Stripped scope base screw hole

Feb 16, 2017
523
16
18
#1
So I picked up a rem 700 short action a while ago and just noticed the front scope base screw hole is partially stripped. The screw will grab and start to tighten, but will not torque to 14in lbs, it will start to spin.

Brownells makes a slightly larger bottom tap/screw kit, has anyone ever used that before? Would I be better off going with a #8? Any other suggestions?
 

mcameron

Sergeant of the Hide
Nov 17, 2011
3,063
3,865
113
#5
Since it's only one screw fill the hole 1/2 way with JB Weld, install the base with the rest of the screws then hand tighten the stripped port, let set for 24 hrs. then apply the correct torque. If it doesn't hold you can always drill and tap later.
ooooooooor.....you could not do that and fix it properly.


fixing it properly involves drilling a slightly larger hole and running a tap.....something most of us could do in our basement......or paying a gunsmith a few buck to do.

that way you arent mounting optics to something that "might hold".
 
Likes: mercracing

ken226

Sergeant of the Hide
Sep 16, 2009
306
87
28
42
Washington
#6
If you happen to be in western washington, id be happy to let you drop by and wait/watch while i fix it for you. No charge.

It would take less than an hour to set it up on the mill on my remington action fixture, indicate the receiver, locate the holes the redrill and tap them.

If not local, just have a local gunsmith do it. JB Weld, despite opinions otherwise is just epoxy. The steel powder may give it some extra compressive strength but that wont do anything for screw threads. Those forces are all shear.

Just do it right the first time.
 
Nov 24, 2011
598
11
18
Brighton, IL
#7
If you happen to be in western washington, id be happy to let you drop by and wait/watch while i fix it for you. No charge.

It would take less than an hour to set it up on the mill on my remington action fixture, indicate the receiver, locate the holes the redrill and tap them.

If not local, just have a local gunsmith do it. JB Weld, despite opinions otherwise is just epoxy. The steel powder may give it some extra compressive strength but that wont do anything for screw threads. Those forces are all shear.

Just do it right the first time.
You don't have your location in your profile, but I'll make you the same offer it you're near St. Louis.
 
Likes: Nooch13
Feb 16, 2017
523
16
18
#8
Appreciate those offers gents. I’m in Pawleys Island, SC. I ordered the oversized tap kit from brownells an I’ll give it a go...I’ll be home from my deer/bear hunt in northern PA on the 2nd and I’ll let you know how it goes
 

Bradu

Full Member
Aug 24, 2011
2,063
301
83
IL
#9
What method do you guys use to locate the holes? I'm learning how to use a mill and would like to hear what you guys do.
 

LongRifles Inc.

Gunny Sergeant
Mar 14, 2010
4,756
257
83
47
Sturgis, S. Dakota
www.longriflesinc.com
#10
You don't drill and tap. That's a great way to make a mess only bigger.

One of the big things that going to an 8-40 thread does for you is its an opportunity to resolve a manufacturing flaw that has intermittently been an issue for Remington; getting the darn holes straight.

Drills like to wander when they get dull. Taps merely follow the hole. IF (and its completely by chance) you have this on your receiver, merely drilling the hole and tapping it, just made the problem all over again.

The better solution:

Have a shop with the ability to helically bore the hole and thread mill the receiver do the work. This way a hole that is off location is not driving the boat. The endmill doesn't care and neither does the thread mill.

I have been doing this very thing for over a decade now. In the cnc world, none of this is really difficult once you "get it." There's a few of us now who have the resources and experience to make it happen.

"We" are who you really want doing this for you.

Good luck.

C.
 
Likes: Badfinger

ken226

Sergeant of the Hide
Sep 16, 2009
306
87
28
42
Washington
#11
Typically for locating the center of a pre-existing hole, i use a conical edge finder.

Put the point of the cone into the hole, dial down about .06" on z, then touch off one side on x, reverse direction, dial out the backlash, then traverse x and touch off the opposite side. Then dial back hald that distance plus the leadscrew backlash and set x to zero.

Repeat for y.

On a cnc, the same but ballscrews remove the backlash issues.

But on a receiver, i like to touch off the receiver OD and front face, the dial to the blueprinted locations and cut the holes with an end-mill.
Making a hole with an end mill, plunge milling, is is sometimes generically called drilling too, but an end mill follows the machines z axis rather than the existing hole.
The pre-existing holes tend to not be exactly where they should be and this method, as long as the holes arent grossly mislocated, corrects any factory tolerancing error.
 
Last edited:

ken226

Sergeant of the Hide
Sep 16, 2009
306
87
28
42
Washington
#12
Ha. LRI beat me to it! ☺

Many Remingtons tend to have the base screw holes grossly outside their location tolerances.
 
Last edited:

ken226

Sergeant of the Hide
Sep 16, 2009
306
87
28
42
Washington
#13
LRI, ive never thread milled a hole that small but i wanna try it. I just never thought it would be economical, particularly in the frontmost hole. A 60$ thread mill in a fairly hard hole, at such a small diameter, seemed like id go through lots of expensive thread mills.

Do you use a single form thread mill for that? You like it better than tapping for that size range? What kinda tool life are you getting?

Would these be acceptable?
https://www.maritool.com/Cutting-To...Mill-.110-Diameter-8-40-UNF/product_info.html

I dont have any canned cycles for thread milling that size, but my thread milling wizard had no trouble generating the g-code.
 
Last edited:
Nov 24, 2011
598
11
18
Brighton, IL
#14
I zero the y-axis of the mill on the bolt raceway using a mandrel and bushings (the same system used in the lathe for the thread and lug truing). This requires shimming the block in the vise with feeler gauges until it is true to the mill x-axis. I then locate all the existing x-axis coordinates with a center finder. I find this works out better than blindly punching out the x-coordinates to published specs as they can be quite a bit off; a decent rail will allow for some slop in holes in the x direction, but you want the y direction to be as true as possible to the raceway center. Then you punch out the holes with a 9/64 carbide endmill and tap to 8-40.

 

LongRifles Inc.

Gunny Sergeant
Mar 14, 2010
4,756
257
83
47
Sturgis, S. Dakota
www.longriflesinc.com
#15
LRI, ive never thread milled a hole that small but i wanna try it. I just never thought it would be economical, particularly in the frontmost hole. A 60$ thread mill in a fairly hard hole, at such a small diameter, seemed like id go through lots of expensive thread mills.

Do you use a single form thread mill for that? You like it better than tapping for that size range? What kinda tool life are you getting?

Would these be acceptable?
https://www.maritool.com/Cutting-To...Mill-.110-Diameter-8-40-UNF/product_info.html

I dont have any canned cycles for thread milling that size, but my thread milling wizard had no trouble generating the g-code.

I only use a single point. I don't care for the hobbs because they have a tendency to bellmouth the hole due to tool deflection changing as the thing winds out of the hole. With a single point, it's the same from start to finish.

Don't let small holes intimidate you. The process is the same regardless of hole size or thread pitch. Just get a small G1 move in there so you can turn on the cutter comp, then let it eat. I always try to climb cut so I start at the bottom and wind out CCW for a RH thread. LH would be the opposite, you start at the top, unless of course you spend retard money and get a tool made to run M4 instead.

Mari is a great source for affordable tooling. Have used them off/on for years. They are my go to for the "little shit" jobs we have around here where it just doesn't pay to put a $150+ endmill in a holder.

Just know this:

8-40 screws don't jive all that well with an 8-40 plug thread gauge. Least the ones we buy don't. If you are going to buy a thread gauge, you'll find your screws tend to waller around a bit more than you probably want. Anymore, we just use the fastener as the gauge to qualify the threads.
 

ken226

Sergeant of the Hide
Sep 16, 2009
306
87
28
42
Washington
#16
Gene,

I made a fixture similar to yours, and also one that threads into the receiver threads about 10 years ago.

Touching off those for y and the receiver face for the x, then traversing x to to Remingtons published locations always put me right over the holes, the same as touching off the OD.

I always kinda wondered, if splitting hairs to find the best location, would i be better off aligned to the raceway (if the base radii maybe then doesnt perfectly match the receiver radii) vs located relative to the threads (also, if the base radii then doesnt match up to the receiver radii) vs touching off the OD, (which then would match the base radii to the receiver radii) but not be quite aligned relative to the raceway or threads. I know, at this point its definitely splitting hairs and the screw to base hole clearance makes it kinda moot , but just as a thought experiment☺

But then, on second thought, having the base to receiver radii match but lose a little alignment relative to the threads puts the scopes center off, and requires a little windage offset from center to zero.

I just decided, rightly or not, that having the base radii match the receiver radii, might be more important than the base to raceway and base to threads matchup.

Whats your opinion on this?

Also,

It seemed to me that the problem i always ran into wasn't so much the holes locations but that they weren't vertical. Dont get me wrong, they tend to be mislocated, but rarely more than a couple hundredths of an inch.

As often as not though, they were drilled at an angle. Obviously that would be cured with an end mill.

Have you found many grossly mislocated?


LRI

I've tried helical boring, but those tiny diameter micro boring bars tend to flex and chatter, and not leave the best surface finish for me. And theyre expensive. Ive always got the best results with a 4 flute carbide mill and HSS tap. What kinda DOC and speeds would clean up the finish?

But, i ordered some multiple and single form thread mills to try. I just never thought to try a tiny thread mill on an 8-40.

On the thread gauges, i found the same. They give a false impression of sloppiness on the #4 thru #10 ish screw sizes. I put together a set of known good screws to use as plug gauges, but still test with plug thread gauges too just to reference.

Your thoughts?

Ill post up a video when i try thread milling one.
 
Last edited:
Likes: Nooch13
Nov 24, 2011
598
11
18
Brighton, IL
#17
I can't really help you much. I don't have CNC so thread milling is not an option. I haven't found any that were off axially, but I've never thought to actually check that. Most of what I see are a few hints of the old 6-48 threads on the sides of the milled out hole. These have never been so pronounced as to affect the 8-40 tapping.

As far as aligning the y's, my first Remington 700 had an issue with the windage needing adjusting as I would go from 100 to 1000 yards in no-wind conditions. It was a fixed amount of about 0.1 MIL per 200 yards. It may have been the scope centerline being off from the bore centerline, or possibly the barrel having some curve in the bore. I try to ensure that the scope rail is aligned and that any barrel curve is aligned to the vertical, though I don't have any hard statistics on how much either of these actually affect point of impact.
 

ken226

Sergeant of the Hide
Sep 16, 2009
306
87
28
42
Washington
#18
Forgive my incessant questions, im cooking and have too much waiting time on my hands. Smoking a spatchcocked turkey over applewood and getting 2 makers mark bourbon pecan pies ready.

No matter how good i may think i am, the discussions i have here on the gunsmithing forum and experience gained by others tend to adjust my own procedures and give me additional insight.

I stopped doing gunsmith work a few years ago with the exception of some long time customers. Mostly nowadays do I do engineering design work, but i still have the interest and try to hone and perfect my gunsmithing knowledge and experience.
 

Rust

Sergeant
Apr 18, 2001
136
12
18
Florida
#20
Ha. LRI beat me to it! ☺

Many Remingtons tend to have the base screw holes grossly outside their location tolerances.
No kidding, I've got one 700 that was so far off a one piece base would take either the front screws or the rear screws. Got around that by using two piece mounts and lapping the hell out of the rings.

Spend a few bucks and have the work done right rather than diddling around trying to do it with a hand held drill and tap. Since your problem is a front screw hole the barrel has to come off because the bottoming tap idea is a non-starter. Old saying, there's always time to do it right the second time.
 
Likes: Badfinger

LongRifles Inc.

Gunny Sergeant
Mar 14, 2010
4,756
257
83
47
Sturgis, S. Dakota
www.longriflesinc.com
#21
Gene,

I made a fixture similar to yours, and also one that threads into the receiver threads about 10 years ago.

Touching off those for y and the receiver face for the x, then traversing x to to Remingtons published locations always put me right over the holes, the same as touching off the OD.

I always kinda wondered, if splitting hairs to find the best location, would i be better off aligned to the raceway (if the base radii maybe then doesnt perfectly match the receiver radii) vs located relative to the threads (also, if the base radii then doesnt match up to the receiver radii) vs touching off the OD, (which then would match the base radii to the receiver radii) but not be quite aligned relative to the raceway or threads. I know, at this point its definitely splitting hairs and the screw to base hole clearance makes it kinda moot , but just as a thought experiment☺

But then, on second thought, having the base to receiver radii match but lose a little alignment relative to the threads puts the scopes center off, and requires a little windage offset from center to zero.

I just decided, rightly or not, that having the base radii match the receiver radii, might be more important than the base to raceway and base to threads matchup.

Whats your opinion on this?

Also,

It seemed to me that the problem i always ran into wasn't so much the holes locations but that they weren't vertical. Dont get me wrong, they tend to be mislocated, but rarely more than a couple hundredths of an inch.

As often as not though, they were drilled at an angle. Obviously that would be cured with an end mill.

Have you found many grossly mislocated?


LRI

I've tried helical boring, but those tiny diameter micro boring bars tend to flex and chatter, and not leave the best surface finish for me. And theyre expensive. Ive always got the best results with a 4 flute carbide mill and HSS tap. What kinda DOC and speeds would clean up the finish?

But, i ordered some multiple and single form thread mills to try. I just never thought to try a tiny thread mill on an 8-40.

On the thread gauges, i found the same. They give a false impression of sloppiness on the #4 thru #10 ish screw sizes. I put together a set of known good screws to use as plug gauges, but still test with plug thread gauges too just to reference.

Your thoughts?

Ill post up a video when i try thread milling one.

It's shown at the :52 second mark.


 

ken226

Sergeant of the Hide
Sep 16, 2009
306
87
28
42
Washington
#22
Beautiful!

Made it look easy!

I think i mistook your cnc boring method due to the terminology.

I've always used "helical boring" to mean boring with a boring bar, where a servomotor spindle maintains the cutting edge position of a single point boring bar using the g76 or g87 fine boring cycle to control spindle orientation during changout, and an offset head is used. Or the part is rotated using a rotary. Whereas the helical movement is provided by the combination of the offset head and the z interpolation.

Ive always known and heard it called, mostly assumed, doing this with a rotating end mill or indexable milling head, as "2d profiling" a hole using helical interpolation.

It probably because the software we've always used, HSM Works, uses these titles for post processing those operations, though, in general, i know "helical boring" is used to describe 2d profiling a hole. It just didnt enter my mind till i saw your video.

But, i now see how your doing it.

Thanks.
 
Last edited:
Feb 16, 2017
523
16
18
#23
So to bump this up, I used the brownells oversized tap kit to fix just the first hole and it appears to have worked perfectly. The only issue is the screws they sell with the kit are WAY to long for the application. Any suggestions on either finding the short screws for the front screw hole or for cutting these down?