Can you use a flat bottom drill as a boring bar? I have a T-Cap Ingersoll Multi purpose drill I want to program.

[alphawireedm]

https://www.ingersoll-imc.com/product?ecatProductId=413999  Here is the tool I'm working with, other manufactures make a similar tool that is capable of flat bottom drilling then stepping out and boring amongst other tasks. 

Here's a video of what its capable of doing

https://www.youtube.com/watch?v=c10M5hCROXg

I have it set up and am programing it as a boring bar just fine but I want to use it as a drill too. Obviously the tool type wont allow me to use a drilling operation, but I was hoping there might be a way to trick a ID profiling opp to mimic a drill movement since I don't need a peck. Then I could save it into my template for this part family rather than copy paste and modify something like 

G0 X.650

G0 Z.1

G1 Z-.250F.0025

G0 Z.1

[johnswetz1982]

You have to create a copy of the tool as a drill with a different offset number. An example would be T0202 for the drill and T0214 for the boring bar.  

[Anonymous]

Not my preference but yes, you can do what's shown in video, providing you have the range in X axis to do it.

Programming that boring cycle is going to be small challenge as your tool will still be oriented to work from center line outward and you will get positive X coordinates.

You can mirror that part of the code or use 101 (I believe) in turret setting of last tab in tool definition to produce negative X coordinates only for boring.

You can use it as drill providing you set tool to have inner insert edge right on center line, not short of it and not overlapping it.

If it falls short, you will build up needle like material that will bust the inner edge of insert because it has nowhere to go as drill progresses.

If tip overlaps center line it will be busted by opposite rotation of spindle relative to cutting edge.

Moving on, overloading of insert tip by using tool as boring bar and turning tool as shown in video will cause inefficient use of cutting edge and premature failure due to disproportionate use.

In order to control bore and OD size separately you will need 3 offsets, one for drill, one for boring bar and one for turning tool.

This puts all your eggs in one basket and even though it saves you fractions of seconds by not indexing turret to call different tool, it has potential to cause damage that outweighs any gain.

Other then that,.... yes you can do it but you may soon discover new way to do welding on CNC lathe.

[alphawireedm]

Seems like I should rephrase the title, I have misled you guys, I was not
asking whether or not this can be done with the tool. I already use a
similar tool to do drilling and boring operations and have for the past 6
years. (It works great by the way) I just want to know how to program it in
Fusion 360. I program it as a boring bar for the boring portion of the
cycle but I need CAM the drill function rather than do manual entry into
the program.

[Anonymous]

Well, thats easy,

define drill size for its diameter,

use 180 degree for tip angle

set it as 1 flute

set chip load value

set it as static drill (clear live tool box)

in drilling operation, use "Drilling - rapid out" option in drilling operation.

If you feel adventures, use pecking cyclen, chip breaking cycle, not full retract,........ I know, I know,... opening another can of worms here, but hey,....... 2" diameter drill works great on Inconel 718 going 10 inches deep and pecking all the way at .01 deep peck. and .002 / rev feed rate.

If you never tried it, put it on your bucket list.

[seth.madore]

@alphawireedm to use it as both a boring bar and a drill, you are going to need to create two tools. Fusion doesn't yet support dual purpose tool, unfortunately. So, create a drill, and then create a "boring bar" of the same dimensions. Apply the same tool number to each tool

[alphawireedm]

Sounds like a viable approach, How do you get the drill to drill at X.650?
Maybe enable y axis or something?

[chris]

@alphawireedm

by setting up the second tool as a drill you give it the same tool number but give it a different offset, the offset value that puts the tool center (or whatever offset the too requires from center to drill a hole) and give that offset a different value, in my fanuc control I would use say T1010 for drill mode and T1013 for boring mode and if you want to set it up for external turning you might have to give it another offset value in a 3rd tool T1014 for example that way it calls the same turret pocket but loads the offset value that correctly corresponds to your operation and tool position requirement.

I am just now going through setting up a similar tool, so if this is all old news to you and you have picked up a few tricks please do reply and offer your experience!  🙂

[jswickJ9PWC]

Heres how I ended up doing it with an Iscar version of the same drill:

I created a grooving tool with the insert set to the drill diameter, round shank, and the center set to "Insert Center"

I then used the Single Groove toolpath and using sketch points, selected the points I wanted it to cut to.

[chris]

is there a reason you wouldn't just define it as a drill and boring bar?  would seem then no sketch points would be required?  you should be able to measure the tool for x offset by the turret bore for center and offset the amount required for the tool to center cut like a drill (if it is required for the tool, as I saw some variations of the tool required a small offset for drilling operations, I am guessing to get the inside corner of the insert on spindle centerline).

Then for boring operations it would just be used like any regular boring bar with the X offset set to the outside of the insert cutting point edge inline with the spindle center.  On mine the tool faces down with outer edge pointing back towards the turret centerline, so it would use M3 clockwise rotation and for boring internal pockets all step outs would be in the X positive direction which is no different the any other boring operation with tool in this orientation..  so for any operation the tool would never be more then a small distance below the tool center spindle centerline position and that should be easily compensated for when setting the X tool offset.

This is at least how I am envisioning it, is there any specific reason this wouldn't work in your situation?

Thanks,

Chris

[jswickJ9PWC]

Simply because I'm still the new guy here and I have to make the code output like what the long-term guys like, hahaha.

[turbobug64]

You apparently can't define a drill in lathe tools. You have to use mill tools and that limits you to using IPM with the drill and IPR for everything else.  Pretty stupid. 

[seth.madore]

@turbobug64 I'm 99% certain this is false, regarding IPR/IPM. Yes, it does require a post processor edit, but the IPR field IS passed onto the post processor.

A drill is neither a LATHE tool or a MILL tool, same as taps and reamers. They had to exist somewhere, and since milling existed first....

[turbobug64]

Well why is there no tick mark in the speed and feed when I make a drill from the milling tab? That tells the PP what to use in the code does it not?

[chris]

mine had feed per rev listed:

[seth.madore]

That's an entirely different question, and the answer is that it's likely just not been implemented yet. The post processor can be modified to either always post out IPR, or we could also have a user toggle to the effect of "Use IPR for drilling"

[seth.madore]

@chris yeah, but @turbobug64 is looking for this option:

 

[turbobug64]

Yes I am. If you just put that tick mark option in drills just like the rest of the turning tools my issue would be solved. 

[seth.madore]

I can 100% guarantee that the post processor edit route is going to get you a solution LONG before that checkbox is implemented

[chris]

I could see that being useful.  options are always good, and having to change a post seems a bit tedious especially if you wanted the capability for switching between per tooth and per rev.  seems like the post change would need to be changed or manually edit the program post as needed if that was a requirement for your part program.  in the interim isn't is the same to just divide your desired feed per rev by the number of flutes the drill is?  not sexy but i would do that before I implemented a PP change.