TB2 - Small Bearing - Bob W

[BobWarfield]

I was thinking about fixturing on the commute in to work today. Something simple that would make it easy to locate the key items, maximize the opportunity for any symmetry on setups, and simplify the rounding over on top. Here is what I have so far:

The fixture is just a base plate with 3 dowel pins, each 3/16" diameter. One is used as a pivot for the bearing hole. The other two are locater pins. You can see from the two how the rounding over works with the pins. I would envision making up a simple handle that bolts to the mounting bolt holes on the bottom of the part.

Manufacturing the part would go something like this:

1. Square the blocks to proper dimensions.

2. Drill and thread the mounting holes in the bottoms. I'm envisioning using the Kurt vise with a vise stop so I can locate one hole and simple flip the part 180 degrees against the stop to get the other hole. This will make whipping through all 16 holes with threading fast.

3. Locate, drill, and ream the bearing hole. Another vise stop situation where you locate once for the first block and then the rest just drop into vise aligned with the vise stop.

4. Place the fixture plate in the Kurt vise. Drop the part on the pivot pin and locate against the lower right pin.

5. Locate the milling cutter to begin the cut with edgefinder, handwheels and/or DRO. BTW, the milling cutter is the yellow object in the CAD drawing. I'm assume a 1/4" diameter end mill in the drawing.

6. Begin the cut feeding very slowly with the part clamped. Monitor the DRO or handwheels. Even a single X-axis DRO is helpful here.

7. Unclamp and do the rounding over until we're against the top left pin.

8. Return the mill table to position, flip the part, and cut the other side while aligned against the lower right pin.

Last stage is to cut the "window" at the bottom:

1. Drill 4 corners. We can use this same fixture with clamping and flipping so we only have to locate top and bottom hole and flip the part to get left and right.

2. Use the fixture to mill out the window by connecting the corner holes. I've assume a 1/8" diameter end mill in the drawings.

What does everyone think of this approach? The fixture plate should be real easy to build and should save a fair amount of time. Others may want to play with the rotab. I have one, but felt this was faster/easier/more repeatable for 8 parts.

Cheers,

BW

 

[Dick L.]

Bob the fixture looks great! Also .125 radii everywhere is good with me. I have a drawing done of my block and I'll post it tonight. Will we thicken the top strap to accommodate the oil cups ?
Dick

 

[BobWarfield]

Dick, I think we're ok on both big and small blocks without thickening the top strap. The oiler just needs a small hole bored and threaded to accept it.

Another thought I had on the fixture is I think I'll cut a window just like the square window on the part in the fixture directly below that square window. I want to make sure the chips have somewhere out of the way to go when the windows are being cut. If the fixture window is an exact analog it can be used to line up the fixture location to facilitate cutting as well.

 

[mklotz]

Bob,

Although I'm not involved with this build, I have a question and a remark.

You wrote:

7. Unclamp and do the rounding over until we're against the top left pin.

Does that mean that you're rotating the part by hand against the cutter, a la my rounding over jig?

If it does, you may want to give that a try on some scrap before building the jig. I tried that with some of Elmer's other fake bearing caps and it was very difficult to control the process due to the large cutter engagement and the tendency for the part to lift.

Eventually I gave up and adopted an entirely different approach to cut the bearing caps. I wrote a specialized version of my ROUNDER program (called ROUNDERA) to incrementally cut the profile with a ballend mill and the part held vertically in the mill vise.

This approach leaves a very finely "corrugated" finish - the cusps between successive ball mill cuts - which is easily dispatched with a vertical belt sander.

ROUNDERA isn't available on my website (too specialized) so, if you're interested in using it, let me know and I'll send you a copy.

 

[Dick L.]

It will be important to have a solid hold on the part when unclamped. I would be inclined to cap the pivot pin with a washer and spring to keep it down flat. Hold the part with an adjustable or some form of parallel jaw tool. I have attached my drawing in PDF. I have .125 radii everywhere but we can surely swap to .062 in the window. Are we going to use oil-lite bushing stock for the small end bearing?
Dick



View attachment Wide Bearing.PDF

 

[BobWarfield]

I'll have enough clearance on the pin to place a collar there as a stop from having the part lift. I'm also planning on making a handle that bolts to the mounting holes of the part and is long enough to provide significant leverage.

Another alternative on the lifting would be to purchase an endmill that spins the other way so the part is pushed down instead of pulled up. I rather like that idea and can always use another endmill or two!

This particular fixture seems so easy to build I think I'll just go for it. If it fails I can always break out the rotab. I designed the fixture so it could fit in the 4-jaw on the rotab if need be as that was my original plan. The second locating pin and rounding over by hand was an afterthought.

Cheers,

BW

 

[Powder keg]

I hope it works OK for you Bob) I'd go straight for the Rotary Table Myself. But like they say. "There's more than one way to skin a cat"

Wes

 

[BobWarfield]

At last, the CNC mill seems to be working, so I started last weekend to try to make the small bearing blocks. Here's how it went:

I'm using MIC6 cast aluminum tooling plate, 1/4" thick. I have glued 2 of these plates together using Loctite, and then clamped them on the ends. The purpose of the Loctite is to hold the part while the CNC mill cuts all the way around the perimeter.

One of the things you have to do with CNC is zero the "DRO". I use that little toolsetter to precisely locate the tip of the cutter. It moves every time you change tools because the tools may be different and because the R8 taper is not designed to be repeatable in Z. I just jog the cutter down until the needle zeros and I know I am exactly 2.000" from the bottom of the setter. So I set my Z DRO to 2.000".

For X and Y, I jog the cutter down close to the workpiece and position it where I want the lower left corner of the part to be. Doing this by eyeball is more than adequate for this operation. Zero the X and Y "DRO" (it's just a DRO-like display on the computer screen) and I'm ready to begin.

I broke down my part into 3 different g-code programs. One cuts the insider pocket. One cuts the outside profile. And one is a peck drilling cycle for the bearing hole. I just feed the reamer by hand using a slow jog. You can see the inside pocket is done and I'm working on the outside profile.

Pretty soon (1/2 hour) we have a part! It's held to the bottom plate by the Loctite, so I can just knock it out with a piece of wood and a little mallet tap.

 

[BobWarfield]

Here are a couple of "proto-bearings" (not ready for production yet!):

The one on the right was done with no finish pass, so surface finish is a bit rougher. It was cut with 0.050" depth of cut both vertically and horizontally with a 3/16" 2 flute endmill. The one on the left had a finish pass with only 0.010" depth of cut and that in the horizontal direction only, so it looks quite a bit nicer. In fact, I'm pretty happy with that finish considering the photo is about 3X magnification.

There is just one little problem: I checked the dimensions and its off by several thou in all sorts of ways. DOH!

After much head scratching I finally mic'd my endmill and discovered that the 3/16" endmill was actually 0.1837" in diameter instead of the expected 0.1875".

I'll try again next weekend and see if I can't do better.

Cheers,

BW