What's new
What's new

G32 after G76 for thread cleanup?

alek95

Cast Iron
Joined
Sep 23, 2022
Hi everyone,

I am using G76 to single point a thread, no big deal.

This part also has a set screw threaded hole (radial, done with a form tap and live tool). This second thread interferes with the first thread. This causes a bit of damage to the single point thread.

Not too big of a deal to fix by hand, but I need to make thousands of these parts per year so it is a waste of labor.

If I run a G32 threading "cycle" after to make another pass to clean up the single point thread, would the G32 follow the G76 to clean it up?

Never had the need to do something like this before, so all information is appreciated.

Machine is a Doosan 2600SY with Fanuc
 
Can you use a wire wheel on a pedestal grinder to remove the burrs?
Are you tapping first or threading?
 
I want to thread then tap, then come back with the threading tool and run 1 pass to cleanup the single point thread.
 
Oh it's an ID thread. If you're able to thread mill the side hole you'll have less of a burr mushing into the id thread. In fact if you thread mill the ID thread then you don't have to worry about lead-screw timing and have a better looking intersection of the 2 features.
 
Just rerun the g76 with the initial depth set the same as the total depth. It will only make one or two passes, depending om other settings.

G32 might work to always force only one pass. Just use same target x and starting z and rpm.

If you use a cofa tool before tapping you'll get a pretty good ID chamfer. That will help. Or drop through with a back chamfer tool.
 
Oh it's an ID thread. If you're able to thread mill the side hole you'll have less of a burr mushing into the id thread. In fact if you thread mill the ID thread then you don't have to worry about lead-screw timing and have a better looking intersection of the 2 features.
When I re-run this job in a few months it will be with a thread mill on the ID thread (it is on order at our approved supplier so it isn't something I can just get next day unfortunately).
 
Just rerun the g76 with the initial depth set the same as the total depth. It will only make one or two passes, depending om other settings.

G32 might work to always force only one pass. Just use same target x and starting z and rpm.

If you use a cofa tool before tapping you'll get a pretty good ID chamfer. That will help. Or drop through with a back chamfer tool.
I'll try the G32 first and let everyone know how well it works.
 
No. The same helix will not be followed by G32.
.........
To explain why a G32 pass will not align with G76 passes. G76 does an angular infeed so each pass cuts most of the material with the leading edge of the tool. The result is that the Z starting point of the last pass of G76 is not the same as the initial programmed pass.
 
To explain why a G32 pass will not align with G76 passes. G76 does an angular infeed so each pass cuts most of the material with the leading edge of the tool. The result is that the Z starting point of the last pass of G76 is not the same as the initial programmed pass.
Is this true of G92 as well? I have used G92 to spring pass G76 cycles on Haas and it seemed to work fine.
 
No. The same helix will not be followed by G32.
As explained by Kevin. However, G32 will work if the included angle of the threading tool (thread profile angle) is specified as Zero in the G76 cycle and the same Z Start Coordinate is used, or if the Z Start Coordinate shift is calculated based on the Thread Profile Angle and the Thread Height specified. In this case, the Z Start Coordinate for the G32 pass would be moved towards the workpiece by the calculated amount.

Is this true of G92 as well? I have used G92 to spring pass G76 cycles on Haas and it seemed to work fine.
The same would apply with G92 as with G32 when compared with G76. When using G92, there would be no reason to mix it with G32, for a single pass with G92 can be programmed at full depth.

Regards,

Bill
 
The same would apply with G92 as with G32 when compared with G76. When using G92, there would be no reason to mix it with G32, for a single pass with G92 can be programmed at full depth.
That's not how it works on mine. That's why i asked. I program the G92 with the same parameters as the G76 and I can rub on the threads as many times as wanted. It does not end at a different place after doing the 30 degree in-feed.
 
Dumb question, but why not thread the inside after tapping the side hole? I used to do exactly what you are wanting to do, and then just tried it the other way and haven't looked back since. There will be a little bit of a burr in the side hole but a quick flick of a dental pick takes care of that.
 
That's what I'm doing currently, first do the tap while working on the main spindle and then doing threading while it's on the sub spindle.

The 10-32 set screw will not go into the tapped hole without chasing it with a tap by hand.

I guess it's all moot because when the thread mills arrive I shouldn't have this problem. Unfortunately the wheels of corporate bureaucracy can move slowly at time. I've been waiting on the thread mills for a few weeks now.
 
That's not how it works on mine. That's why i asked. I program the G92 with the same parameters as the G76 and I can rub on the threads as many times as wanted. It does not end at a different place after doing the 30 degree in-feed.
It is not like that on Fanuc. I explained above what is required to be done.
Maybe, your control does some internal calculations, depending on some parameter setting.
Or, possibly you used 0 degree thread angle.
 
Dumb question, but why not thread the inside after tapping the side hole? I used to do exactly what you are wanting to do, and then just tried it the other way and haven't looked back since. There will be a little bit of a burr in the side hole but a quick flick of a dental pick takes care of that.

This will lessen the life of your insert.

I run a castle nut, and I have ran enough of them over the years that I have tried a few different approaches to keep the cycle time down, but I git more good parts out at the end of the day (runs 24/7 when it runs) by taking the time to thread, then mill, then come back with a quick version of the threading cycle like mentioned above to clean it back up after the fact.

If I was just tapping, I would prefer to cross tap, and then tap the bore and let a few burrs in the bottom of the set screw hole. They should not really be a problem there in application.


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

Think Snow Eh!
Ox
 
This will lessen the life of your insert.

I run a castle nut, and I have ran enough of them over the years that I have tried a few different approaches to keep the cycle time down, but I git more good parts out at the end of the day (runs 24/7 when it runs) by taking the time to thread, then mill, then come back with a quick version of the threading cycle like mentioned above to clean it back up after the fact.

If I was just tapping, I would prefer to cross tap, and then tap the bore and let a few burrs in the bottom of the set screw hole. They should not really be a problem there in application.


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

Think Snow Eh!
Ox
I haven't seen any noticeable difference in the tool life after the change. But, this it is all hot rolled A36, making spindles for one of our ag customers. I would imagine if it was in tougher materials it would matter more. The costs are negligible your way or mine any way.
 
Is this true of G92 as well? I have used G92 to spring pass G76 cycles on Haas and it seemed to work fine.
On Haas's I have done the same with no issue, but on Fanuc lathes like our old mori's it would not work for the reason's that Bill said. The z starting point will not line up. You can Follow what Sinha said , but it is just easier to use a g76 to follow a g76.
 








 
Back
Top