Align keyway to CL of tooth...

Looking for some possible ideas here.

We are trying, once again, to save someone else's screw-up.

Customer sent us 72 helical pinion gears that were supposed to have a key cut in the bore first, and THEN have the gear cut so that the CL of one tooth was +/-.002" to the key.

Well, some genius cut the gear first and now I've been volunteered to save the day.

I've been wracking my brain for an fairly easy, repeatable set-up for this job.

As you might guess, it's the "helical" part that is causing me fits. Kind of hard to cut a helical nest with a WEDM.

Thought of scribing parallel lines to pins and calculating the offset of the 15 degree helical angle so I can scribe a third line on CL, but I don't want to do that 72 times.

In addition, someone went to town with a die grinder "deburring" both ends of the gears, which come in sets...36 left-hand and 36 right-hand.

AND the gears are not to print...but all I'm supposed to do is cut the keyway where it's supposed to be!

Any suggestions?

And yes, I already suggested sending them back with a big NO BID!

Questions -

1) How many teeth - even or odd?

2) Since it's helical, where is the tooth aligned with the keyway, at the center of it's length, at one side or the other, or somewhere else?

If it's an odd number, can you use a ball to align a tooth space 180° out from the keyway?

If it's even, can you use 2 balls in ajacent spaces and align the keyway with a pin between the 2 balls?

What about a fixture, mounted on a plate, 2 spuds, and the second one has a gear that is locked in place. You then put the gear to be machined on the first spud, it will mesh with the fixed gear.. Once you got the fixed gear right, they would all repeat.. Getting the dummy gear set right would be the worst part. You might have to use the first gear as a sacrifice to get it set right.

On jobs like this, I do not hesitate to tell the customer that it might take a lost part or 2 to get the job set up. I used to make some very complex parts, lots of operations, they had some very tight tolerances on some interlocking angles. The best way to make them was to sacrifice one part in several of the setups, to get get things set up correctly.. I had to make batches of 40, I started with 50 sets of blanks, planning to kill 5, intentionally,and hoping not to kill over 5 unintentionally...

davis is right about losing a few parts. a rescue job is a rescue job, you save all you can save but it still has to be economical, you might be able to save them all but how much is that going to cost? at some point it might be cheaper to scrap them and start over but if they can stand to lose a few then it might be cheaper to save them. find out from the customer up front. ive gone both ways on this and had pissed customers both ways, spend the time to save them all and been told by the customer that it was too high he could have had them remade for that or sacrificed like three parts and been told that he really had to have all 175 or whatever number parts and then he expected me to make up the difference, a real pita, so now i clarify this before i start. another thing all rescue jobs are time and materials only never bid. but none of this helps answere your question. i think the fixed gear method in davis post would be best.

Ok, from memory here as I'm WAY away from the shop.

Parts are 5.177" tall

3.999" +.000"/-.0005" bore

7.374" major diameter

6.003" root diameter

20 teeth (stub form)

20 degree pressure angle

15 degree helical angle

Pitch Diameter escapes me ATM.

Keyway must align with CL of tooth on the end with two tapped holes which were also supposed to be aligned with the teeth, but aren't. I cannot use the tapped holes because none of them appear to be in the right place, or in the same place from gear to gear.

Davis, I like that idea. Will have to give it a try when I get back. Thanks.

Assuming the lead is correct on the gear, you could calculate where the center of the tooth is on the end face (5.177"/2 away from that point).

Set the gear on a plate that has a short protruding "spud" that is 3.9985" in diameter. (with a concentric hole through the plate to pick up center).

Bolt a block onto that plate in a known position, and that block could have a hole for a pin with a rounded end at that height mentioned above.

Set the gear on the spud (that takes care of center), and bring in that pin to a tooth gap (that takes care of clocking).

Only have to align the fixture once in the machine, and find center once, then let 'er rip.


I think this should work...

-----

update: (had to go brush up on a couple of things)

Need to know the PD to do the above calculation.

I hope I got this right......

PD = N / DP / cos(helix angle)

Lead = PD * Pi/tan(helix angle)


Maybe that's some help if you choose to go that direction.

PM

Do they have a correct mating part you could borrow? You can make a setup fixture with the keyway on the mating part in the correct orientation, then figure out where your "theoretical" keyway will go. Make some type of locating finger that engages the gear to be cut based on that position, could just be a pin with a faux gear profile cut on the end, and program from there.

The tough part will be making a fixture to locate the gear that will still allow you to get the flush cups real close. A part that tall without good flushing is going to cut real slow!

The tough part will be making a fixture to locate the gear that will still allow you to get the flush cups real close. A part that tall without good flushing is going to cut real slow!

Click to expand...

Not that difficult, cut a keyway or grind a flat on the locating pin for the gear and press that into a hole in the fixture base. Make sure the keyway lines up with where you are going to cut the keyway in the gear if your locating pin is a bit shorter than the gear it should be simple to flush, of course I could be wrong, I have not used a WEDM in many years.

Thank you gentlemen. Will be back in the shop tomorrow. Will give all your suggestions a try.

Update time.

Every shop should have a Jack.

Jack has worked here about a year longer than I, but has several years more experience.

So often the solution to a problem is to show Jack what "they" want done and listen to him say how we can't or shouldn't do it, and wait 15-20 minutes. Then he will show us how to do it better and faster.

I was working at the layout for a fixture plate for these gears using a .5"x12"x12" 316SS plate, 1-2-3 blocks for locating, and a dowel pin for indexing.

Jack looked at it and said we ought to use two dowels aligned to the helix to index the tooth and just rotate against a 1-2-3 block for location.

I said doing that we didn't need a 1-2-3 block any more, just another dowel.

So, the fixtures in their final form are simply a 12"x12" plate of .500" 316SS with a 5.25" bore through the center, a pair of .375" dowels @ 90 degrees through the plate at a 105 degree angle on one plate and 75 degrees on the other, and a third dowel pin tangent @ 180 degrees. Plus a pair of tapped holes for clamps.

All much simpler than what I originally envisioned.

Thanks guys, you were really helpful and put me on the right track.

Sorta humorous postscript...

One of the Company's stated goals is that all jobs that need machine programs will be programmed in "Engineering" before they are even released to the shop floor.

Let me know when you stop laughing.

OK, as you can probably guess, this is the cause of more than a few headaches for me.

The bore in these gears is dimensioned 3.999" +.000"/-.0005".

The keyway width is .750" +.002"/-.000"

The overall keyway depth is 4.215" +.010"/-.000".

When I reviewed the program that "Engineering" sent me I noticed that the keyway looked a little shallow, to say the least. The 2.110" depth call-out from the bore center confirmed it.

When I politely informed said "engineer" that I thought the keyway depth "might be a little shallow" I was dumbfounded when he proceeded to give me a "lesson".

I was told that you should take half the unilateral tolerance (+.005") and add it to the overall (4.215") and divide by two to get 2.110"!

I pointed out to him that 3.999" was almost 4.00" and that if you took half of that (2.00") and subtracted it from 4.220" you should have 2.220" NOT 2.11".

I would have liked to have seen my face when he told me I was wrong!

At that point I "suggested" he pull up his CAD drawing and double-check the overall keyway depth.

An hour later he brought me a "revised" program.

Keep in mind that he is a (supposedly) experienced engineer and CAD/CAM guy.

Glad you got it all solved.

Engineers should not be allowed near a CAM program. I'm going to leave it right there for now...

JUST WANDERING, IF YOU PUT IN KEYWAY FIRST, HOW DOES GEAR SHOP LINE UP THEIR HOB IN A WAY THAT WOULD BE WITHIN .OO2 ,SO THAT C/LINE OF TOOTH OR VALLEY IS TIMED. FUTHERMORE IF THE GEAR SHOP RUNS BACKLASH THERE WILL BE A VARIANCE ALSO IN THE TIMING. I'M ALWAYS AMAZED AT THE ENGINEERS THAT COME UP WITH PROJECTS AND THEN THE MACHINE SHOP HAS TO FIGURE OUT WAYS TO MAKE THEM WORK.

Getting within +/-.002" would be a simple matter of indicating your setup in.

Backlash can be virtually eliminated by taking all your cuts in the same direction.

Both SOP.