How to setup CNC for making dog gears

[Matt Reiland]

Originally Posted by sanddrag

I was just wondering how to make Technokat style dog gears in a CNC mill. I know all about the programming and tooling and stuff, but I'm wondering how to go about setting up the gear in the machine. Do you just clamp it in the vice with lead or aluminum jaws? How do you make sure the teeth don't get deformed; just don't clamp it too tight - but how tight is tight enough? Or do you machine a radius the same as the gear partially into the jaws of the vise to hold it? Would you make some sort of fixture to hold it? Also, once it is held in the machine, how do you go about centering the part because in the program I assume everything would be referenced from the center since it is round. I have only centered rectangular parts with an edgefinder before so I'm not sure how you would do this. Thanks.

I would do it in one of two ways:

1. The easy method would be to make a shaft that fits perfectly in the bore of your gear, then slide this into the chuck on your mill to indicate the center of the gear relative to the spindle. Set your NC machine to 0,0 once you can drop the shaft into the bore of the gear. This should be accurate enough for making the pockets for a dog.

2. Using a dial indicator in the chuck of the mill you can indicate the center of the gear by rotating the indicator around the bore to find the center with relation to the spindle. This is more accurate but also more time consuming to do versus a shaft.

As for mounting the piece, I would probably not use a vice but instead hold the piece flat to a table with screw down clamps out on the edges, this would put very little stress on the teeth since you are clamping through the meat of the gear. You should be able to get far enough out that you can mill all you want.

Matt

[JVN]

Originally Posted by Matt Reiland

As for mounting the piece, I would probably not use a vice but instead hold the piece flat to a table with screw down clamps out on the edges, this would put very little stress on the teeth since you are clamping through the meat of the gear. You should be able to get far enough out that you can mill all you want.

This is how we do it, and it has worked fine for us in the past.

Combined with a way to place consecutive gears on the same center (such as the method Matt mentioned above) it greatly decreases the setup time necessary.

JV

[Veselin Kolev]

[quote=Travis Covington]
Centering the hole is done the same way as you would with any piece, but instead of an edge finder on an edge, you use the edge finder in the hole for both the x and y axis'. Or you can use a dial indicator and get the same result.
QUOTE]

Well, if you use the bore cutting function on a CNC, and using the same method that Travis described, all you input is an origin (0,0) centered between the aluminum jaws and have the radius be the outer radius of the gear, and let it cut away. After that, you just put the gear into the nice hole, clamp down, and if your CNC saved the (0,0) for the cut, you can use that for the center of the gear, since they are supposed to be the same. Thats how we did it, and we didn't get wobbley gears

Oh one more thing, you can use parallels for shims to put between the jaws; they work nicely because they come in lots of widths.

As for the cut in the gear itself, use some CAD softwear to get a list of coordinates that will cut the shape in the gear. CNC mills (at least ours) are easiest to work with when you're doing straight cuts from point to point. All I do sometimes is give my machinist a hunk of steel, tell him how wide, and give him a list of coordinates in order. Of course thats bad since he doesnt know what it should look like until the end, but thats why I usually give drawings too.

Hope that helps