Live tool drilling with spindle.

[Boxtoolin]

Fighting drill walking off center. In another post I seen a recommendation to drill with a live tool and have the spindle turn at the same time. What % of speed should each be doing? 50/50? I'm running a 3/8 HSS jobber drill into 8620.

 

[guythatbrews]

If you are using 3/8 jobber drill with no spot that is your problem. Ya gotta spot it!

 

[Boxtoolin]

I'm using a 90 spot

 

[guythatbrews]

So the hole is concentric at the start but becomes progressively eccentric the deeper you go?

 

[CNC_Chip_Thin]

I'm using a 90 spot

The angle of your spot drill should be greater than the angle of the drill itself. A shallower angle on the spot causes the outside of the drill to contact first and is likely causing the drill to walk. You want the center of the drill to contact first

 

[SageGlad]

Use140 degree point drill and drill with 135 degree drill bit. Play with speeds and feeds a little to have size you want to see.
No live tooling needed.

 

[Boxtoolin]

Guess I'll explain my process. Although if someone has experience with turning with mill head drilling I'd like to hear your experience. I'm spotting 90 spotting into a 35/64 (.546) (90 spot leaves left over chamfer) to a depth of .750. Then coming in with a 3/8 drill to a depth of 2.17. Both drills are 118. First drill has only .0005 out of round. Back side of 3/8 drill has run out that jumps all over no matter what I do .005-.020. Drills are to size with nice finishes. I've tried carbide and get the same results. I'm indicated in, played with the feeds and speeds to no avail.

 

[guythatbrews]

You need to spot the bottom of the 35/64 hole. The 3/8 drill is walking on the dead center of the bigger drill.

FWIW, although it's common wisdom that the spot angle is > the drill angle. I don't have trouble with 90 spots and hss drills. I do follow the rule for carbide.

 

[Boxtoolin]

You need to spot the bottom of the 35/64 hole. The 3/8 drill is walking on the dead center of the bigger drill.

FWIW, although it's common wisdom that the spot angle is > the drill angle. I don't have trouble with 90 spots and hss drills. I do follow the rule for carbide.

I follow the same rules when it comes to 90 spots. I didn't think about it walking on the bigger drills center. Thanks for the suggestion.

 

[wmpy]

I recently did the live tool / main spindle drilling thing with some small HSS taper length drills. I split the rpms 50/50. It worked O.K. The holes weren't perfect, but they were good enough for my purpose. I only had 20 parts to make, so I didn't bother dialing it in any further.

 

[Ox]

I am not a believer that a shallower angle spot will give you a better run-out at all.
I believe that the whole recommendation of that is for best tool life of the drill.

A steep spot, be it 90* spot or 60* C-drill, should give you a good location, but may chip the corners of your drill.
And then THAT could cause other issue...
With a shallower spot, your tip will hit with a little room to wonder before it seats in.
If I'm really looking for a good tool lilfe, I like to spot with the exact same tool as I am drilling with.
Like if I am using a carbide tipped drill @ 8D, use another stubby 1.5D drill that takes the same insert to use as a spot.


With that said - IDK how on Earth your 3/8 drill would be so far out in such a short distance.

Yes, you can run at 50/50 with fine results unless there is some reason to go to a different ratio.

But first, have you jogged your drill in and out of the hole after it is done?
Doo you see any movement in the drill tip in any direction?
Put your finger on it - can you feel it it the part as it enters the hole?
You need to doo this fast enough that you will see and feel the movement, likely NOT at .001 on the MPG.
Use .01 or just the JOG button.

If you are out of location and have a stiff holder, this SHOULD show up as a tapered hole that the trailing flutes are rubbing on, and not exactly show up as a out of center exit, but ... (???)


OK, another thought, and this can be an issue on rigid spot drills on lathes:
Any chance that your spot holder is a bit out of center?
It is possible to leave a tit in the center of your spotted hole .. for a while ... depending on your material and the orientation of your tool / off center.
If this tit is taller than, or even close to (?) the point in which the shoulder of your flutes starts into the outter taper of the spot, then your drill can get pushed out of center for sure! This is one reason that I prefer to use a longer C-drill in lathes sometimes, especially if your turret is known to be needing aligned. The longer tip of the C-drill hollows out the bottom of the taper, and if you let it hang out a ways, the C-drill will pull onto center if it's not out too far, and if it is, it will break the tip, giving you a hint of what is wrong.


-----------------------

I am Ox and I approve this post!

 

[camhead420]

If its a 135 deg jobber do you need a center or spot drill?

 

[EKrol]

Tried drilling with both spindles turning. In my opinion i don't think this will help you. Drilling with only the turning spindle worked always the best in my cases.

 

[angelw]

Tried drilling with both spindles turning. In my opinion i don't think this will help you. Drilling with only the turning spindle worked always the best in my cases.

In order of hole alignment accuracy, from least to best, its:
1. Workpiece stationary, drill rotating
2. Workpiece rotating, drill stationary.
3. Workpiece and drill counter rotating

The above is tried and true over many decades and not just a hypothesis. Point 2 above is often demonstrated on lathes where the centre line of the tool holder, and hence the drill, is slightly off to that of the rotating spindle. In practice and within reason, the point of the drill will be pulled into alignment with the axis of the spindle.

Many machines that have live tooling don't allow the main spindle to be rotating under normal turning conditions and the live tool at the same time. Rotating the spindle as a "C" axis would be doable, but the max speed wouldn't be well suited to small diameter tools, but the RPM combination of the two counter rotating spindles will achieve the correct surface speed for the drill being used. However, if the OP's machine is capable, it will be easy for him to implement, and there are no negatives in doing so.

Regards,

Bill

 

[Nerdlinger]

Years ago a Guhring catalog said spot with a larger angle for carbide (usually 142 v 140 for me) and smaller angle for HSS (90 v 118.) So assuming your 118 drill is HSS please try spotting to maybe 3/16” diameter, then drilling, then coming back to chamfer and see if it helps. Good luck!

 

[Ox]

In order of hole alignment accuracy, from least to best, its:
1. Workpiece stationary, drill rotating
2. Workpiece rotating, drill stationary.
3. Workpiece and drill counter rotating

The above is tried and true over many decades and not just a hypothesis. Point 2 above is often demonstrated on lathes where the centre line of the tool holder, and hence the drill, is slightly off to that of the rotating spindle. In practice and within reason, the point of the drill will be pulled into alignment with the axis of the spindle.

Many machines that have live tooling don't allow the main spindle to be rotating under normal turning conditions and the live tool at the same time. Rotating the spindle as a "C" axis would be doable, but the max speed wouldn't be well suited to small diameter tools. However, if the OP's machine is capable, it will be easy for him to implement, and there are no negatives in doing so.

Regards,

Bill

In total agreeance with Sir William here.

Years ago I wanted to perform such task on my fairly new Hardinge lathe. It had all the hardware to doo so, but I couldn't make it doo it. So I called Hardinge and asked about it. They faxed me a macro that allowed me to run it. And I still doo to this day on a few deep hole jobs.


--------------------

I am Ox and I approve this post!

 

[wmpy]

Years ago a Guhring catalog said spot with a larger angle for carbide (usually 142 v 140 for me) and smaller angle for HSS (90 v 118.) So assuming your 118 drill is HSS please try spotting to maybe 3/16” diameter, then drilling, then coming back to chamfer and see if it helps. Good luck!

I remember reading this in the Guhring catalog. I believe they said when spotting with a 90 degree center for a HSS drill to create a spot that is 70% of the diameter of the drilled hole. That's what I've been doing and have had good success.

 

[Boxtoolin]

Thanks for the replies and discussion everyone. I think the issue was related to heat, I do not have a through coolant drill right now but I found the more I would baby it, the better the TIR would be. I ended up double drilling the hole using a 23/64 jobber into a 3/8 screw machine length drill. TIR has been within a thou and the finish is good.

Many machines that have live tooling don't allow the main spindle to be rotating under normal turning conditions and the live tool at the same time. Rotating the spindle as a "C" axis would be doable, but the max speed wouldn't be well suited to small diameter tools, but the RPM combination of the two counter rotating spindles will achieve the correct surface speed for the drill being used. However, if the OP's machine is capable, it will be easy for him to implement, and there are no negatives in doing so.

Regards,

Bill

Mazak makes this super easy and it was my first time trying it out. It asks for the spindle RPM and then whatever is left over to match your entered SFM is what speed the live tool runs at.

But first, have you jogged your drill in and out of the hole after it is done?
Doo you see any movement in the drill tip in any direction?
Put your finger on it - can you feel it it the part as it enters the hole?
You need to doo this fast enough that you will see and feel the movement, likely NOT at .001 on the MPG.
Use .01 or just the JOG button.

If you are out of location and have a stiff holder, this SHOULD show up as a tapered hole that the trailing flutes are rubbing on, and not exactly show up as a out of center exit, but ... (???)

-----------------------

I am Ox and I approve this post!

Thanks for this suggestion Ox, I did try jogging it in and out of the hole (giggity) but did not see any flex or movement in the drill. I will add this method to the ole brain bank for future use however.

 

[lethal375]

I have had similar problems with wandering drilled holes in my CNC lathe.
I do not have live tooling.
After checking everything I found that even though the turret was trammed in square to spindle and the tool holder was spot on center, the drills were not straight with axis.
No matter how I checked the collet holder, close to chuck or 6 inches away it was spot on
When I put a precision bar in the collet, the bar was not straight/parallel with axis.
In shallow holes everything was fine but as depth increased hole runout would also increase.
Seen this on tail stocks where alignment is not the same with the quill retracted or extended.
Guys will center the tail stock in full retract then put an indicator on the side of the quill and crank it in and out showing no runout.
But if you extend the quill fully and move the tail stock (on the bed) you will find it is not parallel.
Need to check the tool holder also as the quill can be straight but the issue is in the holder
This is a big problem with reamers and precision bores.

 

[Ox]

Floating reamer (drill?) holders...
I use'm, and I recommend'm.
Y'all can fight the fight.
I like to werk around'm as much as possible and git shtuff out the door...


---------------------

I am Ox and I approve this post!