I want to machine this part but I need ideas how to make this part the toth are really small and the material is very strong..

Depends on the quantity. For the teeth, you could get a slitting saw or T-slot cutter and have that profile ground onto it. Then set the part up vertically on an indexer and cut the grooves. Time consuming but it would work. If the quantities are higher I would look to see if you could roll or form the shape onto the parts (similar to a knurl). Anybody in your area have a gear hobber?

:cheers:

Custom made tapered end mill.
20+k spindle would be nice as well.
These guys http://www.tungstentoolworks.com/ will make them the may be close to $100 each.
You will have to contact to know for sure.

What is the material, hardness etc. Qty?
add: accuracy of index & general tolerances?

What is the material, hardness etc. Qty?
add: accuracy of index & general tolerances?

It is in fine print on the drawings; one piece 1018 or 1045, the other piece with the square hole, aluminum nickel bronze with a machinability rating of 50 compared to brass.

I think the easiest way to do these parts is give them to somebody else :) .

A specially made end mill would help, however looking at it, the "valley" of the teeth is not a regular shap but rather a tapered shape, it calls the teeth dim's out, so therefore I would think the valley has to be tapered. It wouldn't just be a simple pass of the end mill. Instead it would be at least two pass's to get the proper profile.

FWIW

I would likely use 3 passes.
1 roughing with a straight cutter and 2 finish with the taper mill.
No indexer is required. CNC is.

It looks like the two parts interface w/ each other so.. it probably doesn't matter too much in the end.. as long as both are done the same way..

I would likely use 3 passes.
1 roughing with a straight cutter and 2 finish with the taper mill.
No indexer is required. CNC is.

A 0.015" diameter end mill is very tiny. I put my money on a custom ground side and face cutter and an indexing head; complete the slot in one pass.

I may be missing something but the slot width on the bronze part is .381 mm. By my numbers that's just under .015" wide. I wouldn't use an endmill. The tool would be too small and cost prohibitive to make. Get a t-slot cutter ground with that profile and do it in one pass.

Or the best way to do it.....sub it out...:D :D

Good luck!

:cheers:

I may be missing something but the slot width on the bronze part is .381 mm. By my numbers that's just under .015" wide. I wouldn't use an endmill. The tool would be too small and cost prohibitive to make. Get a t-slot cutter ground with that profile and do it in one pass.

Or the best way to do it.....sub it out...:D :D

Good luck!

:cheers:

Plagiarist :D :D :D

I will agree that a .012" cutter is a rather small diameter.
But what's the big deal?
No problem - OK maybe need to take 3 roughing passes instead of 1.

I figure they want tapered sides so that they will get almost 0 backlash.

In a lot of cases a design like this is made by an engineer who knows very little about machining manufacturing.
Talk to them and you can likely get them to change the design to something you can cut with a standard slotter
or maybe a standard V cutter.

Plagiarist :D :D :D

Plagiarist?:boxing: Look at the second post. I recommended that way back when. I was just confirming that 1) I read the print right and 2) that great minds think alike :D :D :D

:cheers:

Plagiarist?:boxing: Look at the second post. I recommended that way back when. I was just confirming that 1) I read the print right and 2) that great minds think alike :D :D :D

:cheers:

Whoops, sorry, grovel, grovel.

:cheers: With all this beer drunkin going on who is going to drive home from work?

:cheers: With all this beer drunkin going on who is going to drive home from work?

What your truck doesn't g-code? :confused:

I guess it's time for a new truck

Thanks for the Feedback!!

I need to make 5 of each for now and It could be more later on.
I will try T-slot cutter first, andI let you know the outcome.

the cut is .015" and that will be hard to make it with a end mill because there are 180 slots.


Thanks

:cheers: With all this beer drunkin going on who is going to drive home from work?

Already there :) .

Hi chak, how many do you want to make?
If you're going to make one, then having turned the item the next job is to mill the teeth, broach the square hole and drill the holes.
There's plenty of faces and diams to grip, so holding and locating should not be a problem.
The teeth are parrallel sided with the slots tapered to the centre line.
Due to the size of the tooth it would easiest to make it with a slotting head on a milling machine, with the job held in a dividing head and plunging from the top, or if height is a problem then from the side in the X axis, and a "u" shaped single tooth form ground cutter, so forming the tooth in one pass as you go progressively deeper into the face.
This will give parrallel sided teeth with the tapered form.
If a form ground cutter is out then then a single tooth cutter ground to a "V" shape with flat end, narrower than the slot, would cut first one side on all teeth, and then the other side of the teeth in a second pass.
Having the centre higher makes it impossible to form the teeth with a pair of cutters on an arbor due to cutter diam and run out.
If you really want to get primitive and do it with the average home work shop tooling, then try racking the slots, like a shaper, with the lathe saddle and a boring bar, and the job held in the dividing head on a plate bolted to the bed at right angles to the lathe spindle.
It's a straight forward cutting and turning exercise, that is determined by the tooling available.
The hardest part would be to get a method to divide the number of slots required.
If you're going to make it a production job, investment cast it.
I would tend to agree with Darebee about the design/engineer part as this is usually how these jobs are phantisized when the digestive juices are at full slurp.
Ian.

The 3/4" square could likely be done with a rotary broach. You would have to add a chamfer on the broaching side, but 3/4" square x 3/4" deep with corner radii is usually doable, although I have no experience with this material. A heavy duty rotary broach that size with custom corners is about $150, probably too much for such a small amount of pcs. Then again, if you could do them all with the one broach you may save yourself alot of time.
I hope you know this material!
Square Broaches (http://www.slatertools.com/rotary9.htm)

Apears to me as a 3.000" by 180 tooth Hirth Coupling, Another wonderfull Metric designed in Inches and converted to metric; could be cut on a Gleason # 3 straight bevel machine, tools would be a dog with the none standard Pressure Angle, and 0.015" whole depth, getting the cutters past each other? Don't have access to a machine anymore. A 0.750" dia disc cutter would go thru on the mill, 18.4349 deg P.A. custom cutter.

Cheers Les H.