# Boring Problem



## prasad (Apr 22, 2016)

Guys, 

I am trying to bore a 1.5 inch deep hole in 6061 aluminum of 1 inch OD using my 9x19 Grizzly G4000 lathe. Hole has to be quite precise to 0.708 inch (18 mm) diameter to mate a shaft. I am using 1/2 inch shank carbide tip boring bars I bought from Little Machine Shop. Lathe runs at 1000 RPM setting. The piece is held in my 6" 4 jaw chuck and 1000 rpm is the highest speed I am willing to run it. next speed setting available is 2000 rpm and I am too scared to try it. 

I wasted three aluminum pieces till now. Each I got very poor finish. I have made sure that every thing - all gibs, tools and everything  is tight. No play of any kind. The boring bar is quite thick and should not flex (I hope). I take very tiny cuts, never more than 0.002 inch at a time. I use plenty of WD40.  The finish I get is terrible, almost like a sand paper to touch. The boring bar was never used before this and therefore new as shipped by LMS. It is set at precise axis height. 

Where am I going wrong? What will get me better or smooth finish? 

Thank you
Prasad
Eastern PA


----------



## TOOLMASTER (Apr 22, 2016)

try raising or lowering the cutting tip


----------



## ChipsAlloy! (Apr 22, 2016)

Make sure your bar sticks out to a minimum from the holder. Just enough to reach the end of your bore. Too much overhang will produce unecessary flex


----------



## prasad (Apr 22, 2016)

I can not raise the boring bar. It is already as high as it can fit in the 4-way tool post. I can lower it. I will try that and see if it helped. The boring bar is shortest it. If I shorten it further I will not be able to plunge to 1.6" deep I want it to go. 

I will try all this tomorrow and post my result, 

Thank you
Prasad


----------



## Bob Korves (Apr 22, 2016)

+1 to what Toolmaster said.  Make sure that the tool is not rubbing on the work below the cutting edge, or anywhere else besides the cutting edge for that matter.  Sometimes those tools are ground poorly, and if you have the cutting edge set level or with a positive rake, the tool can sometimes rub on the work.  You can grind away any part that is rubbing, but if it is the lower portion of the brazed carbide then you will need diamond tooling to cut the carbide.  It is also OK to set the tool at a slightly negative rake to stop the rubbing (cutting edge pointing slightly downward.)  That actually works pretty well, and usually leaves a good finish, which is hard to believe at first.


----------



## mikey (Apr 22, 2016)

Prasad, are your boring bars brazed or inserted tip carbide? I assume the shank is steel, right? Maybe post a pic of your bars?

Your tip needs to be about 0.005-0.010" above center to allow for tangential forces. I suggest zero axial rake (top of insert horizontal) to reduce tangential forces further. Align the center of the bar with the spindle axis and take a decent cut, at least deeper than the nose radius of the cutter to rough. Do not dwell or stop on entrance to the bore; start your feed and maintain it as you enter and proceed down the bore. 

Since you must be very accurate, you need to know how your bar behaves with a given depth of cut. For a finish pass, you might try a depth of cut between 1/3-1/2 the nose radius. Check the ID, dial in your cut, make a pass and check to see how much that DOC increased the ID. You can then rough until you can precisely dial in that finish depth of cut and come in on size. 

You should be able to run the lathe at max speed and take much heavier cuts. Watch your chips and adjust your feed to produce tightly coiled chips; should look like a coiled spring when you get the feed right. Use WD-40 with every pass.


----------



## prasad (Apr 23, 2016)

Hi Mikey

The boring bars are made up of "special heat treated steel" (LMS description) and the carbide tips are brazed. I selected a bar with just the right length for the work. Here is a photo of the bars copied from their web page. 




I have the work mounted in the heavy 6 inch 4-jaw chuck. I calculated the spindle speed and I get a figure of 3000 rpm. My lathe can run at 2000 rpm max and I am scared to run this heavy chuck at that speed. 

I am measuring the bore diameter only at the front end using my caliper. I can not measure diameter at the deep end of the work. I have sprayed WD40 before start of each cut. I will next try tool settings per your advice and see how it goes. 

Thanks
Prasad


----------



## Jim1946 SB9" (Apr 23, 2016)

I have a boring bar similar that did not have a sharp edge on it, it was not dull mind you, when I put a very keen edge on it, all my issues went away and the surface finish is now amazing. It took me forever to get the edge right on the carbide as I don't have a diamond stone but the ceramic stone I have finally did the job. You can shave with it now. Make sure you keep after that WD-40 as aluminum will build up on the cutting edge and the surface finish might go away.


----------



## Bill Gruby (Apr 23, 2016)

prasad said:


> I can not raise the boring bar. It is already as high as it can fit in the 4-way tool post. I can lower it. I will try that and see if it helped. The boring bar is shortest it. If I shorten it further I will not be able to plunge to 1.6" deep I want it to go.
> 
> I will try all this tomorrow and post my result,
> 
> ...



 You can turn (as in twist) the boring bar. This will effectively raise or lower the cutting edge of the bar. It won't take a lot of movement to change the finish.

 "Billy G"


----------



## Franko (Apr 23, 2016)

None of the braised carbide tools I've gotten were sharp. You probably need to touch up the cutting edge.


----------



## master53yoda (Apr 23, 2016)

prasad said:


> Guys,
> 
> I am trying to bore a 1.5 inch deep hole in 6061 aluminum of 1 inch OD using my 9x19 Grizzly G4000 lathe. Hole has to be quite precise to 0.708 inch (18 mm) diameter to mate a shaft. I am using 1/2 inch shank carbide tip boring bars I bought from Little Machine Shop. Lathe runs at 1000 RPM setting. The piece is held in my 6" 4 jaw chuck and 1000 rpm is the highest speed I am willing to run it. next speed setting available is 2000 rpm and I am too scared to try it.
> 
> ...





as far as speed is concerned the 1000 is close, the chart shows 1200 for 1" aluminum.

turning the cutter up or down will move off of center,  I had to sharpen the boring set that looks like yours as the cutters were not very sharp.  on a 1" bore you may also need to relieve the steel portion of the botton of the cutter as well.   



Art B


----------



## JimDawson (Apr 23, 2016)

Try slowing down to about 100 RPM, and and increase the feed a bit. 



Bob Korves said:


> It is also OK to set the tool at a slightly negative rake to stop the rubbing (cutting edge pointing slightly downward.) That actually works pretty well, and usually leaves a good finish, which is hard to believe at first.



And what Bob said.


----------



## Tony Wells (Apr 23, 2016)

Might want to look at the corner radius also. A sharp corner requires less pressure to cut, so is easier on the material and the machine, but isn't always optimal. Even as small as a 0.002-0.005 radius will change your finish. Really, it shouldn't be smaller than whatever feedrate you are using. If it is, you will see a more pronounced toolmark, almost like you were threading at a very very fine pitch.


----------



## Andre (Apr 23, 2016)

Make sure no chips are falling between the nearby cutting edges (not in contact with the work) and the bore. This can happen when there is too little point relief. Hard to explain though


----------



## stupoty (Apr 23, 2016)

prasad said:


> I can not raise the boring bar. It is already as high as it can fit in the 4-way tool post. I can lower it. I will try that and see if it helped. The boring bar is shortest it. If I shorten it further I will not be able to plunge to 1.6" deep I want it to go.
> 
> I will try all this tomorrow and post my result,
> 
> ...



if it is way to low you can always shim up the whole tool post, I do that quite a lot with booring tools that have a very low cutting edge compared to my other turning tools.

You can do the rule method of height setting on the OD of the part then turn the tool round.  For booring it's the reverse of OD turning, that is to say the tool will cut when too high but just rub if it's too low.

Stuart

edit (their may be cases when you can get it to cut when too low but the whole clerence thing is going to be more problematic)


----------



## mikey (Apr 23, 2016)

I have one of those sets. They are marginal as delivered but mainly because of two things: first, the area under the carbide tip is ground round but still rather thick so clearance can be an issue and second, as the others pointed out, the edges are not that sharp. You can gently grind the area under the carbide for more clearance. Keep the rounded shape but take off some of the material at the bottom of the tool. Use a diamond stone to sharpen the edges; it won't take much to do this. Then form a tiny radius at the tip and then hone the top. The tool should cut pretty well after that. 

I suggest using the biggest bar that will fit in the hole and still reach the depth you need. The supposed hardness of the bar, even if it was true, is immaterial. Deflection is influenced by bar diameter and the biggest bar that will fit will deflect less. 

As for speeds, go with what you are comfortable with. Try different speeds on some scrap and see what works best. On my lathe, I bore aluminum at the max speed my lathe can generate, about 2800 rpm, and get a nice finish.


----------



## 4GSR (Apr 23, 2016)

With the rough finish you are getting sounds like the corner of the carbide is chipped.  As others have said, you need some kind of corner radius on the tip of the boring tool. And definitely slow your spindle down to about 600-700 RPM.  Once you get it cutting like you want then start playing with increasing your RPM's.  Feed rate should be around .005-.010" per revolution.  Ken


----------



## prasad (Apr 23, 2016)

Guys

Woohooo... I made it. Thanks for all your advice and I did every trick you gave.  I raised the boring bar, tilted it up, shimmed the entire tool post and finally took it out a ground the tip. In the end I was able to get a decent smooth finish. Main contributing factor was the carbide tool tip sharpness. I don't have a diamond tool grinder wheel. I ground carbide tip on my ordinary 6 inch bench grinder and it worked. I also ground the bottom of the steel part under the carbide tip. 

I learned many things today. Here is a short summary. 
1. Carbide tip of Chinese origin may not be sharp and may need some sharpening. 
2. Carbide tip of Chinese origin can be sharpened using an ordinary grinder wheel. (Obviously poor quality carbide tip)
3. Boring bar height can also be adjusted by tilting the tip up or down (this came in handy when 4-way tool post has been shimmed up (under boring bar) to its full capacity. 
4. Additional height adjustment can be done by placing additional shims under 4-way. 
5. Take very small cuts to minimize flexing of boring bar. 

Thank you all, your help is immensely appreciated

Cheers
Prasad
Eastern PA


----------

