All of this depends on your HP, coolant, tooling and ability to break chips and get them out of the hole. Best of luck.

 

[unclesyd]

I'm waiting for a call back for the people that did a lot of work for us. I know that they could part of the hole in your tolerances.

If you decide to go the way funnelguy suggests I would talk to Engis.

Quote with a been there and done that. You cannot go oversize on a bore.

"Once set to size, Engis superabrasive bore finishing tools precisely finish the inside diameter of parts in a single pass. The result is bore geometry as good as 20 millionths (.0005 mm), sizing to better than .0001" (.0025 mm) and surface finishes as fine as 4 microinches (.1 micrometer Ra.)."

 

[Nate102]

Funnelguy and Unclesyd bring up some good points. The parts I had gundrilled had great finishes so I have to assume they were honed. They met my quality criteria so I didn't care how they were made. Most of the time they were datums, so I had to locate off them and a quality finish had to be there. I checked Unclesyd's links, out of the (3) company's I have used (1) is listed here. Listing company's names and addresses may be concidered "promoting", here's my email if you want a source that was good for me.

black_lab_rat@hotmail.com

Any other questions/experiences I'd rather see on this thread.

Nate102/1

 

[4AXIS]

funnelguy,
The part is a 20deg spur gear. Pretty basic part, just turn the blank, cut the teeth, keyway and setscrew. Need to hold .003" t.i.r. for teeth cutting. Thought maybe about a bore releif with no surface finish and more tolerance. Then just match bore the two ends.

 

[funnelguy]

4AXIS,
I'm sorry, you've lost me. I thought the part had a 1.689" bore 12.250" deep. I thought the "LTB" designation meant length to bottom.

Now I'm envisioning a gear machined from a hub on a rather long hollow bar whose bore extends through both ends. It also sounds as though only a portion of the 2 ends of the hollow bar need to meet the critical bore dimensions and the center between them could be relieved.

Am I anywhere near close?

 

[4AXIS]

Funnelguy,
Kinda close. First of all this is just one example of a part with a long bore to diameter ratio. That is the problem that started this thread. You are right that this part has a thru bore. The work piece will start as a solid bar sawed long. Then put in a turning center and drilled, bored and turned. Agian, with the long bore it becomes a problem of boring. That is why I suggested a bore relief in the center of the part and match bore the two ends. But, a lot of the time for one reason or another the customer will not let us modify their design. Sorry for any confusion.

 

[unclesyd]

You still need a an accurate hole that straddles the center line prior to relieving the center section. You will have to essentially finish the hole from one end, though a good fixture would allow finishing from either end. The object would be to bore/drill a precision hole the finish it. A hole can only be so bad before it can't rectified.

If you can get precision with the drilling/boring operation go for it even though it may cost a little more it sure saves in the long run.

If you plan to relieve the center section as stated, the Engis hones are well suited for this type application. If you look at the section on Helical Hones they will even hone with a cut keyway.

 

[funnelguy]

Well, here's my advice. (And it's worth every cent you paid for it. )

The ability to machine most of the part in a single chucking is a big plus. I would definately try to get the bore machined for concentricity in the same setup as turning other critical features. Working the part from 2 ends will almost certainly unecessarily compromise precision and add cost. The only reason to work the part from both ends is to help alleviate the overhang problem. Stop trying to get a 63 finish and +/-.0004 with the bar.

I can see how you might want to face and turn the first end, and drill halfway through the part. Then flip the part end for end, and finish machine the rest of the part. You will have fewer problems drilling.

You are throwing away quality and money and turning center time. Bore for position, hone for finish and tolerance. You will be amazed at how quickly you can achieve your objectives.

A hone is a funny animal. You have to work with one to understand how much money you can make (save) with one and where it may help you in other parts. Similar to CAD, waterjet and vacuum heat treating, IMO.

Find a local shop with a vertical hone and some expertise and pay them to show you the processes' capabilities. Or have one of the manuf's train an operator AND an IE. I wouldn't farm out the honing operation. Better to keep control of the quality and lead times in house. Hones aren't that expensive, are trouble free and easy to learn. You won't need a dedicated operator unless your work rules require one.

Last, I personally have stopped trying to get customer's to produce sensible designs. Producing overdesigned parts with practically no tolerance is what I get paid to do. Tighter specs means fewer competitors and more money. Let your competition whine while you bring in more accounts. I also will not correct a customer's drawing without being compensated or certainly not until after I have a PO for the parts. Why should I help my competitors? Good luck!

 

[4AXIS]

This is an awesome web site. First time I ever posted a question and look at all the response. It is very nice for a change to get other people's idea's who deal with these problems daily and know what it is like. It gets very old trying to explian why there is a problem with a part and have somebody look at you like "IS THERE A PROBLEM HERE?". Anyway thanks for all the replies and and if I have anymore questions I will ask agian.

 

[Jnicely79]

I use kennametal tuneable de-vibe bars. theyll get you ten to 1 and can be pushed a little further at times