PDA

View Full Version : Machining order-of-operations help wanted



Cobbler
05-12-2010, 12:12 AM
I have been working for some time reverse engineering unavailable parts for a High Standard HD Military 22 pistol. This part has me at a stalemate.

http://i187.photobucket.com/albums/x308/kennyrolling/HD11.jpg
http://i187.photobucket.com/albums/x308/kennyrolling/HD12.jpg

This is the safety. The part is .370" wide x 1.175" long x .193" thick.

On the outside, you see serrations over a curved surface, a .75" radius at an angle on one end, a scalloped step with a .75" radius towards the other end and at the extreme end a .221" hole, a .281" x .050" deep countersink, and a .185" radius.

On the back side there is a radius step (forgot the radius because I already cut it), one straight slot cut at an angle, another slot with a radius bottom cut at a different angle, and a staked in ball and spring.

You can see I have roughed out the width to dimension, drilled the hole, and I cut the large radius on the back side using a boring head. Now I'm stumped on what to do next and what to do it with.

At my disposal, I have:
Vertical mill
Horizontal mill
Shaper
Rotary table (with 4 jaw chuck)
Index centers for both milling machines.
Boring head

I'm fairly well equipped with tooling for all above machines. I sure could use some advise or suggestions as far as order of operations and setups to complete this part. I have zero training as a machinist, have never run any machines other than what resides in my own shop and am completely self taught. I try to learn as much as I can here but this one has me stumped.

Thanks!

Here's a link to the whole project.http://garagegunsmithing.com/index.php?option=com_jfusion&Itemid=54&jfile=viewtopic.php&f=21&t=264

winchman
05-12-2010, 01:13 AM
I'd do everything on the back side first. That's the side shown in the second photo. I'd even put the ball in, since it will be easier to deform the edge of the hole around it at this point.

Then I'd do the counterbore around the hole from the top.

Next would be finishing the two long sides and the radius on the end with the hole.

Then I'd remove the extra material over the counterbore and form the radius between the hole and the grooved section.

Then I'd make the radius where the grooves will be, followed by the grooves themselves. Extend them a little long, then cut the finished part free of the stock.

ADGO_Racing
05-12-2010, 01:20 AM
Some fixturing will definitely be in order. It will certainly simplify things.

winchman
05-12-2010, 02:27 AM
Keeping the part attached to the stock until the very end eliminates the need for fixturing. The stock can be held in a vise, or clamped to a rotary table.

You can clamp it to a 90-degree angle (on the rotary table) with the end up to mill the radius where the grooves are going to be. Then turn the RT on its side to mill the grooves themselves. Or you can even cut the radius and the grooves with the RT on its side and the long axis of the stock (and the part) parallel to the mill table.

Do you have any idea how the original part was made?

JCHannum
05-12-2010, 07:29 AM
Roger's order of operations is as good as any. Keeping the part attached to the parent stock greatly simplifies fixturing. Another decision to make is which dimensions are critical to the function and which are merely appearance.

The operations on the bottom side are critical, while most of the operations on the top are appearance. The hole and counterbore for the pivot are critical, the balance of the top can be completed by hand filing if needed.

In pre CNC days, small gun parts were produced on dedicated machines that performed one or two operations. The part was moved from machine to machine to complete. If only making one piece, this is not feasible and hand work can replace many of the non-critical surfaces.

Good luck with the project, the High Standards are good guns.

BadDog
05-12-2010, 07:47 AM
As said, I would keep it part of a larger piece till the end.

As for the odd shapes, us "NC" techniques. As in CNC without the C.

1) If it's a regular curve, identify the radius and use one of various convenient formulas to determine points at regular offsets (in Y or X depending on orientation).

2) For the fluted finger grip, do the same thing but in Z, and no need for filing. Could be roughed with ball end mill and then done with a single lip.

3) For compound curves, blow up some known factor. 10x is good. Then just scale it out, preferably on a drafting table. There are your NC points to machine to. Then file/paper as needed.


Make offsets as fine as needed, then file smooth.

Tony Ennis
05-12-2010, 09:07 AM
How would you machine the ramp-like cut on the back side? It looks like an inside corner is formed.

snowman
05-12-2010, 09:54 AM
The order is already laid out. Basically the order you are already going in :-)

The radius step? Use an endmill of appropriate diameter (radius = radius) and grind relief on the endmill, basically making a t slot cutter.

The radius on the front of the part that contains the V's? File If you know the radius, you can always cut a "female" master then use it with some blue and take your time and hit the high spots. Either that or grind a form cutter for your shaper.

The V's? Use your shaper...a little bit at a time.

The compound radius...ground toolbit in the boring head, just like you did the radius on the back side.

You do good work :-)

Mark K
05-12-2010, 10:30 AM
And, thanks for the Garage Gunsmithing link. They have a new member.

Mark

krutch
05-12-2010, 04:21 PM
A keyseater for the small grooves. The right cutter should give the radius 'ramp'. Serrations? Another post used a tap with the flutes ground off except for one to cut the form. The answers here are all good, so think about it and enjoy your end product!

Sorry! Ground tap won't produce the radius serrations. My bad.

J Tiers
05-12-2010, 08:15 PM
How would you machine the ramp-like cut on the back side? It looks like an inside corner is formed.

Looks radiused to me...... in which case the right sized woodruff key cutter in any mill it fits.....

Cobbler
05-13-2010, 01:21 AM
This is awesome. So many ideas I never would have thought of. There certainly is a lot of talent and knowledge on this site.

Here's what I'm thinking.... Start on the back as suggested. Find the angle of the through slot on the right and plow through it with an endmill in the vertical mill. For the slot on the left, it might be better cut it with a proper size cutter on the horizontal mill but I don't have a proper size cutter for this. I do have a keyway cutter of aproximately the correct diameter but it will need to be ground down narrower. I suppose I could cut stock down a bit so I could get a fairly short vertical hold in the vise to cut it standing up that way.

For those serrations on the radiused surface on the front.... I have done a few projects where I cut a radius on a long surface with the vertical milling machine, a ball endmill, and an Excel program and they turned out very nice. I wonder if using that program with a fixed distance for stepping sideways and use the shaper with a lool like a lathe treading tool would produce the desired effect?

Probably the most critical feature is the distance and angle from the hole to the nose of the radius at the oposite end. This pops up into a notch in the slide when you put it on "SAFE". I fear that his one may be best done by hand on a belt grinder so it can be walked in to the proper length. I have two frames and two slides I'm using to swap parts back and fort to confirm I am hitting "factory specs" and I have noticed that this factory safety I'm copying works with one frame/slide combination but not all combinations.

Mark K
05-13-2010, 11:35 AM
Another possibly workable idea for the serrated radius would have you offset the part in the 4-jaw, assuming the piece is still attached to the parent metal. Turn the radius and plane the serrations with your engraving or slotting tool, which can be as simple as a boring tool. You'd require a simple dividing method for the lathe spindle.

Mark

krutch
05-14-2010, 01:06 PM
I might look at using a lathe ID threading tool in the mill spindle for the serrations. If the serrations are radiused at the bottom, which it appears to be, you could grind that on a used insert.

Cobbler
09-16-2010, 10:55 AM
I did some work on the back side using my Atlas Horizontal mill.

http://i187.photobucket.com/albums/x308/kennyrolling/HD15.jpg

The only cutting tool available for the radiused cut was a gear cutter which left the sides of the slot splaying out a bit... it should not effect how the part works. The other cut, shown below, was made with the vise set at a 5 degree angle. Good thing I didn't scrap this old, broken, crappy vise... the way it cinches down on the table allows me to spin it wherever it is needed.

http://i187.photobucket.com/albums/x308/kennyrolling/HD16.jpg

...and the product of an evenings work (and head scratching). I'm still trying to find a source for a (free, salvaged) ball and spring for the detent.

http://i187.photobucket.com/albums/x308/kennyrolling/HD18.jpg