What's new
What's new

Angled hole to a flat surface

rokstarr999

Aluminum
Joined
Feb 7, 2014
Location
Sonoma County, USA
Good Morning,

Looking for some tips on the correct way to machine the 2.125" holes into this plate. It's 5.5" diameter plate with a 2.25" x 4.437" rectangle boss centered on the back side. I know I'll have to use a sine plate in our CNC mill or keep it simple and grab the square boss in a vice and tilt the head on the manual mill Would a tooling ball be the correct way to locate the center of the hole?

Thanks in advanceCNC HELP.jpg
 
In a word. Yes.

Although with bores that size you could just set the plate at the angle you want, guestimate as close to location as you can, bore a smaller hole thru, check location, adjust and machine to size.
 
How should you do it? Its probably going to suck.

If I had to do it where you are at now, my first thought is to
use the rectangle to hold it, and ignore the round thing.
Of course the round thing has to be down, which complicates things.

2 soft jaws that are long enough to span 2 vises. One machined.
One plain. Lay the jaw down, put in a pocket at the appropriate
angle to hold the rectangle. Add a locating feature (this is where
CAD comes in handy. Bolt jaws between 2 vises and bring the part
up from underneath, squeeze and machine, maybe use a screwjack underneath.

I probably would have preferred to start off with the bottom plate being
square, and then machining it round last, after all the holes are in.
Then you could have just grabbed it in some angled soft jaws.
 
How should you do it? Its probably going to suck.

If I had to do it where you are at now, my first thought is to
use the rectangle to hold it, and ignore the round thing.
Of course the round thing has to be down, which complicates things.

2 soft jaws that are long enough to span 2 vises. One machined.
One plain. Lay the jaw down, put in a pocket at the appropriate
angle to hold the rectangle. Add a locating feature (this is where
CAD comes in handy. Bolt jaws between 2 vises and bring the part
up from underneath, squeeze and machine, maybe use a screwjack underneath.

I probably would have preferred to start off with the bottom plate being
square, and then machining it round last, after all the holes are in.
Then you could have just grabbed it in some angled soft jaws.

I didn't think about laying a soft jaw down and machining the angle in it. Much easier than fixturing to a sine plate. And the 5.5" diameter is at that top of the hole so grabbing the boss will work great.
 
In a word. Yes.

Although with bores that size you could just set the plate at the angle you want, guestimate as close to location as you can, bore a smaller hole thru, check location, adjust and machine to size.

This would work. The shift after sweeping the tooling ball at that angle is only .008" Took me a while to draw this up in cad. Fusion isn't very cooperative...or I just don't know how to use it very well...lolCapture.jpg
 
The only tolerance I see on the drawing is a +0.003/-0" on the diameter of one of the holes. Is there a note on the drawing about the others? That would influence how this is approached.

Rokstar999 talks about the first problem I see here and that is just where do you need to line up to locate the angled bore. Just putting the tooling ball in a center hole on the original surface of that side does not place the center of that tooling ball on the axis of the needed hole. There will be some offset and he claims he has calculated it at 0.008". That sounds high to me, but he did not say what size tooling ball he was assuming and the offset will change with that size. (The 0.008" offset with an angle of 1.5 degrees seems to imply a tooling ball who's center is about 0.305" above it's base. Perhaps not as high as I first thought.)

As to how it is held, again that depends on those stupid little things called tolerances. If the angle needs to be held down to arc seconds, that is one thing, but +/- 1/2 degree is another.

My approach would definitely depend on the needed tolerances.

Another fuzzy thing on the drawing is the location of the point where the axis of the two holes meet (square one and angled one). It appears to be at the right side of the overall plate, but that is not really clear. This is an important point when calculating the offset from the center of the tooling ball.
 
If the angle is relatively shallow I would clamp a square sided vise, like a Kurt 3600, at the correct angle in another vise. It is a really convenient way to hold parts at a shallow angle. Just hide the vise handle for the lower vise, it makes you feel real dumb if you loosen it by force of habit.
 
The only tolerance I see on the drawing is a +0.003/-0" on the diameter of one of the holes. Is there a note on the drawing about the others? That would influence how this is approached.

Rokstar999 talks about the first problem I see here and that is just where do you need to line up to locate the angled bore. Just putting the tooling ball in a center hole on the original surface of that side does not place the center of that tooling ball on the axis of the needed hole. There will be some offset and he claims he has calculated it at 0.008". That sounds high to me, but he did not say what size tooling ball he was assuming and the offset will change with that size. (The 0.008" offset with an angle of 1.5 degrees seems to imply a tooling ball who's center is about 0.305" above it's base. Perhaps not as high as I first thought.)

As to how it is held, again that depends on those stupid little things called tolerances. If the angle needs to be held down to arc seconds, that is one thing, but +/- 1/2 degree is another.

My approach would definitely depend on the needed tolerances.

Another fuzzy thing on the drawing is the location of the point where the axis of the two holes meet (square one and angled one). It appears to be at the right side of the overall plate, but that is not really clear. This is an important point when calculating the offset from the center of the tooling ball.

According to the drawing I have +/- 1 degree on all angles which makes zero sense. Everything else is +/- .005 for .xxx This drawing is dated 8/12/70. And your correct about the tooling ball height being .312" from center to shoulder. I think my plan for the angled features is to machine a soft jaw at the correct angle, sweep the ball, run one pocket and then spin the part around and run the other pocket. I'll ream .250" holes for the tooling ball when I cut the rectangle boss.
 
Just hide the vise handle for the lower vise, it makes you feel real dumb if you loosen it by force of habit.

Been there and done that countless times, so I made a bunch of these.
Vise Stops.

48690807571_c424954c82_c.jpg
 
The lathe I run now has a barloader. I just put it in barloader mode and the pedal doesn't work.

Wasn't always that way.
 
It’s such a shallow angle. Me, in my ignorance, would attempt to do them flat in the vise and interpolate it with a boring type spiral toolpath. It’s slightly undercut on one side, so a tool like a dovetail cutter (flat bottom, multiflute, single point contact) with a .02 radius, and use .005-.01 step downs. Too bad it has that step where the angled bore meets the straight, but a smaller diameter cutter(1/2” or smaller) would leave an acceptable crisp step for the tolerances, I would expect.

No fancy setup, just cnc. The cycle would take way longer, but reliable and takes the human error aspect out which is usually where my setups fail. If just a few I’d trade reliability for speed any day.


Or you can clamp it to a tilting/rotary table.
 
Last edited:








 
Back
Top