Is it practical to use a single point boring tool for CNC boring? What type of boring bar would be recommended? An example of what I would be using it for is a customer of ours uses a specialty wheel for their forklifts. They have speced out a certian bearing to use with this wheel. It requires us to enlarge the existing bore to .031 over to the same depth. It is 3.25 deep from the factory and normally I use a 3/4 endmill with a flute length sufficent to make my finally .005 finish pass at depth for a nice clean bore after a couple of spring passes to account for any deflection. Rather than having to order endmills specificly for these parts that I so far haven't found approriate for other jobs we perform I'd like to just program a boring cycle using a helical toolpath in mastercam and be done with it. The conventional machinist in the shop suggested an offset boring head, but Im wary of that for a couple of reasons. Am I I off track in wanting to use some sort of indexable boring bar? I appreciate any input, thanks.
Scott

The indexable cutter or single point is the way to go. This will save you from running any spring passes and mesuring after each pass. If a bar is set right you only have to work it in once to get the size required.
As you said yourself, using a 3/4 EM you get tool deflection and a inconsistent bore, especially if it is a bearing fit. The boring bar will be faster in operation, give you a better finish and you have more control over the desired size.
I would say if this is a repeatable job to get a bar the will be rigid enough to do this in 2 passes. One to rough and leave .015 for finish.

HTH

You could get a relieved endmill for your helical interpolation in which case the deflection would be the same, all the way down the hole.

You could get a relieved endmill for your helical interpolation in which case the deflection would be the same, all the way down the hole.

Im not trying to say this is a bad idea, it does work for a lot of applications, but for a hole that deep and relieving the EM would cause worse deflection, and this is something you dont want for a bearing fit.

I am a bit confused exactly what you are asking. You have the question: Is it practical to use a single point boring tool for CNC boring?

But then you say; I'd like to just program a boring cycle using a helical toolpath...

Are you thinking about using a single point tool to helically interpolate a bore; in other words using it as if it was a single flute milling cutter?

Or are you planning on boring the hole with a single point tool set to cut the correct hole diameter?

If it is the single point helical interpolation yes you can do it, I have done, but the finish tends to be not very good and it can be slow.

Single point boring using either an adjustable tip boring bar or a boring head gives the fastest and best hole quality. Because you are taking off such a small amount you should be able to do it in a single pass once you have the tip adjusted for the correct diameter.

Not exactly a Haas specific question, so I'll chime in. When we got some "real" machines, I pretty much put the boring heads away, then I realized that I was missing something, pulled the boring heads back out and have been loving them ever since.

You didn't say what size your bore is, only the depth, but you can do some really cool stuff. I've hand ground a trashed endmill, hung it out of the side of the boring head and stuffed a 2" head all the way down into a 2.3" diameter hole, 3" deep. Its also really easy to make your own stiffer attachments for criterion boring heads, so that you can drop a 1.5" bar down a 1.75 hole.

Interpolation is great, but it really sucks when you are going deep and need a really tight tolerance, besides, you get to the bottom, spindle orient, back off .010 and rapid out, huge time save, and once its dialed in, it just repeats and repeats and repeats, good stuff.

BMackinnon

The only inserted cutter I have seems to be to much for the machines we have. It is a 1.25 Dia Serria Sine III endmill, but I just can't seem to tune it in using Valanite's recommended SFM for the selection of inserts for it. I forgot to say the bore size as pointed out. It was 2.371 +.001 -0.0 as specified by the customer.

Geof

I had thought to use a helical toolpath which would have been equivalant to a single flute cutter. Mainly to have the convience of set it and forget it so I can keep the other machines we have cutting. I had thought to not use the offset boring head to prevent the need to adjust it for a finish pass. I figured it would be slower, but if it was a consistant and held my tolerance and gave a nice finish I thought it might be worth taking a little longer. If it is going to be an excessive amount of extra time, or give me a poor result then I need to figure something else out.


I'm basically trying to learn different ways to do the same job. Now that I have some help taking some of the load in the shop off of me I'm trying to expand my bag of tricks and learn more about this trade.

Thanks
Scott

I would be tempted to rough out to within .005 using the single point in helical interpolation but then finish off with a boring head that only has to be set to the finish sized.

BMac,

Do you really think taking 0.01" off the diameter of a 0.75 endmill is gonna make a big difference stiffness wise?

I've used this method many a time to great success. It really depends on the spec of the hole. How round does it have to be and such, and the capability of your machine. If you have trouble with the machine repeating after a toolchange, not even a boring head will help your application. If you are confident that your tools repeat in the spindle, then boring head all the way.

Iscar ITS boring system is the cat's A$$. Sanvik's system is pretty good. D'Andrea makes the same system as Iscar, but it might be cheaper. I've seen the techniks system in some trade mag's, but I've never used them. Iscar and Sandvik are pretty much set it and forget it. If you have good machining parameters.

...Do you really think taking 0.01" off the diameter of a 0.75 endmill is gonna make a big difference stiffness wise?...

I wondered so I did a calculation. Treat the cutter as a simple cantilever beam (although I admit I have never seen a beam with flutes and cutting edges:) ). The deflection depends on the moment of inertia which varies with the fourth power of the radius for a round solid and the third power of the depth for a rectangular beam. Fourth power gives a reduction in stiffness of about 5.3% and third power about 4% and it is probably safe to say that the cutter will fall somewhere between these two. So if the 0.75 cutter was deflecting 0.005 you may see the difference which is about two tenths.

But I don't think it matters because the deflection is going to be constant and when you have the upper end of the cutter relieved you can offset the cutter path to compensate for the deflection because there is clearance. With a parallel cutter a compensating offset is not possible.

I think the suggestion of setting the offset boring head to finish would be best for me. If the buy us the refurb monoset I would be tempted to try something a little more fancy, like a relieved EM, ground from a resharpened em we already had, but I'm trying to stick with tooling we already have in the shop so we can stop using single purpose (to date) tooling. The salesman named a ridiclulesly low price per wheel, so while we have the contract on it I want to minimize the expense and time required for me to do the job. If I can set it and forget it and keep my other machines cutting it helps the shop's productivity numbers with the front office.
Thanks all