Process instability(Boring, Deep Hole Drilling)

[MaticB]

Hello all,

i am having problems with this boring opeartion mainly that i can't reliably hold the 20H7 tolerance(mm), sometimes loosing 0.01mm from the 1st hole to the 2nd.
The main problem it that the entrance surface is angled at 30deg. and the cross hole causing vibations.
Currently i am ramping to 19.8mm then using a boring bar with a 0.2mm radius at 850rpm and 76 mm/min (0.09mm per rev). Thinking of leaving more stock for the boring bar and incresing the feed.

The second problem i have is when i am deep drilling a 5mm hole (125mm deep) the drill is going off centre.
Drilling a pilot 5mm pilot hole 20mm deep then deep drilling with a carbide parabolic drill at 1800rpm and 110 mm/min feed(0.06mm per rev). I know i should increse the feed but the thru coolant isn't clearing chips and you can see them while the drill is retracting.

Material: X20Cr13 - 420 Stainless

Any suggestions? Thanks!

 

[Orange Vise]

How many do you have to make? That'll dictate whether you should keep going down this rabbit hole or just add a secondary process, e.g. honing.

 

[MaticB]

How many do you have to make? That'll dictate whether you should keep going down this rabbit hole or just add a secondary process, e.g. honing.

A few hundred per year. We also want to run them unattended.

 

[ViktorS]

Regarding the boring op, not possible to use a reamer instead? Seem to be close enough that a carbide reamer might go in to the next hole before passing the first.

Otherwise, I have found that such slim bars really like to have the full TNR in cut to avoid being pushed. Also, I'd say 0.2 TNR is really tiny for an interrupted cut. The cross hole is problematic, and some vibration will probably always be seen around it with a single point cutting op.

Regarding the deep hole drilling, I have no suggestions. I hate deep hole drilling.

 

[guythatbrews]

We poor mortals cannot divine an H7 tolerance from memory. You'll get more responses if you take the time post the explicit tolerance. I looked it up for you. +.0008"'-.0000".

Unless you can cut the 30* angle and put the cross hole in after boring i think you are chasing your tail a bit. You will always have a problem with discontinuity around the asymmetric features. Even so, the cross hole will be tough to add after boring.

What size bar and overhang? What bar material? What kind of boring head? What insert? Go to .1 mm tnr and maybe rough bore then finish bore. I wouldn't leave more stock, I'd leave less to reduce cutting force effect around unbalanced portion of cut.

I'd have to say orange vise is on the right track suggesting honing. You are the man if you can run this lights out.

My only suggestion on the deep hole is double check all your alignments.

 

[MaticB]

Regarding the boring op, not possible to use a reamer instead? Seem to be close enough that a carbide reamer might go in to the next hole before passing the first.

I've consinsidered a reamer but given the the 30° face i've come to the conclusion that the hole wouldn't be cylindrical and two tool sales rep. voiced the same concern.

Unless you can cut the 30* angle and put the cross hole in after boring i think you are chasing your tail a bit. You will always have a problem with discontinuity around the asymmetric features. Even so, the cross hole will be tough to add after boring.

The raw mat. is a forging/casting so the angle is already there albeit with more stock but not much and the drilling after the hole is done just woulnd't work.

What size bar and overhang? What bar material? What kind of boring head? What insert?

The bar: https://www.sandvik.coromant.com/en-gb/product-details?c=R429U-A12-20060TC09

The Insert: https://www.sandvik.coromant.com/en-gb/product-details?c=TCGT 09 02 02L-K 1515

Go to .1 mm tnr and maybe rough bore then finish bore. I wouldn't leave more stock, I'd leave less to reduce cutting force effect around unbalanced portion of cut.

A second boring bar is also an option but i don't think it would do much.
I thought i would leave more stock to hopefully intruduce more axial force to reduce the vibration while it is cutting on only one side.

My only suggestion on the deep hole is double check all your alignments.

What do you mean by alignments?

 

[DanielG]

Is your machine good enough to interpolate the hole?

 

[MaticB]

Is your machine good enough to interpolate the hole?

Surely you mean a circular contour not a helical interpolation? I dont really know i'll have to try if all else fails

 

[guythatbrews]

I've consinsidered a reamer but given the the 30° face i've come to the conclusion that the hole wouldn't be cylindrical and two tool sales rep. voiced the same concern.


The raw mat. is a forging/casting so the angle is already there albeit with more stock but not much and the drilling after the hole is done just woulnd't work.

The bar: https://www.sandvik.coromant.com/en-gb/product-details?c=R429U-A12-20060TC09

The Insert: https://www.sandvik.coromant.com/en-gb/product-details?c=TCGT 09 02 02L-K 1515



A second boring bar is also an option but i don't think it would do much.
I thought i would leave more stock to hopefully intruduce more axial force to reduce the vibration while it is cutting on only one side.


What do you mean by alignments?

With the angled entry I agree a reamer is unlikely to work.

Your 10mm bar is not helping you at all. You can get a 5/8 or 16mm boring bar with a 20mm minimum bore. You can also modify the 20mm minimum bore bar if you think you need more chip clearance. Sometimes on a job like this you have to modify a bigger bar to get things to work.

I believe if you leave more stock you will exacerbate your problem. A bigger DOC will also increase the radial cutting force and cause more discontinuity around all the asymmetric features. Get a heavy metal bar or a carbide shank bar. The .1 mm TNR will really help. Talk to the insert people to get the best grade and coating for finishing. Mention the interrupted cut. You haven't said but I'm assuming you are running this on a machining center using a boring head. You need a top notch boring head to make this work.

If you continue to have problems you may just have to hone the hole.

On your deep hole problem, by alignments I mean is everything completely true? Have you checked runout on your 20mm deep pilot hole? Is the drill straight and concentric, etc. You might try a high speed peck if the chips are not breaking up sufficiently. If they are packing in the flutes you need to completely retract at intervals. Not something you want to do but sometimes you have to.

Good luck!

 

[Garwood]

I have found through trial and cursing that boring tools that adjust at the toolholder suck shit compared to boring tools with rigid shanks that adjust at the tool tip.

 

[guythatbrews]

I have found through trial and cursing that boring tools that adjust at the toolholder suck shit compared to boring tools with rigid shanks that adjust at the tool tip.

Right you are. Here is a 19mm minimum bore 87mm depth.

https://rigibore.com/wp-content/uploads/2022/09/Straigh-Shank-Boring-Bars.pdf

 

[Garwood]

Right you are. Here is a 19mm minimum bore 87mm depth.

https://rigibore.com/wp-content/uploads/2022/09/Straigh-Shank-Boring-Bars.pdf

I use those in bores from .620 through 12". Very good tools.

 

[Orange Vise]

A few hundred per year. We also want to run them unattended.

At those quantities I'd just hone the bore, either DIY or send it out. Shouldn't be very expensive either way. Under a minute per part and will make a difficult feature downright easy.

 

[ToolmakerTH]

For what I have done with deep hole drilling and reaming on a curved or angled surface, I bore the entrance of the hole with an endmill to be slightly larger than the reamer, usually at the larger side of the tolerance, at around 1.5x diameter deep, then start reaming with the reamer slowly going into the hole at first. I use high performance reamers like Guhring HR500 with high pressure coolant; they can take quite a bit of crossed hole interruptions. If the crossed holes are too much of a problem, see if you can do the critical tolerance deep holes first then drill the cross holes after.

For the 5mm drill at 125mm deep, start with stub drill, then gun drill. Proper gun drilling procedure and a good gun drill with high pressure coolant should be no problem with this hole. Also, do not retract while drilling especially in stainless steel. Pecking will shorten tool life and also can cause drill to go off center ; you need to keep constant tool pressure.

 

[CarbideBob]

The second problem i have is when i am deep drilling a 5mm hole (125mm deep) the drill is going off centre.
Material: X20Cr13 - 420 Stainless

I like this one.
To my cutting tool...Why do you twist, turn and snake? Punch the hole I want that I sent you in.
I loaded your brother and got a good hole and you go kiddywhampus. It is like I have no control.