DESPERATELY need help with deep hole bore!

Hello fellow machinists.

I'm having some trouble finding a solution to my issues.

Heres the situation:

I am working with a HAAS UMC.
I am required to create a hole 20" deep, with a diameter of 2.5594" +/- .0004" in two conjoined parts made of A356 T6 aluminum
The two parts are roughed individually, then mated together with press fit pins, and then mounted to the fixture. It is then rough cut with the boring tool again and then finally finished with some very light finish passes. The bore is at the center of the seam.

I have been able to produce good results using a modular single point boring tool. (D'andrea), and I am able to check my results using a sunnen dial bore gage.

My problem is it takes me 10-15 hours to create this bore... I start with a very ugly rough bore and use a .016R nose insert and take .006-.008" off dia with every rough/finish pass. Feeds and Speeds for rough pass is .6ipm and 700 rpm. I have to take about 8 rough passes to get withing .010" of my required dimension. I then switch to a .008R nose insert and take .001-.002" pases and take 4-6 passes to get to my finish dimension Feeds and speeds for the finish pass are .3ipm and 700rpm

If I try to push it any harder or faster, my cutter vibrates and gouges the bore resulting in lost time when I have to remove the part and get it welded for repair.... then rough out the welds individually to somewhat match the bore, then reassemble the two parts, re-setup, and then finally start boring again.

The part is for automotive applications, specifically the crankshaft main bore for a horizontally opposed motor.

My question is.... IS THERE A BETTER WAY???

Can anyone who is in the automotive manufacturing industry or any experts on deep bore holes? Right now we have a french company "ittede" working on a quote for a custom tool but is there anyone out there that is already doing this (or something like this) successfully?

Please help!

Is this For the fa20 engine?

Is it a blind or through bore?

First of all, you're cutting less than the tool nose radius. Not a dealbreaker, but certainly less than ideal since it will cause long chips and more deflection.

Also, what happens when you take the whole 0.010" off in one or two passes? Too much vibration?

My calculator tells me you're running at .001-.002 per pass at 0.0004 IPR. No wonder it's taking forever.......



If all else fails you could try a drill for the roughing cut and a massive reamer for one finish pass.

Like this for the drill: Allied - Item Detail

And this for the reamer: Allied - Overview

As you can see, the drills go up to 4.5" by 28xD; the reamers go up to 7.8" with a modular shank. And they can be adjusted 5% to dial in the bore size.

What he said^^^

I did not really consider feeds and speeds. I do start at a good point and see with my eyes adjustments to make. Splitter does state the obvious. I did not really notice.


Yep what one can do in your spot is avoid overworking the hole.

Long parts which a shop usually has not done are often under bid which applies pressure.

Remember taking out .01 on the I’d is only .005 per side on a small nose radius a larger cut will go a way towards cutting vs rubbing.
Under bidding is really common. Despite what they say do it right. Show you are open to improving it as always yet sometimes pushing it without proper tooling or equipment on site can hurt you.

Sometimes it does boil down to the machine and rigidity. Of course largest size id bore tool for the rough hole fit is top of the list. You can gage vibration by allowing enough material on the I’d to take some test passes at different feeds and speeds. It is a process worth the effort.

Plenty of chip expulsion from through coolant is important.

Crankshaft main bore? Then you don't have a 20" bore, you have 4? 1" bores, spaced 6" on center (or so). For roughing, you need a 2 flute boring bar. But when you say Haas and 20" tool I don't get a warm fuzzy feeling.

With your equipment I'd bore half from each end and finish with a line hone.

hsokhi said:

I am required to create a hole 20" deep, with a diameter of 2.5594" +/- .0004" in two conjoined parts made of A356 T6 aluminum

Click to expand...

Picnic on a 2B Devlieg. Too bad you don't have one.

My question is.... IS THERE A BETTER WAY???

Click to expand...

A real machine ? Or a Berco automotive line boring machine would work. Ross has one. Send it to him.

Alternatively, if you're stuck using a hack saw to cut down a redwood, make a 22" long bar out of the heaviest metal you can find that's about .200" under the size of your rough bores, with an integral shank 50 taper or whatever you have, buy five (or seven ? however many mains you have) Microbore inserts, index the bar, drop it .100" away, run it in, raise it up, spin the spindle to rough, index, drop it, back it out, adjust each cutting tool, repeat repeat.

Maybe make two, one for roughing and one set to finish size, if you have a lot to do.

The subaru fa20dit engine
Has a very very similar crank bore size. Anyways I’m a Noob with a 1957 SB16 so I have no real info to give sorry

hsokhi said:

Hello fellow machinists.

I'm having some trouble finding a solution to my issues.

Heres the situation:

I am working with a HAAS UMC.
I am required to create a hole 20" deep, with a diameter of 2.5594" +/- .0004" in two conjoined parts made of A356 T6 aluminum
The two parts are roughed individually, then mated together with press fit pins, and then mounted to the fixture. It is then rough cut with the boring tool again and then finally finished with some very light finish passes. The bore is at the center of the seam.

I have been able to produce good results using a modular single point boring tool. (D'andrea), and I am able to check my results using a sunnen dial bore gage.

My problem is it takes me 10-15 hours to create this bore... I start with a very ugly rough bore and use a .016R nose insert and take .006-.008" off dia with every rough/finish pass. Feeds and Speeds for rough pass is .6ipm and 700 rpm. I have to take about 8 rough passes to get withing .010" of my required dimension. I then switch to a .008R nose insert and take .001-.002" pases and take 4-6 passes to get to my finish dimension Feeds and speeds for the finish pass are .3ipm and 700rpm

If I try to push it any harder or faster, my cutter vibrates and gouges the bore resulting in lost time when I have to remove the part and get it welded for repair.... then rough out the welds individually to somewhat match the bore, then reassemble the two parts, re-setup, and then finally start boring again.

The part is for automotive applications, specifically the crankshaft main bore for a horizontally opposed motor.

My question is.... IS THERE A BETTER WAY???

Can anyone who is in the automotive manufacturing industry or any experts on deep bore holes? Right now we have a french company "ittede" working on a quote for a custom tool but is there anyone out there that is already doing this (or something like this) successfully?

Please help!

Click to expand...

Sandvik make precision boring heads on long devibe bars similar to their silent bars for boring on a lathe.

I have a 45-55mm one that is about 400mm long and like all their silent tools it works exceptionally well. Just treat it like a normal length boring head and it just works.

CoroBore 825

You may have to build modular assembly to achieve the length/diameter you need. They lose some of their effectiveness when mounted on extensions, but are still a huge upgrade from a solid tool.

An alternative might be to use one of their symmetrical lathe bars and make an adapter to mount one of your D'Andrea heads to the end of it.

These tools are expensive, but probably less so than custom application tooling.

Sure would be nice to know the application, but from the bore diameter and 20 " depth, it's not a Subaru. I've line bored Subaru blocks in my VM20 too many times to count, well over 200 by now. IMO this needs to be done on a European style line bore, like Berco, Schou or my Robbi (RMC). I've done Subarus on mine and it's doable, just not as easy to hit the size. You can't use a steady rest on the line bore with a boxer but with a good straight bar it should be no problem, especially with that tolerance.

slowmotion said:

Sure would be nice to know the application, but from the bore diameter and 20 " depth, it's not a Subaru. I've line bored Subaru blocks in my VM20 too many times to count, well over 200 by now. IMO this needs to be done on a European style line bore, like Berco, Schou or my Robbi (RMC). I've done Subarus on mine and it's doable, just not as easy to hit the size. You can't use a steady rest on the line bore with a boxer but with a good straight bar it should be no problem, especially with that tolerance.

Click to expand...

What Subaru engines? The old EJ series? (Ej18/20/22/25?) or the new fa20dit? Because they are very different

Homebrewblob said:

What Subaru engines? The old EJ series? (Ej18/20/22/25?) or the new fa20dit? Because they are very different

Click to expand...

I've also line bored FB25's, they are indeed different with a 73mm mainline. FA20's have the same 73mm as the FB25, unless there is a brand new version that I have not yet seen. The EJ30 has a 68mm mainline. Maybe the OP is boring the 64mm EJ blocks to 65mm for some reason. Oversize o.d. bearings do exist but only +.005", not a full mm that I am aware.

I have done extensive R&D on Subaru mainlines. The cycle time for one pass is now down to 2:30. I've machined out the center 3 bores and installed steel inserts for a customer. It was successful but they then switched to billet blocks, which cured the problem so we abandoned the insert idea. I'd still like to know from the op what the app is. There aren't too many opposed motors out there.

slowmotion said:

IMO this needs to be done on a European style line bore, like Berco, Schou or my Robbi (RMC). I've done Subarus on mine and it's doable, just not as easy to hit the size. You can't use a steady rest on the line bore with a boxer but with a good straight bar it should be no problem, especially with that tolerance.

Click to expand...

Done lots of Boxer style engines on my Berco with a center/steady rest.....just have to turn the case on its side and run the support in through one of the cylinder liner bores.....
Best to come up from the machine base to the case ,not from above as usual with a straight in line..

As to the OP's quest...done lots of long reach bores in that size and reach range using Sandvik Capto tooling on the horizontal spindle of my FP4NC Deckel.....
Cheers Ross

Trepanning tool, take a look for David wilkes on YouTube, there are a few tool building videos, he seems to get good results, final sizing with a supported cartridge tool
Mark

ChipSplitter said:

First of all, you're cutting less than the tool nose radius. Not a dealbreaker, but certainly less than ideal since it will cause long chips and more deflection.

Also, what happens when you take the whole 0.010" off in one or two passes? Too much vibration?

My calculator tells me you're running at .001-.002 per pass at 0.0004 IPR. No wonder it's taking forever.......



If all else fails you could try a drill for the roughing cut and a massive reamer for one finish pass.

Like this for the drill: Allied - Item Detail

And this for the reamer: Allied - Overview

As you can see, the drills go up to 4.5" by 28xD; the reamers go up to 7.8" with a modular shank. And they can be adjusted 5% to dial in the bore size.

Click to expand...

interesting reamer. no lead in angle an no radial lands. wouldnt have thought that works.

Homebrewblob said:

Is this For the fa20 engine?

Click to expand...

for the air cooled porsche 911 crankcases. We are machining brand new castings

Limy Sami said:

Is it a blind or through bore?

Click to expand...

It is a through bore

gbent said:

Crankshaft main bore? Then you don't have a 20" bore, you have 4? 1" bores, spaced 6" on center (or so). For roughing, you need a 2 flute boring bar. But when you say Haas and 20" tool I don't get a warm fuzzy feeling.

With your equipment I'd bore half from each end and finish with a line hone.

Click to expand...

yes technically it is 8 approximately .800" long bores spaced approximately 2" apart




Thank you all for your replies and advice. These are all great starting points. I reached out to my network over the weekend and got very similar answers.

Apparently haas isn't known for very rigid machines but this is what I am working with. It has been great so far for most purposes.

I also learned the D'andrea may not be rigid enough either. If I put my tool in the spindle and hold it (with m19) then set a dial indicator near the bottom of my 20" long tool, with very little force from my hand, I can deflect the tool about .006"
Again not sure if this is due to lack of rigidity from machine or tool or both

I've already done approximately 8 different case main bores with the feeds/speeds/cuts I described in the original post, however on the latest case main bore, it just keeps vibrating out of control... very frustrating. We have changed to a higher quality foundry and heat treatment so the material properties may be slightly different as well...


To summarize what I've gathered from other machinists, these are the things that I need to look into

-I need to try to take cuts that are bigger than my tools insert nose radius (i tried that in the past but remember too much viration, but will try again with even bigger cuts)

-I need to combine this with a higher feed, apparently I should be cutting closer to 1.4ipm?

-Modular single point D'andrea combined with haas umc simply may not be rigid enough.
Will look into the allied, and sandvick tools

-single point at this length may just not be practical. Maybe with at least two cutting points, some of the deflection could be mitigated and there would be more emphasis on


Conclusion
Right now I am cutting "a redwood with a hacksaw" lol
Need to look into more rigid, anti-vibe style, multi-point, cutter for this. Or send it out for the main bore op. Since I'm in SoCal I doubt I would send it to Ross (AlfaGTA?) but worst comes to worst I'll keep that in mind (if hes up to it?). We will see

Thank you all for your replies

p.s. You guys can see some pictures of the cases on instagram @carmansokey

Through hole - easy enough to line bore on a lathe with just a simple between centres boring bar, ..........it's only been done since the days of Stephenson and Newcomen & Watt.

I know from line honing the T6 billet Subaru's that I do that it will take to a hone very nicely. The blocks we get are also have unfinished mainlines, but only .005"-.010". It's also only an 11" reach top to bottom and the KAB6 Kaiser boring shank I use is .020" smaller in diameter than the bore so there is a lot of support for that length. 1100 rpm, .2 feedrate, .0015" depth of cut gives an excellent finish with no chatter. On occasion, I've had to dust the mainline with the line hone. I believe the saddles on a Porsche are the same width so you could easily leave as much as .002" and have them come out the same diameter, especially with the tolerance they allow you. Considering the amount you have to remove, a line bore followed by a minimal line hone might be the fastest method. Of course this would involve an automotive machine shop. Unless you have a lathe large enough, as previously suggested.

If you're doing a bunch, it might be worth calling Ingersoll. They have a team that specializes in automotive engine blocks.

They showed me a custom PCD-tipped tool that gets used for the crankshaft bore, so I know they have experience with it.

Donovan was still using Cincinnati H-40's to machine their blocks around 1980.