Folks, I've dremeled and belt sanded all the flash from an aluminum Freeland hooked buttplate casting. Looks much better. Now it's time to cut a through slot for a socket head screw that will fasten this buttplate to the hollow bolt in the Remington 540X buttstock.
The existing buttplate has a 17/64 slot for the bolt shank, and a 33/64 widening of that slot for the bolt head.
I can drill out the length of the slot with a 1/4" drill.
Should I follow that with a 17/64 end mill through and through, followed by a 33/64 end mill, leaving .250 of the 17/64?
spot drill, then drill 17/64. should be plenty accurate for a butt plate. Spot drill is the key here, puts drill perfect on center so it don't wonder off.
Again, a 33/64 endmill would be a rare thing. They make a tool just for socket head pockets. it has a guide pin and cuts the right size. Senior moment don't remember the name. I have an incomplete set of them.
When i don't have the right one, drill with a regular drill, 33/64 in this case, till its the correct depth at the I.D. Then sharpen a drill flat or zero degrees tool bit angle and finish the cut. I keep these drills in my drill drawer so its ready for next time.
17/64 end mills do exist. Cleveland makes em. I will measure the key again to see if I can't use a more common end mill.
Here's the crux - this is a three inch long through slot, 17/64 through, with a wider slot of 33/64 for the bolt head.
The swiveling buttplate is fastened onto a hollow shaft that has a threaded cap on one end. This threaded cap has a mating key that mates with the 17/64 slot, preventing unwanted rotation of the buttplate.
_____ ____ | | | | Think of this like a security standard screwdriver |-----------| with a "U" in the center of the blade. |-----------| | |
The buttplate can slide up and down on this key. The tube is pushed in or pulled out in order to adjust length of pull. Two cross screws in the mounting plate clamp the tube at the desired angle and length.
The critical width is the 17/64 through slot, since too much slop in there would allow the hooked buttplate to wiggle on the shaft. Looking at the design, I could use a mill a little bigger than 33/64 for the socket head, since it is not a critical dimension. A 34/64, or a 17/32, would do nicely for the socket head.
Still, I can do a series of 1/4 inch drilled holes to rough out the slot, followed up with a 17/64 end mill to clean up the sides. Follow with a 17/32 to leave a .250 thick web for the socket head to snug up against.
Then I can finally use my Freeland Mr Cairo Palm rest without the rifle wanting to pivot forward...
sorry misunderstood what you're doing. Just use a 1/4 endmill for your slot. And a 1/2 endmill for the wider slot. You can widen any slot by moving the endmill to one side.
Is there some reason you can't do the whole job with a 1/4" endmill? Maybe drill a 15/64 hole at each end of the slot for clearance and to avoid a deep plunge if the material is thick.
Louis Ohland wrote in news:xGC2q.35622$ snipped-for-privacy@newsfe02.iad:
In my experience, cutting a slot to full width in one go usually results in a rough finish. Having chips flying around getting caught can also mess things up, so make sure you have a good flow of air/coolant (I use a vacuum). I'd use a 1/4" end mill, run it down the middle, and then mill each side in a clean-up pass to get 17/64. It's been a while, but I think you also get a cleaner cut with three flutes because it only cuts on one side at a time.
Louis, Others have mentioned using a 1/4 endmill and moving off center to get the desired width. This is really the best way to do the slot. If you need a full radius at the slot ends then drill 1/4, then 17/64, at the slot ends. When cutting a slot that's the same width as the cutter the cutter will deflect from one side of the slot and dig into the other. This not only makes for an ugly slot it also effectively moves the slot centerline. If you mill the slot in one direction and then the other the slot will be oversize as the side that the endmill deflected away from is re-cut. With a 1/4 endmill hanging out a long way from the collet it is possible for it to deflect so much that one side of the slot will not clean up at the 17/64 dimension. So take light cuts. Eric
I'd use a 1/4" end mill for the whole thing. If you have CNC, this is a trivial project, if not, then you need to do just a little calculating of the right offsets. I get MUCH better results when I am cutting only on one side, and climb mill as much as possible. This gives a much better surface finish.
If you mill the slot in one direction and then the
I get worse results from the drill a series of holes then mill to connect. every time the end mill breaks into a new hole it grabs and pulls and goes off center even worse. Drill only one hole at the start of the slot and slot it from there. I'd go .100 deep each pass. it will take awhile. To finish your 17/64 slot you only need to offset .008" to each side, I'll guess your end mill will deflect more than that and you will only clean up one side of the slot and the other will remain looking like crap.
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.