feasibility of sink edm tapping a hole in a motor shaft

TomSmith · Feb 16, 2017

Apologies if this is a stupid question, but I haven't done any EDM work before.

I have a series of brush DC motors with fully hardened shafts, and I need an blind axial threaded hole adding to the output shaft. I was wondering if someone could advise me whether it is practical to sink EDM a M2.5 thread into a 12mm hardened shaft in a assembled motor?

I appreciate this work would be better done on the shafts prior to building the motors, however I am against the clock, and the motor manufacturer is adding 9 weeks to the lead for that option. The particular motor design cannot be easily dismantled / reassembled.

Milland · Feb 16, 2017

Do you have access to a vertical machining center? If so, look at carbide drilling, then threadmill the tapped hole. It'll help to know the actual hardness of the shafts, but if it's below RC50 - 55 or so I don't think it'll be a problem.

gking86 · Feb 16, 2017

TomSmith said:
Apologies if this is a stupid question, but I haven't done any EDM work before.

I have a series of brush DC motors with fully hardened shafts, and I need an blind axial threaded hole adding to the output shaft. I was wondering if someone could advise me whether it is practical to sink EDM a M2.5 thread into a 12mm hardened shaft in a assembled motor?

I appreciate this work would be better done on the shafts prior to building the motors, however I am against the clock, and the motor manufacturer is adding 9 weeks to the lead for that option. The particular motor design cannot be easily dismantled / reassembled.

Entirely possible, you'd have to dam up around the shaft with putty and submerge the shaft in dielectric assuming you don't want the motors submerged. Practical though? What's the size of your run?

Red James · Feb 16, 2017

EDM threads is best done with a cnc edm. Non orbit capable machines use threaded guides, were very slow, and in general a great pita.

Somehow you have to keep the dielectric oil out of your assembly (and no, you MUST use oil to edm). Not an easy task. Best to try machining as Milland ^^ suggested.

gking86 · Feb 16, 2017

Red James said:
EDM threads is best done with a cnc edm. Non orbit capable machines use threaded guides, were very slow, and in general a great pita.

Somehow you have to keep the dielectric oil out of your assembly (and no, you MUST use oil to edm). Not an easy task. Best to try machining as Milland ^^ suggested.

Somehow I always forget non-CNC sinkers exist.

toolnuts · Feb 16, 2017

This would be an easy job for a CNC sinker, but for one thing - alignment.

If you keep the motors assembled it might be difficult finding a way to hold and properly
align the motor/shaft. Many motors don't have a surface that would lend itself to vertical
alignment.

If it has a good mounting flange then you could build a fixture to hold it
properly. The CNC can center itself to the shaft and your off to the races.

Good luck,

Paul Hoffman

Modelman · Feb 16, 2017

gking86 said:
Entirely possible, you'd have to dam up around the shaft with putty and submerge the shaft in dielectric assuming you don't want the motors submerged. Practical though? What's the size of your run?

He didn't say how big these motors are... if less than the weight rating of the machine, the easiest way to keep oil out of the motor is to fixture the motor to the ram, with the electrode in the tank.

Dennis

implmex · Feb 16, 2017

Hi All:
A point worth mentioning that no one's touched on yet; you run the risk of trashing the motor bearings if you run EDM current through them.
If this was my job, I'd do as Milland recommends and thread mill them.
Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
www.vancouverwireedm.com

Davis In SC · Feb 16, 2017

Any chance that the shaft could have been induction hardened, so the core of the shaft is soft enough to drill and tap?

Milland · Feb 16, 2017

Mr. Smith seems to have gone AWOL, we may never know what he needed to solve his problem. The unrequited machining questions just continue to stack up...

TomSmith · Feb 16, 2017

Hi everyone, thanks for the replies, and apologies for the delay in responding.

I have previously sent a sample of the motor to our machinist to see if they could drill the shaft, and they reported that it was hard throughout, rather then having a hard outer layer, and they were having difficulty machining it. That said I don't have the exact material spec / hardness, so i have contacted the supplier for that information. It is possible that machining could still work, and if the material is soft enough i will go down this route, as it does seem simpler.

The motor manufacturer rep suggested sink EDM as an option to modify the shafts prior to motor construction, however their lead time is near 4.5 months end to end for doing this (apparently the shafts are made by a subcontractor so quite a lot of delay involved).

The motor bodies are 40mm diameter, and 80mm in length, and weigh about 450g. I was planning to modify a batch of 6-12 to do some prototyping whilst i run down the manufacturer lead time.

Modelman: I too was concerned about contamination of the motor internals, so interesting to know about the ram attached approach.

implmex: Its good to know about the risks to the bearings, i would not have thought of that. Being new to EDM processes, am i right in thinking that with sufficient shaft length before the bearing i can make good electrical connection to the shaft directly? I have about 40mm to play with on the front shaft.

Thanks again for the helpful advice.

Milland · Feb 16, 2017

Tom, that's a relatively small motor for a 12mm shaft, is it quite powerful for its size? What sort of purpose does it have?

On the attempts of drilling the shaft, do you know how the motor was held, and what drill material (HSS, cobalt, carbide) was used? If regular HSS bits were tried it's not too surprising they failed, but I'd be shocked if carbide didn't work.

For fixturing (and again, presuming use of a VMC), I'd take a 12mm thick plate, split it at one end, tap two M6 holes along the split part to create a clamp, overhang a vise by ~25mm, then drill/ream a 12mm hole along the split. If needed shave 0.1mm off the mating face to ensure clamping. Now you've got a pretty rigid fixture that will repeatedly locate the motor shaft, just indicate for concentricity to be sure.

A little masking with paper and tape will help prevent chips from getting into the motor housing, for what you're doing machining dry should be OK with just an air blast.

If you do have to use EDM I'll defer to the guys who know much more than I.

strokersix · Mar 8, 2017

Bore a round hole 6-8mm diameter in the shaft then anaerobic (loctite) in a sleeve with threaded ID. Depending on structural requirements of the joint this might be adequate.

SBAER · Mar 8, 2017

strokersix said:
Bore a round hole 6-8mm diameter in the shaft then anaerobic (loctite) in a sleeve with threaded ID. Depending on structural requirements of the joint this might be adequate.

I think this is the way to go

andypugh · Mar 8, 2017

M2.5 is pretty small, what does that thread do? Maybe there is another way to do the job, with a Trantorque bush or similar.
Is there a rear shaft extension> If there is then I could imagine gripping the rear shaft and lowering the motor onto the EDM tool.
I have read that electrochemical milling has no tool wear, that might work better for threaded holes. (No experience, I just read an article once)

dougspair · Mar 9, 2017

..There a several very skilled machinists on Youtube, doing exactly this.....use a 6-8mm sleeve threaded and green locktite stud and bearing retainer....a 2.5 mm threaded hole couldn't have that much load on it....

toolsteel · Mar 9, 2017

Drilling the hole should be no issue with the correct tool. I would use a YG Dream Drill. They have a decent selection in that size range. I would go to the high end of the hole tolerance (maybe slightly over). Drill as deep as allowable. Then use a carbide tap with plenty of Moly Dee......I have done this many times with 4 mm to 8mm size taps in A8 and D2 at 58-62 Rc.....never tried a 2.5mm. It shocked the shit out of me when it worked with the 3mm tap. You wont do this by hand though....has to be in a mill...under power. I did 25 M6 holes this way modifying an existing fixture. One carbide tap.......threw it out when done, I didnt want to accidently use it next time. I figured no way that tap could keep going..lol

I would also consider the thread milling option mentioned earlier but I have no experience thread milling that small....have never actually even looked to see if such a thread mill is available.

Peter from Holland · Mar 9, 2017

Find another way to do what you want to do
There must be a easier way
But as long as we do not know what it is you want to do we can`t help you with a solution

Peter

vancecam · Mar 15, 2017

I like the insert approach, but I'm not sure I'd trust green Loctite with that direction of force. But you could 'easily' make the insert longer than needed for the screw, then carbide drill a hole, say 3/32" diameter, thru the shaft radially, and secure the insert with a 3/32" spring pin.

feasibility of sink edm tapping a hole in a motor shaft

Plastic

Diamond

Plastic

Stainless

Plastic

Cast Iron

Titanium

Diamond

Diamond

Diamond

Plastic

Diamond

Hot Rolled

Hot Rolled

Plastic

Plastic

Titanium

Diamond

Plastic

Similar threads