Watch your "spring" passes!

[T Bredehoft]

Was the hole OD enough that you could have used a larger/heavier boring bar to finish?

 

[macardoso]

It is a mount for an 85mm AC servo motor (Allen Bradley MPL series) for my CNC. It is made from billet aluminum 4x4x5". The ballscrew support bearings are integrated into it (I messed up one of them). Similar to this one (X Axis), but more complicated.

 

[macardoso]

Was the hole OD enough that you could have used a larger/heavier boring bar to finish?

Yes, and now that you mention it, I should have finished with a 3/4" bar. Good Idea.

I'm thinking I will rebore/re-line the hole with a sleeve and hit the size correctly, in this case I will use the larger bar.

 

[mikey]

If I'm understanding you correctly, you're boring on the lathe and you have two bores back to back in the same part. Each bearing bore has to be concentric with the other within 0.0005" so you have to bore one and then flip the part and bore the other side to tight radial and axial tolerances, correct? To me, that is problem #1; not insurmountable but can be tough to indicate an odd shaped part. Assuming you can do it ...

Deflection with a steel bar is going to be a real issue, as you pointed out. Thing is, if you sleeve the bore and try again are you going to use the same bar material or are you going to step up to a carbide bar? I ask because you are trying to take very tiny cuts in a deep hole with a carbide insert. As you know, radial cutting forces rise until the depth of cut exceeds the nose radius and this is going to compound the deflection you already have with that bar material, leading to even greater uncertainty and inaccuracy. Best option is to go with a carbide bar and switch to the smallest nose radius you can get for your finishing passes. Minimum depth of cut you can expect some accuracy with will be about 1/2 the nose radius so smaller is better but ideally, you want to take a minimum depth of cut a few thou larger than the nose radius to provide enough support to overcome the radial forces. If you can find an insert that fits your bar with a nose radius of 0.002", that will probably work. What is your nose radius, anyway? What kind of insert?

You are using the compound to feed the bar because you need more precise control of bore depth? A good, solid carriage stop is a far better device for depth control. If you don't have one, you really should make one if you're going to do precision boring.

With regard to overboring on the final step, that was a big miss. If you were taking identical depths of cut and getting proportionally the same increase in ID each time then simply reducing the feed rate would not have caused that large a discrepancy. Something else is going on. Some things to ponder:

• Did you allow the part to cool to ambient temp before taking the last few passes? As you know, metal heats up and aluminum in particular can expand enough to make an accurate measurement a problem until it cools down. A related issue: are you sure you measured the bore correctly? Not being a dick; this is a common reason for a miss and I'm using myself as the prime example because I KNOW this is a factor to consider.
• Was the insert broken in? If you used the same point on the insert, was it worn or damaged? It should cut the same if it is intact. Look at the insert under magnification and make sure.
• Are you certain your depth of cut was set correctly? I've made this mistake more times than I care to admit; when I miss a bore, this is usually why I missed the damned thing. The larger the error, the more likely it was me.
• Did you drag the cutter out while it was still in contact with the bore on the final pass? I assume not but if you did then this is very possibly the culprit.

Bottom line: you did good all the way up to the end. I'm just not convinced that "spring" is responsible for that big a miss. If you had issues when roughing and mentioned spring then yes, I might agree there. However, with tiny cuts like you're taking at the end, spring is usually not an issue that causes this big a miss on a final pass. Radial cutting forces, deflection caused by the user and the bar material itself, the condition of the insert, the heat of the part, coolant or no coolant, adequate depths of cut for the nose radius in use all make a difference and, at least in my case, the very important pilot error. When you're boring for a bearing and the fits impact on internal bearing clearances, you're working into the low tenths and everything matters.

By the way, I'm not being critical in the least here. I know what its like to spend hours on a part and blow the whole thing with the final pass in a critical bore, believe me. My best advice is to sort out the issue before you attempt to bore that sleeve. Personally, I wouldn't attempt it without a carbide bar.

 

[macardoso]

If I'm understanding you correctly, you're boring on the lathe and you have two bores back to back in the same part

Mikey,

Thank you for the detailed response. I don't feel criticism at all, in fact I am still plenty new to all of this (<10 years) so I'm trying to learn everything I can (hopefully that never stops.

You are correct about the part, there are several features on this part, but the critical ones are the back to back bore which hold a pair of angular contact bearings. Concentricity is critical here as any runout between the features would cause uneven loading on the bearings and poor alignment of the ballscrew. I chose .0005" as an attainable value, however I'm trying to hold as tight as I can. The axial distance between the bores is slightly less important, but I wanted to hold better than +/- .005" so I opted to use the compound slide. I gave a .002" tolerance, but it was less critical than the bore.

I agree it was tough to hold these tolerances, but the smallest diameter hole through the part was cut in the same setup as the backside bore which allowed me to indicate it when flipped (The indicator was completely inside the part to reach!).

My plan for sleeving will be to use my 3/4" x 10" steel boring bar, as T Bredehoft commented above. I have confidence I will be able to hold the tolerances with a little more care than might have been given before. I will one day invest in carbide bars, but I can't stomach the costs right now, so a little more skill/luck/care will be required. My bar is a SCLCR with CCGX 31.51 (1/64" radius) or CCGX 31.50 (1/128" radius), I can't remember which I have mounted currently. I have been using these razor edge ground inserts for a while now with good luck. I really can't get them to rub even when taking <.001" cuts.

You are correct about the use of the compound slide for depth control. I have been thinking of making a carriage stop, so I may have to bump that up on the roster of projects.

In answer to your thoughts:

1. Temperature was kept nominal by the very slow cutting speed, small depths of cut, and application of coolant. I agree it can mess with measurements, but in the case of a bore, wouldn't that tend to undersize the bore? I very well could have screwed up the measurement, we all know I have done that before. I personally don't love the "feel" type of measuring instruments like the telescoping bore gages I used, however I had no other way to measure the bore deep in the part. I would prefer a direct reading 3 point bore gauge, however the money is better spent elsewhere.
2. Insert is relatively new but has removed some material. I don't know if the break in is as important as it is on inserts for tougher materials, but it is a thought. The insert is sharp and has no damage.
3. I've goofed plenty before so I can't rule that one out! I didn't think I missed it, but 8 thou is a serious discrepancy.
4. Cutter was backed off the material before backing out of the bore. I never reverse cut.

I agree that I was surprised to be that much oversize. I might be exaggerating the impact of the spring in the bar and there may be other factors at play here. I think with the equipment I have, I am happy when I hold within .0005" on diameter.

Thanks for all your thoughts!!!

Here is a model of the part:

And a cross section showing the bores:

 

[mikey]

Thank you for not feeling that I was being critical; I am really trying to help. Boring accurately on a part like this requires that we control every single variable we can.

If this was my project, I would probably bore the through bore first so that I have a really accurate surface to indicate from. I would do the inner bearing bore second in the same set up that I used to bore the through bore. Then I would flip the part and dial in the inner bore to get it dead on or as close as I could get it. Done this way, you should be able to maintain concentricity between the two bores that is well under a thou.

I think part of the problem is the insert you're using. More specifically, the nose radius. The 32.50 insert has a 0.008" nose radius, which is great for general work but a finish cut would require a 0.003-0.004" deep pass and even that is a bit on the light side. A more accurate cut would be a 0.010" pass as this gives the nose maximum support. Of course, you would need to know how accurately the insert will take such a cut but if you stage your roughing cuts precisely enough to get you within 0.020" of final size, you can take two 0.010" passes. The first pass is to make sure the insert is cutting on size and the second pass will bring you in on size.

May I suggest you do some practice runs? Do a practice bore at the same depth and in the same material and do a few rough passes. Measure what the change in ID is with each roughing pass so you know how the insert likes to cut. Then do the same with your finishing passes but try using a 0.010" finish pass. Most commonly, a 0.010" finish pass will increase the ID by slightly less than 0.020" so either adjust your depth of cut to give you a number you prefer or just work with what you get. For example, if a 0.010" finish pass produces a change in ID of 0.0190" then you know that when you reach 0.0190" of final size, a 0.010" deep pass will bring you in on size. Every insert cuts the way it wants to cut so you have to sort out what yours wants to do. This is because the wear pattern on each insert differs so you have to accommodate that when boring to the tolerances you're trying to hit.

The other thing to do is to contact the insert maker and see if they make a smaller nose radius insert. While this is unlikely with an SCLCR bar, you might get lucky.

The cooling the part thing has to do with measurement. If the part is hot then the bore is going to be larger than when it is cool. How much larger will vary with each part and who knows what that measurement is? You would think that a hot part would produce an undersized hole but from experience I know that sometimes it does and sometimes it doesn't. I agree that being 0.008" oversize is not likely to be due to temp variation but you have to control what you can control.

The other thing is that you said that speeds were "very slow". Can you clarify this? Did you change speeds when roughing to finishing? In general, your tool will cut a particular way at a given speed but it will cut differently if you change speed. This is simply due to tangential cutting forces, which tend to rise as you slow down and that can really throw your accuracy off when you're working to the tolerances you're working at. My suggestion is to set a speed (probably max your lathe can run at) and leave it there. You can change your feed rate and depth of cut but leave the speed where it is.

The other thing I forgot to mention is that feed rates differ between roughing and finishing so when doing your practice cuts to sort out how the insert cuts for finishing passes, settle on a feed rate and don't alter it when doing the real bore. You will find that changes to any of your cutting conditions - speed, feed or depth of cut - will alter how the insert cuts so keep things as constant as you can.

So, make a carriage stop and learn to use it with power feed. Mark your bar about 1/4" or so before hitting the bottom of the bore and power feed until you hit that mark, then kick it out of power feed and feed manually until you gently bottom out on the stop. Try to keep your feed rate similar to the power feed rate and don't slam into the carriage stop.

Good luck on this. If this bore is important, and it sounds like it is, then you really need a carbide bar. Even with a 3/4" steel bar, your max depth is only 3" before you run into deflection issues. Something to think about.

 

[mikey]

I forgot to ask. Are you going for a line-to-line fit? This means the bearing bore is the same size as the outer diameter of the bearing. This is the recommended fit for most angular contact bearings because it locates and holds the bearing securely but minimizes the influence of the bore size on internal bearing clearances. If this is what you're going for, tolerances in the bore are typically in the range of +/- 3-5 microns - pretty tough to measure that, let alone hit it. You can do it but you have to hit the bore dead on so try to control every single variable you possibly can.

I did this kind of bore with this kind of fit for a live center I made for my Sherline lathe. I hit that bore exactly on size so I know you can do it.

 

[GrayTech]

Mikey,

Thank you for the detailed response. I don't feel criticism at all, in fact I am still plenty new to all of this (
You are correct about the part, there are several features on this part, but the critical ones are the back to back bore which hold a pair of angular contact bearings. Concentricity is critical here as any runout between the features would cause uneven loading on the bearings and poor alignment of the ballscrew. I chose .0005" as an attainable value, however I'm trying to hold as tight as I can. The axial distance between the bores is slightly less important, but I wanted to hold better than +/- .005" so I opted to use the compound slide. I gave a .002" tolerance, but it was less critical than the bore.

I agree it was tough to hold these tolerances, but the smallest diameter hole through the part was cut in the same setup as the backside bore which allowed me to indicate it when flipped (The indicator was completely inside the part to reach!).

My plan for sleeving will be to use my 3/4" x 10" steel boring bar, as T Bredehoft commented above. I have confidence I will be able to hold the tolerances with a little more care than might have been given before. I will one day invest in carbide bars, but I can't stomach the costs right now, so a little more skill/luck/care will be required. My bar is a SCLCR with CCGX 31.51 (1/64" radius) or CCGX 31.50 (1/128" radius), I can't remember which I have mounted currently. I have been using these razor edge ground inserts for a while now with good luck. I really can't get them to rub even when taking
You are correct about the use of the compound slide for depth control. I have been thinking of making a carriage stop, so I may have to bump that up on the roster of projects.

In answer to your thoughts:

1. Temperature was kept nominal by the very slow cutting speed, small depths of cut, and application of coolant. I agree it can mess with measurements, but in the case of a bore, wouldn't that tend to undersize the bore? I very well could have screwed up the measurement, we all know I have done that before. I personally don't love the "feel" type of measuring instruments like the telescoping bore gages I used, however I had no other way to measure the bore deep in the part. I would prefer a direct reading 3 point bore gauge, however the money is better spent elsewhere.
2. Insert is relatively new but has removed some material. I don't know if the break in is as important as it is on inserts for tougher materials, but it is a thought. The insert is sharp and has no damage.
3. I've goofed plenty before so I can't rule that one out! I didn't think I missed it, but 8 thou is a serious discrepancy.
4. Cutter was backed off the material before backing out of the bore. I never reverse cut.

I agree that I was surprised to be that much oversize. I might be exaggerating the impact of the spring in the bar and there may be other factors at play here. I think with the equipment I have, I am happy when I hold within .0005" on diameter.

Thanks for all your thoughts!!!

Here is a model of the part:
View attachment 274627
And a cross section showing the bores:
View attachment 274628

Looking at that part, wouldn't it have been easier to bore straight throughfor both bearings at one size and then press in a sleeve for the spacing between them?

Sent from my H3123 using Tapatalk

 

[macardoso]

Looking at that part, wouldn't it have been easier to bore straight throughfor both bearings at one size and then press in a sleeve for the spacing between them?

Sent from my H3123 using Tapatalk

Yeah, that would have been a good idea! Only thing would be that it would need to be a fairly heavy press fit as that shoulder will be taking all the thrust loads from the screw. Which, if everything goes well, will be very high. These are 1kW 5000 rpm servos for the axis motors.

 

[macardoso]

Mikey,

My experience, and please feel to contradict, is that you don't need a light cut to hit a critical dimension - you just need consistency. I have gotten away with holding tight tolerances in the past when I take my final cut to size at .005 to .010 radial depth of cut. In this way you full engage the nose of the insert and don't have issues with rubbing. If your semi-roughing passes are taken in an identical manner (same radial and axial DOC, spindle speed, and insert) then your final pass should land right on size.

I think that a smaller nose radius insert would be good here, but I think the bigger issue was the consistency of the cut. If you know anywhere to find aluminum specific sharp corner inserts (CCMT31.50), please let me know!

Temperature sure plays a big role in tolerances at this size. I used to work in a metrology lab where everything was temp controlled. We couldn't sign a measurement if the room was out of spec.

The "very slow" spindle speed (100 rpm) was due to bar resonance at higher speeds. I might have been able to go even faster, but I found the chatter to subside at 100 rpm. A carbide bar would really help here.

I will be practicing before I make the final cut! Re-boring it for the liner will be a good test too!

Since this is aluminum, those tight of fits really don't matter quite as much. It will stretch far more than a solid semi-hard steel would. That being said, I'd like to keep it somewhere around a light press to a very tight slip fit. I figure this is in the -.0004/+.0002 range. I'm not sure how much tighter I can hold with my skills and equipment at this time.