how to machine this part

[star1280]

I would like to know the best approach to machining this link out of steel and what tool to use. My concern is clamping it and more importantly creating a round surface for the bosses with no divets or flats since these are mating surfaces.

The competing machinist uses a deceleration code (M1 99)???

I have a BP S2 with a fagor control. I also have bobCAD.

The two bosses are 3mm in diameter.

Any tips would much be appreciated.

Alicia

[Delw]

If roundness is critical you need a tight mill to do the boss's, personally I would do the boss's in a lathe( due to them being small 3mm) on with a boring head on a mill then the rest in the mill and blending the center section of the boss's were it meets the flat stock.
will a tight mill you could run it in 2 operations with out a lathe operation and a fixture and face plate.

I have in the past used a boring head with the tool turned the opposite way so you could cut the boss ( basically turning on a lathe) it would be less of a hassle than putting it on a lathe. still 2 operations on a mill. you would need to oriant the mill so it doesn't come back up the boss and put lines in it. don't forget you would have to go in reverse if you use a standard boring head and tool due to the tool being the opposite direction

with out a print and specs its a crap shoot as to what you really need to do

[star1280]

sorry I'm waiting on drawings but the total length is only 21.97mm and width is 3mm also.

[The Inventor]

You don't say how many you have to make???

You might think about putting it into a vise mounted on an
"A" axis -- mill the flat and just rotate the 'part' for the ends.

It would require a stop block to center the part to the 'A' axis
and turn the part around and over, to get all 3 bosses,
but if you only have a few to make it would work.

[lerman]

For volume production:

Use a (I forget the actual name) end mill with a hole down the center. They are used in a lathe or in a mill to make a long thin post of the diameter of the hole. They cut only in the plunge direction. That should produce clean posts of the proper diameter on a mill. You might have to get a custom tool made.

Clamp the 3mm stock, cut the two posts on one side. Then change tools and mill that side. Flip the stock over and do the opposite side.

Ken

[LeeWay]

It might be a whole bunch faster to simply use 3 mm rods and flat bar. You would need to spot weld them and clean it up, but you can do a pair of long rods and lots of flat bars all in one part like a ladder. Then cut them into the correct length in sections. With the right jig, you could turn out bunches of them pretty quickly.
Very little waste this way and it would be nearly as strong as if you milled it out of one piece.

[mark c]

What Lerman is talking about is called a "hollow mill". They are probably kinda "spendy", so unless you're making a lot it will cost to much, although the ones I have used were adjustable through a somewhat (as I remember) large range

HTH

[HIRAH]

I would also go the 2 op route. but i would finish the outside of the long boss on the first op. i would also program the 2nd op boss radius a little bigger than the first side. you'll have less chance of a mismatch this way.

[joecnc1234]

I would machine the side with the two bosses out of flat stock then flip it over against a stop and finish the thickness and profile the boss. If you have blend issues move x or deburr to blend, If it's really tight tolerances than make a fixture for the second side.
Joe

[star1280]

Turns out I had backlash in my lead screws so Fagor techs came in to tune my drives. So the corrected the offset "half moon" effect I'm getting. If you can imagine, putting two identical half moons together you should get a perfect circle, well my machine gives me a slight offset of the two together.

By the way my quantity is one for the prototype but if all goes right there will be more.

Thanks for introducing me to the hollow mill idea. I contacted www.geneseemfg.com/products/hollowmill/ thanks Lerman and mark c! Seems like that would be a nice clean cut.

I was avoiding BobCAD because in the past it would leave step marks because of the limited path selection. Anyway around this?

Thanks all.
Alicia

[star1280]

Well guess they did their best today at tuning the controls and I'm still getting error so they think its the ball screws...

stay tuned...

[HIRAH]

personnally, i wouldn't use a hollow mill or any boring head on this part. you have more to worry about with a mismatch between the sections of the bosses. i would finish it with 1 tool. that way, when the diameter is set, at least the first side should always come out perfect. plus you can adjust your diameter for the half of the boss on the second side to eliminate a step.