Internal threading on a turret lathe Rear mounted tools

[Philtrueman]

I am having trouble finding a threading boring bar to work on the inside back side of the work.
In the CNC 12 tool library it seems that i can only put a tool in that is rear mounted to work on the back side inside bore.
The tool library will not allow you to configure a threading tool to work on the inside front of the bored hole.
I had to mount my threading tool upside down "see video" working on the back side of the bore. This was not ideal as the cutting forces are trying to pull the turret away from the locking pawl. It did work. It is cutting a left hand thread 1.75x16tpi UN thread.
I was looking for a 11 size insert and internal threading insert for smaller internal threaded bores.
11ER seem to be for external threads and i can only find 11ir which are the wrong handed insert.
I cannot find any 11NL inserts. 16UN thread
https://youtube.com/shorts/qcXxwnJQDoQ?feature=share
I did get my through coolant boring bar to work.

[suntravel]

Nose Vector OD Thread is 8, ID Thread is 6 on my lathe with front tooling. Works as it should be.

Uwe

[Muzzer]

I don't understand how "the tool library will not allow you to configure a threading tool to work on the inside front of the bored hole". That's an issue for me potentially, as my turret lathe seems to operate in a very similar way, so I'd like to understand more.

How are you generating your g code - are you using Intercon (conversational) or using a CAM program? Perhaps the solution is to either code it fully manually or use CAM. That might generate code that does what you require. It seems the Fusion post processor has got it cracked, for instance.

Insert threading for internal features will be limited to larger bores. You can get smaller insert tools for use down to 8mm or so eg Simturn DX but they are F expensive. I have one of those but given the cost of the inserts, I have only used it for internal profile turning and as a milling cutter. The other option is a solid micro boring bar but they could work out more expensive per broken tool. There are some on Aliexpress that might be worth considering for small threads (£5 each if you buy 5) https://www.aliexpress.com/item/1005004 ... 3683%7Csea
It may simply be best to use a tap. Rigid tapping or a tension compression head should be manageable on these machines.

[cncsnw]

The tool library will not allow you to configure a threading tool to work on the inside front of the bored hole.

I assume by "front" you mean the X- (negative diameter) side, since your turret is in back, and therefore X+ should be to the back.

In that case, you will need to enter negative values for the major and minor diameter (and for the approach/retract X, if needed).

I assume by "tool library will not allow", you mean that when you specify that your tool is an ID Thread tool and choose '8' for the nose vector, you get an indication that '8' is not a valid nose vector for that tool.

That "warning" does not matter. Just enter vector 8 and go about your business.

Alternately, just tell CNC12 that the tool is an OD threading tool instead of an ID threading tool. Then it will accept nose vector 8 without complaint.

[suntravel]

11 IR = internal right
11 IL = internal left

For small ID threads Horn Super Mini System 105:

https://eshop.phorn.de/Gewinde-Inch-105-TP

Uwe

[Philtrueman]

The tool library will not allow you to configure a threading tool to work on the inside front of the bored hole.

I assume by "front" you mean the X- (negative diameter) side, since your turret is in back, and therefore X+ should be to the back.

In that case, you will need to enter negative values for the major and minor diameter (and for the approach/retract X, if needed).

I assume by "tool library will not allow", you mean that when you specify that your tool is an ID Thread tool and choose '8' for the nose vector, you get an indication that '8' is not a valid nose vector for that tool.

That "warning" does not matter. Just enter vector 8 and go about your business.

Alternately, just tell CNC12 that the tool is an OD threading tool instead of an ID threading tool. Then it will accept nose vector 8 without complaint.

Yes on the X- side.
I never thought of telling the tool library it is a OD tool "well done" then it will behave in the same way for entering the thread and exiting the thread. I did have to use the post process for the approach and retract otherwise the tool would crash through the work because the tool has to start at the Z- end of the workpiece.
Is the only difference between external and internal threading inserts the clearence angle underneath the cutting edge? Thanks

[Philtrueman]

I don't understand how "the tool library will not allow you to configure a threading tool to work on the inside front of the bored hole". That's an issue for me potentially, as my turret lathe seems to operate in a very similar way, so I'd like to understand more.

How are you generating your g code - are you using Intercon (conversational) or using a CAM program? Perhaps the solution is to either code it fully manually or use CAM. That might generate code that does what you require. It seems the Fusion post processor has got it cracked, for instance.

Insert threading for internal features will be limited to larger bores. You can get smaller insert tools for use down to 8mm or so eg Simturn DX but they are F expensive. I have one of those but given the cost of the inserts, I have only used it for internal profile turning and as a milling cutter. The other option is a solid micro boring bar but they could work out more expensive per broken tool. There are some on Aliexpress that might be worth considering for small threads (£5 each if you buy 5) https://www.aliexpress.com/item/1005004 ... 3683%7Csea
It may simply be best to use a tap. Rigid tapping or a tension compression head should be manageable on these machines.

The distance between the turret and the chuck is not very much so using any kind of chuck to hold a tap would be a problem.
I just used Intercon to work out the g code. I need to find a way to just run the final pass as sometimes 1 or 2 sping passes are not enough. I had to do 7 on the last job.

[tblough]

To re-run with just a "final" pass, just change the starting cut depth to something large.