Thread Milling

[TurboDude93]

I need to thread mill an 8-36 thread into a glock slide for an RMR sight. What size thread mill do I need? I would guess a number 8 thread mill? Thoughts?

 

[D Nelson]

We use 6 /32 threadmill the dia. Is .118


Sent from my iPhone using Tapatalk Pro

the thing to watch is the right screw goes into the ejector rod hole and it is not centered in the hole the drill and tap are half in and half out so be careful

 

[D Nelson]

I use Kyocera drill and a spiral flute threadmill they seem tougher emuge


Sent from my iPhone using Tapatalk Pro

 

[Hazzert]

If you are using a multi point threadmill you’ll need any 36 TPI threadmill #8 or smaller. If you use a single point threadmill any threadmill that will fit in the hole with the correct TPI or less is close enough.

 

[TurboDude93]

Can you post pictures of the thread mill and drill? I am curious about this.

 

[D Nelson]

I can tomorrow for you. I’m home now. We got a lot of snow today but will probably be at the shop tomorrow. Don


Sent from my iPhone using Tapatalk Pro

 

[TurboDude93]

How deep do you drill? And how deep do you take the thread mill? I have never thread milled before, so this is daunting to me.

 

[D Nelson]

How deep do you drill? And how deep do you take the thread mill? I have never thread milled before, so this is daunting to me.

.450 deep threadmill to .350 deep from top of slide not to bottom of site cut


Sent from my iPhone using Tapatalk Pro

 

[D Nelson]

.450 deep threadmill to .350 deep from top of slide not to bottom of site cut


Sent from my iPhone using Tapatalk Pro

here is some magwell extensions we threadmill also



Sent from my iPhone using Tapatalk Pro

 

[precisionmetal]

We use 6 /32 threadmill the dia. Is .118

The thing to watch is the right screw goes into the ejector rod hole and it is not centered in the hole the drill and tap are half in and half out so be careful

Don,

I've never done that installation -- would it be possible to insert a "consumable" rod into that ejector rod hole for the drilling op, then pull it out either after drilling or after drill/thread mill?

Just curious...

PM

 

[D Nelson]

I don’t but I drill slow like 2 ipm 5500 rpms give it time to do its thing. I use a short 3 mm drill so it is tough the bit is probably.5 inches long. I go easy some of them slides are pretty hard. A colt cold cup stainless is very hard


Sent from my iPhone using Tapatalk Pro

 

[D Nelson]

I don’t but I drill slow like 2 ipm 5500 rpms give it time to do its thing. I use a short 3 mm drill so it is tough the bit is probably.5 inches long. I go easy some of them slides are pretty hard. A colt cold cup stainless is very hard


Sent from my iPhone using Tapatalk Pro

Sent from my iPhone using Tapatalk Pro

 

[D Nelson]

Ok here is a couple of pics

drill is Kyocera 3 mm and threadmill is niagara spiral flute 32 tpi


Sent from my iPhone using Tapatalk Pro

 

[TurboDude93]

My next question is how to write the G-code for this? I am using an 8-32 screw, any thoughts on this?

 

[706jim]

An easy way to create a thread mill program is to use G41 G1 to get to the thread OD radius, then write a simple subroutine that indexes up the thread pitch in Z every 360 degrees. Use L for the number of repeats to get the depth you need.Then G40 G1 to get back to the center and retract.

Or there are thread milling routines that you should be able to dig up somewhere on the net.

 

[TurboDude93]

Thank you, I am fairly new to writing programs, the reason I am asking is because my CAD/CAM for some reason doesn't have thread mills in it.

What would said subroutine look like??

 

[706jim]

O1
g90g0x0y0z1.0m3s1000
g1z-0.320f20.0m8
g41y0.078d21f1.0
m98p2l11
g90g40g1x0y0m9
g0z1.0
m30

o2
g91g3j-0.078z0.0313
m99

Can't get this site to print upper case G and XYZ codes.

Main program positions tool and enters cutter compensation. Sub program repeats a full arc with Z index. You may experience a slight pause as the sub repeats, but this has worked ok for me in the past.

 

[precisionmetal]

Thank you, I am fairly new to writing programs, the reason I am asking is because my CAD/CAM for some reason doesn't have thread mills in it.

What would said subroutine look like??

What are you using for CAM?

 

[TurboDude93]

Fusion 360. I cannot for the life of me find the thread mills. I do not know if it is in a different tool library that would need to be uploaded? I only have the one thread mill, so these will have to be super super light passes

 

[yugami]

Just make a new tool. Thread mill is a tool type.