How would you turn this profile in small quantities ?

I need to make pushrods with this end geometry. Material is mild steel, probably 1018 or similar. I'll be making 10 or so at a time, so will be turning 20 ends, controlling the length to ±.010. Not enough quantity for cnc, but I'm finding it a PITA on an engine lathe with off the shelf tools. I no longer have a radius/ball turner.

I'm picturing a bespoke radius tool, maybe a brazed carbide tool.

If you would use a form tool, how would you make it, and how would you cut the part to get a good surface finish?
I don't have wire EDM, not that great at hand grinding female radius.
If not a form tool, how would you do it?
I'm just out of other ideas here for this simple little job, haven't had to do this before
.

If this was my job I would have a form tool wire (edm) cut. You don't say what sort of finish you need but a wire cut form tool will put a very high finish on the part.

Ruling out the ball turner attachment (looks like you got rid of it too soon ) and cnc, brazed carbide form tool. If it is somewhat critical (form wise), have a few wireburned. If you just need somewhat close you could use a green wheel and a radius gage...?

SIP6A said:

If this was my job I would have a form tool wire (edm) cut. You don't say what sort of finish you need but a wire cut form tool will put a very high finish on the part.

Click to expand...

Make it a skiving form tool, to keep the potential of chattering down.

what does that look like? you stretch the radius axially like in a spring?

You could probably use something free-machining, which would help. Pushrods aren't going to care.

I would do them in a CNC with a collet nose with a stop in the collet. Not sure what you mean by not enough. I do one off work on CNCs all the time.

I'd turn the 15 deg on the tips first, then use a radius tool with the compound set at 15 (or 75) and feed in with the compound.

I've also used corner rounding endmills in a boring bar holder. Hokey, I know.

For Qt. 10-20

5C collet chuck with stop. HSS form-tool hand-ground to the profile. If you're having trouble free-handing the radius then maybe a .125 radius grinding stone in a dremel to hit the correct profile on the form tool (think chainsaw sharpening bit).
Micrometer hard-top on the ways to dial in the length.

And if you're getting surface finish problems because of the length of the form...

you could always keep the left hand side of the radius open on the form tool. Cut just the radius first on all the parts, then do the 15 degree blend as a 2nd op with the compound.

Hardplates said:

I would do them in a CNC with a collet nose with a stop in the collet. Not sure what you mean by not enough. I do one off work on CNCs all the time.

Click to expand...

Don't want to stop a machine, take the chuck off, put collet chuck on, rig up a collet stop for a 15" long part, etc. then put it all back when I'm done and others are waiting for the machine.

Booze Daily said:

I'd turn the 15 deg on the tips first, then use a radius tool with the compound set at 15 (or 75) and feed in with the compound.

I've also used corner rounding endmills in a boring bar holder. Hokey, I know.

Click to expand...

I'm doing exactly that now on the sample parts, looking for faster and simpler, hoping to learn something here. I'm using a SuperBee carbide insert radius endmill and I'm chipping the insert because the cutting edge is going past the centerline of the stock when set at the 15° angle, and because of the rake of the tool.. Next step would be tailoring the insert slightly, but hoping for a one shot method. I'll need to make some custom one piece length pushrods from time to time, would be great to have a form tool set up in a QCTP holder to grab and go.

Mud said:

...I'll need to make some custom one piece length pushrods from time to time, would be great to have a form tool set up in a QCTP holder to grab and go.

Click to expand...

You should contact Severance tool. They can make a rod-end forming cutter to do it in one shot.

Severance Tool - Countersinks, Chamfering Mills, Deburring Cutters, Forming Tools

Hi Mud:
I've got the toys to do this a whole bunch of different ways.

I could:
1) spin them on the Deckel SO cutter grinder
2) Form dress a wheel on the surface grinder and spin grind them with the Harig spin fixture
3) Stand them up in the CNC mill and 3D surface them
4) Wire cut or form grind a form tool and turn them manually
5) Spin and burn them with the wire EDM and the rotary fixture
6) mill electrodes and burn them on the sinker EDM
7) program and turn them on the CNC lathe.

You know which one I'd pick?
I'd program and turn them and I'd have them done faster and better than any of the other methods, even if I had to turn them all to length on the manual lathe first and then touch off for each part individually if I was too lazy to set up a stop.

Sometimes you can over think a project and spend more time farting about making stuff than just accepting it's not going to be perfectly efficient and doing it the obvious way.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Edit: Whoops, others posted while I was typing.
You don't just happen to have a single lip cutter grinder do you?
The Deckel would do them pretty quick and so would the surface grinder and spin fixture but I'd pick the Deckel first so I don't have to dress a wheel..

If I HAD to to these on an engine lathe, depending on the customer, I'd compound the angle and file the radius on.

But just toss em in the cnc and be done with it. You'll have 20 ends done in an hour, tops.

guest said:

You should contact Severance tool. They can make a rod-end forming cutter to do it in one shot.

Severance Tool - Countersinks, Chamfering Mills, Deburring Cutters, Forming Tools

Click to expand...

That might be it. I have some of their tube end tools, didn't know they did customs.

Hi again Mud:
Another way, if you really have to do them on the manual lathe is to set the compound over at 15 degrees and then make up a table of offsets to move the tool in X and Z in small increments.
If your turning insert has a nice big radius and you have a DRO on your machine you can do them pretty quick this way too and they'll be nice enough that you can clean them up with a bit of emery cloth on a stick.

Another way I've done before is to use a boring head as a radius turning tool.
Make a quick and dirty pinch block for a toolholder and knock up a quick and dirty boring bar with an offset end if you don't have a straight shank boring head.
Clamp on a long handle and go at it.
Lube the shank and snug up the pinch block until it just runs snug and smooth.
It's hokey and more fucking around than I'd accept, but it does work and it's amazingly accurate for such a hacker setup.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Booze Daily said:

I'd turn the 15 deg on the tips first, then use a radius tool with the compound set at 15 (or 75) and feed in with the compound.

I've also used corner rounding endmills in a boring bar holder. Hokey, I know.

Click to expand...

Not hokey atall. Why grind tediously what can be had ready-made easily?

Milling cutter for a horizontal will give yah a lot more edges .annnnd.. still do its own job if but one or few of many end-up a tad worn.

The ball end is a 1/8" radius and that is a 1/4" diameter. You can get abrasive points in various radii all over the place. So, get some HSS tool bits (5/16", 3/8", or whatever you can use on your lathe)(you did say 1018 steel) and a couple of 1/4" diameter or slightly larger abrasive points. Dress the points to 1/4" +/- whatever your tolerance is and use the first one to do the radius section of the form tool to within a few thousandths of the final form. Your print does not give a tolerance. Grind at a small angle to provide some relief. Then switch to the second burr which has the better tolerance on the radius and finish with that. Then grind the 15° section tangent to the radius. Again, at a small angle to provide clearance. If you make both of these clearance angles the same amount and in the same direction (parallel to the length of the tool blank) then you will be able to sharpen it by just grinding the top down. As for the top, I would leave it at 0° rake. If the tool bit is as large as possible, that should work. And with an overall part diameter of only 0.312", you do not want to get into any geometric distortion.

Make two or three of these tool bits so you don't have to stop to sharpen them while working. A dead sharp tool is a good idea here. I would even polish the top, rake surface after sharpening them.

This work can be done in a T&C grinder or, dare I mention it here, one of the small, multipurpose machines like a Unimat, Sherline, etc. Something with a fast spindle and the ability to orient that spindle at various angles.

As for the good surface finish, you will need a heavy, tight lathe to do the turning. Use an oil based coolant and plenty of it. And finish them with a form fitting lap.

Mud said:

I need to make pushrods with this end geometry. Material is mild steel, probably 1018 or similar. I'll be making 10 or so at a time, so will be turning 20 ends, controlling the length to ±.010. Not enough quantity for cnc, but I'm finding it a PITA on an engine lathe with off the shelf tools. I no longer have a radius/ball turner.

I'm picturing a bespoke radius tool, maybe a brazed carbide tool.

If you would use a form tool, how would you make it, and how would you cut the part to get a good surface finish?
I don't have wire EDM, not that great at hand grinding female radius.
If not a form tool, how would you do it?
I'm just out of other ideas here for this simple little job, haven't had to do this before
.View attachment 280961

Click to expand...

Okay I'll say it, ;-
Turn the taper and do the rad with a smooth single cut millsaw file.

A skilled man and a bit of practice, .........….and I'd wager 99% wouldn't know the difference.

But back to reality

Turn the taper and use a .125 R router rounding over cutter.

I'd hand grind a hss form tool and include the 15 degree angle. You don't have enough surface speed or enough parts to need carbide. A shadowgraph, or even an eye loupe can get the tool close enough no one can tell the difference.