Lathe question on holding +/-.00015 bore dia

[dforsythe]

I’m not a lathe guy, but we are working on a part right now 4130  that has a .998 thru bore 6” long and need to hold a tolerance of +/-.00015 in a production environment.  Is this possible and if so, what kind of tooling would you recommend?

 

Thanks, Damian

[kccadcam]

Sunnen Hone - bore about .0005 to .001 small and hone them. Best way to get consistency on that tolerance.

[djstedman]

That's asking for 6 times diameter deep and that's before even taking into account that the bar would actually be a lot smaller than finish size.

 

Add in the fact that on a lathe your cutting error is doubled since your only cutting one side of the hole, and your asking the machine to be able to hold position to +/- .000075 while having the bar cut a dead true hole at what is likely an actual 8 times diameter deep hole. While it may not be impossible, I would venture to say its impossible to do in a production setting.

 

If the customer does in fact NEED that kind of accuracy.. I think kcadcam has the right idea.. hone the parts for size

[K2csq7]

Even with the best machine, best boring bar, best everything..... that is not going to happen in a production setting. (ok, if you had the best ever everything it might....)

You will find it cheaper to send it out for honing or ID grind than to pay your guys to go on a wild goose chase. 

I hope they quoted that appropriately. 

Give the operator a -.001/-.003 tolerance & make sure he is checking concentricity. 

 

Honing guys will cry if you give too much of a range on the size of the parts, grinders wont care if there's .002 or .007 stock on....

[dforsythe]

Thanks for the info.  Sounds like the ID grinding is the best way to go.

 

 Anyone recomend a shop in the N CA area?

[djstedman]

I still think your better off honing, a relatively small diameter combined with a large ratio of depth to diameter will probably make internal grinding a no go.. or at least quite costly..

 

 

Why Honing?

We have used honing since the inception of our business. We have tried hard turning, but we had difficulty controlling quality, especially for microfinishes. Another process, ID grinding, is good for gears with larger bores (greater than 0.75 inch) and low L:D ratios (0.5:1), but our range of work includes smaller diameters and relatively deep bores. In addition, ID grinding at L:D of 5:1 or more can cause deflection in the spindle, exacerbating taper issues. Honing, on the other hand, removes material faster than grinding as soon as you reach an L:D of 2:1. We still outsource parts for ID grinding, such as those with blind holes where counterbores leave no relief for honing tools.

 

 

The above comes from the from the following article in modern machine shop.. and I think addresses the issues your likely to run into with attempting to grind this..

 

http://www.mmsonline.com/articles/why-we-use-honing

[dforsythe]

Great artical.  Hone looks like the way to go!

 

Thank you!

[Sticky]

Honing guys will cry if you give too much of a range on the size of the parts, grinders wont care if there's .002 or .007 stock on....

 

 

What? The grinding guys are not going to like sticking to a quote when the material sizing is 3x more then necessary.

 

If you find a grinder crazy enough to do this job anyways I would run. This is a honing job.

[Del.]

How does a hone machine actually straighten out the perpendicularity of a hole that is not straight to begin with. Does it not want to follow existing hole?

[crazy^millman]

How does a hone machine actually straighten out the perpendicularity of a hole that is not straight to begin with. Does it not want to follow existing hole?

 

Yes it does to a point it will make the hole straight, but yes if the hole was .02 out of perpendicularity to start it will stay that, but there are some honing machines that can take can do some serious material removal. V&M in Brea still has some hones that can broach almost 4 foot in one stroke. hearing those things what is what Yankee Fan still gets to here if they are still using them.

 

Honing is another one of those art forms in machining I have always found interesting. Seems like basic principles, but good honing guys are like artist.

[DODGERFAN]

. V&M in Brea still has some hones that can broach almost 4 foot in one stroke.

 

.

Why does that name sound so familiar?  

[DUM1]

BURNISHING MIGHT BE AN OPTION http://www.cogsdill.com/products/burnishing/roll-a-finish-tools/

[DUM1]

BURNISHING?http://www.cogsdill.com/products/burnishing/roll-a-finish-tools/