Drill and Bore with same tool... with tool on centerline?

[amw]

Hey guys ive been needing to drill and bore with same tool more and more lately and trying to find the best possible way to handle this. Any suggestions on which way to go? 

Option 1 - Create two tools in tool library. One on center for drilling, and one off the edge and using different tool offset number for boring. This requires duplicate tools in library, two offsets in the lathe, and requires me to use offset number not equal to tool number. Right now I have post configured to force offset number to be the same as tool number to prevent accidents, would prefer to keep it that way if i can. 

Option 2 - Use a single tool and program everything with the outside insert. Need to use a X offset in "Lathe Drill" toolpath to bring the tool back on center for normal drilling. Need to remember to touch the outside insert when loading tools instead of just setting on centerline. Im nervous about operators touching tool properly with this method. 

Is there anyway to do an option 3 where I use a single tool and offset with tool set on centerline to drill AND bore? I feel like this would be the safest way to go, but not sure if its possible. Any suggestions? 

[jpatry]

Program the profile cutting to an offset contour, should achieve the same result,

Will run on a single offset, but may also be confusing for whoever is setting up the job

[AHarrison1]

Option 2 is my approach. Im going to use my .75" u-drill as an eg.

The tool is touched off the same way as a boring bar by referencing the outside insert.

To drill I either create a line at centre then move line by half drill dia, .375" and create a finish contour to handle the drilling.

Another way I handle the drilling then boring is to have a points array and program point to point. The points array I keep in A seperate file that I can merge in when needed. This is all handled with 1 tool and 1 tool offset

[amw]

It took me a very, very long time to figure out how to setup the tool so that the center insert, which sticks out further, is on Z zero, and the outer insert still bores tapers properly to size. Might save someone else some trouble so here is how I did it. 

You need to setup a 3D tool. Make sure you use "Edge" compensation.  Put tool center on the outer insert radius, and then adjust clearances to use a negative value to compensate for the center insert sticking out further. You need to play around with the clearance numbers until the other two circles represent the shape of what both inserts will cut together. The edges of these circles are very important. The edges will become the x/z zero point for the tool, and this is what will be used for calculating toolpaths. The 3D file is used to update the stock, but not actually used at all to calculate the toolpath. 

Once its defined you can drill by using "lathe drill" and entering a suitable X offset. And the same tool can be used as a normal boring bar. Can drill and bore with single tool and offset in the machine. 

[crazy^millman]

On 11/22/2023 at 6:55 PM, amw said:

Hey guys ive been needing to drill and bore with same tool more and more lately and trying to find the best possible way to handle this. Any suggestions on which way to go? 

Option 1 - Create two tools in tool library. One on center for drilling, and one off the edge and using different tool offset number for boring. This requires duplicate tools in library, two offsets in the lathe, and requires me to use offset number not equal to tool number. Right now I have post configured to force offset number to be the same as tool number to prevent accidents, would prefer to keep it that way if i can. 

Option 2 - Use a single tool and program everything with the outside insert. Need to use a X offset in "Lathe Drill" toolpath to bring the tool back on center for normal drilling. Need to remember to touch the outside insert when loading tools instead of just setting on centerline. Im nervous about operators touching tool properly with this method. 

Is there anyway to do an option 3 where I use a single tool and offset with tool set on centerline to drill AND bore? I feel like this would be the safest way to go, but not sure if its possible. Any suggestions? 

MT will not allow Option one just so you are aware. Option two is you best option which you already figured out.

[amw]

I had another attempt at this today and I managed to get the origin on the center of tool, and get it compensating to the edge of insert properly. It will do a finish bore cycle perfectly. But for some reason, no matter what i try, i cant get a roughing cycle to recognize remaining stock. Maybe because the center of the tool isnt actually cutting anything? Still strange since it works in a finish toolpath.

While I was struggling with this I thought of another problem. If I do it this way, the diameter in the program is not the actual diameter being cut so it would mess up all the surface speed and RPM calculations too.

So its obvious now that option 2 will be the best way to go. Only downside is I have a few programs done already drilling on centerline. Id like to keep our procedure of setting up insert drills the same everywhere so Ill have to go back and change those programs but not the end of the world. Thanks for your help guys, hopefully this post might be helpful for someone else in the future too.