Re: [CAD_CAM_EDM_DRO] Eccentric Follower

Darrell, Ballendo, Carey, Dave, et. al.,

Yes, I saw that. Really makes me want to get the Rotary table!

Darrell wrote:

> Alan,
> If you don't have 4th axis, it looks like you will need to finish it up on
> the lathe. Chuck it with the big hole and cut the slot between the ears.

> A lot depends on the size of the cutter. I probably wouldn't cut any deeper
> than the diameter of the cutter with that mill and never cut thicker than the
> radius. on the finish pass (just taking off a couple of thousands) I would
> cut the full depth.

What size end mills? I have .125 and .25 and larger... for now. I
think I'd much rather mill the slot, then have to cut into the
off-center "ears" on the lathe. I've cut eccentrics that way before, a
slot for a crankshaft or this part would be a little rougher. I have the
5" Sears/EMCO "Compact" (?) lathe of about 14 years ago. I've found a
new supplier for the lathe, so I can get the remainder of the
accessories (at a higher price then before!).

>Not having seen the part, I would clamp the raw stock in a vise and drill
>the holes. Then I would face the block off to the required thickness. Then
>I would drill a couple of holes in a block of steel at the same positions as
>in the part to make a mounting fixture, tap them to take bolts and mount
>the stock on the block clamped in the vise. (make the block small enough
>that the part hangs over on all sides) If you have G41/G42 cutter comp,
>tell the control that your tool is larger than it really is and the machine
>will cut a roughing pass. Reduce the tool size untill you are using the actual
>tool size for the final cut. If you dont have G41/G42, you will have to draw each
>tool path.

I like the mounting fixture, sounds like a good way to go. I could
probably use the fixture in the lathe, too. Reducing the tool size keeps
you away from the final contour?

Ballendo wrote:

>A lot of times generating the code is the easiest part of making the
>part. Thinking through the process takes the time. If I understand
>the part correctly(.jpg,yes please.), I would do the bore(s) first
>while holding the block with flat clamps. Then I could USE the bores
>to locate and hold down SECURELY for the outline contouring. (I'd
>prob'ly also cut the slot 'tween the ears b4 the outline cuts, while
>the pear was square).

.JPG's in the Files section. Well, I've got the little Sherline Mill
vise, and square stock is easier to hold.


Carey wrote:

>Alan: I would bore the big hole first. Then I would stand the block up
>in a vice and end mill the slot to rough it in. Then put an arbor
>through the hole and turn in a lathe. Then mount it flat through the
>hole and drill the small hole. Fixture it down with both holes and mill
>the cam contour. At this point there is not a lot of thickness to deal
>with . That is the way I would go about it.

The initial slot milling might get me by when I get to the lathe, then
there wouldn't be so much material to remove.


Balendo wrote:

>1. clamp a thick sub-plate on the mill table, hangin' over the front
>of the table (he has a sherline,guys)
>2. mill the overhang to a clean 90. We'll use it later.
>3. clamp the stock (1.125x1.875x.750 (or so))with straps that clear
>the bore and part outline locations.
>3a. (added on re-read,forgot the thickness) mill the area of the part
>to thickness (could use a pocket routine here,so you dont hit the
>clamps holding the stock edges.
>4. Do the bores. (drill 1st will take the end load off the endmill)Or
>use all this helical stuff we been talkin' 'bout. :)
>Be sure the big bore goes into the sub base a ways.(trick is coming)
>5. tap the drill holes darrell mentioned (in the sub base) and use w/
>bolts to hold the part for the outline milling.
>6. Do the outline.

I like the "trick" of the fixture getting it's holes from the parts'
bore. 'Tho .75 is a BIG bolt to tap for me! Guess I could use .25 and
a spacer plug.

>Alan, any reasonably current MaxNC DOES have G41,G42. Practice "air
>cutting" before you rely on it, tho. Also, the blue insulation board
>sold at Home Depot works well for this type of "proofing" parts while
>learning. Dust is not TOO bad. Thanks to RON at Flashcut for this.

I'll have to look again for G41 & G42. I've been cutting a lot of "air"
(no pun intended), even chucked a pencil in the collet, trying to follow
MAXNC's actions. What is this blue stuff? I was thinking of shifting
to pine wood for the next round, lottsa sawdust... might have to take
the mill and computer to the garage again! Actually, I could mount a
vacuum hose near the mill, might get away with that. I've been on the
lookout for an old printer housing, to do some milling in.

>7. Now,part is done, except the "ears". Remove the sub-base and re-
>mount with an angle block so the "holey pear" is in the natural
>position(upright)Use a piece of stock the size of the big bore to
>locate and "pivot" the part. Run a boltand heavy washer(s) through
>the middle of this locating pin to hold the part while you machine
>the slot(end mill or slit saw) Rotate the part, re-clamp, and re-cut
>until you have that "he musta made this on the lathe" look.

Well, I DID read too fast, and almost missed the final step! Now I see
the *TRICK* I like it!

Hay, thanks everyone for all the great ideas and suggestions. I think
I've got a plan now, and after I cut some "blue boards" I'm on to the
Gold, er, BRASS.

Actually, I'd like to see more "answers" along these lines on this list,
if it doesn't clog things up too much. BCNC (before CNC) I would have
been in my "lathe mindset" and just machined it on the lathe (well, a
somewhat similar, ROUND part). But with CNC I can get the profile I
want!

Thanks again,

Alan (learn mode)