[BNX]

I want to make my own custom hub. I am having difficulty thinking about how to cut inter spline for the axle. Any ideas? I linked a video from youtube. I can’t seem to find much on it. I’m using SprutCAM 7.

Rick CNC Cutting a Internal Spline - YouTube

[SCzEngrgGroup]

Most splines are broached, not machined. The depth alone makes machining impractical.

Regards,
Ray L.

[MichaelHenry]

Ray - it looks like the video is showing a broaching tool being held in a non-rotating spindle to make the splines. Perhaps the OP is asking how SprutCAM can be used to do that?

Mike

[SCzEngrgGroup]

Ray - it looks like the video is showing a broaching tool being held in a non-rotating spindle to make the splines. Perhaps the OP is asking how SprutCAM can be used to do that?

Mike

Michael,

Sorry, you're right - I wasn't able to watch the video. That looks like a hexagonal being used as a simple single-point broach. I'd be surprised if any normal CAM could be coerced into doing that, but manual programming would be pretty simple, as it's simply plunging, then stepping radially outward from the workpiece axis a thou or two, then plunging again, until the desired diameter is reached. Then, rotate the 4th axis, and repeat. It would be quite easy to write a parametric g-code program that would allow you to enter the hole center, starting and ending diameters, step increment, depth, feedrate and number of "teeth", as parameters, and the G-code would do the rest. However, you'd also want to figure out a way to lock the spindle so it can't turn, because if it turns, the spline will be ruined. I've used this method many times to cut a simple internal keyway. The tool I used was just a 1/8" lathe tool held in a piece of steel rod, with the tool profile ground to the keyway profile. The exact same method could be used here. Make the rod as large as possible, to make it as stiff as possible. Depending on the spline profile, you might be able to use a carbide threading insert instead of a HSS lathe tool. It won't be fast, but it will work, and would cost next to nothing.

Another, much more expensive, option is to buy a rotary broach and holder, though rotary broaching is done in a lathe not a mill. But, it is MUCH faster, and probably a bit more precise as well.

Regards,
Ray L.

[waltpermenter]

Ray - it looks like the video is showing a broaching tool being held in a non-rotating spindle to make the splines. Perhaps the OP is asking how SprutCAM can be used to do that?

Mike

you are correct, perhaps the op could message the guy on youtube for some g-code. search youtube, there is one broaching video on a little x2 that shows the subroutine used, very simple to write your own.
walt

[tbaker2500]

Here's another thread on this topic:
http://www.cnczone.com/forums/g-code...broaching.html

[rlockwood]

Michael,

Sorry, you're right - I wasn't able to watch the video. That looks like a hexagonal being used as a simple single-point broach. I'd be surprised if any normal CAM could be coerced into doing that, but manual programming would be pretty simple, as it's simply plunging, then stepping radially outward from the workpiece axis a thou or two, then plunging again, until the desired diameter is reached. Then, rotate the 4th axis, and repeat. It would be quite easy to write a parametric g-code program that would allow you to enter the hole center, starting and ending diameters, step increment, depth, feedrate and number of "teeth", as parameters, and the G-code would do the rest. However, you'd also want to figure out a way to lock the spindle so it can't turn, because if it turns, the spline will be ruined. I've used this method many times to cut a simple internal keyway. The tool I used was just a 1/8" lathe tool held in a piece of steel rod, with the tool profile ground to the keyway profile. The exact same method could be used here. Make the rod as large as possible, to make it as stiff as possible. Depending on the spline profile, you might be able to use a carbide threading insert instead of a HSS lathe tool. It won't be fast, but it will work, and would cost next to nothing.

Another, much more expensive, option is to buy a rotary broach and holder, though rotary broaching is done in a lathe not a mill. But, it is MUCH faster, and probably a bit more precise as well.

Regards,
Ray L.

Just program is as a g81 drilling cycle, plot the points and make sure they're in order.. Every CAM package is capable of this, but i'll admit I hand programmed them the first few times because it wasn't my first thought.

[handlewanker]

Hi, you mean you're going to drive the Z up and down with your precision ballscrew?????
Ian.

[David Bord]

I too have been looking for ways to do internal splines. The ID is pretty small. Somewhere around .3125-.375" so the tool would need to be small. This would be in aluminum... think of a motorcycle shifter. Some sort of single point 60 degree tool? Just not sure what I could use or how to make one?

Got any ideas?

David

[handlewanker]

Hi, without any doubt, for a hole that size you would broach it in an arbour press......the broach takes out a few hundreths of a mill with each step on it's length and can produce a perfect shape, or almost so, in one pass.....the tool is only really suitable for lots of holes as it cost a lot to make the broach.

A poor man, or for just one hole, would use a boring bar with a single point tool bit and a rotary table and plunge the grooves in the bore, adjusting the depth for each pass and indexing round for the number of grooves required.

It can also be wire cut, if you have access to a CNC wire cutting service.
Ian.

[qwk racing]

I have a press broach tool 1-.125 48 spline. what do I machine my id for my broach and whats the tolerances for the id. Thanks

[handlewanker]

Hi the end of the broach has to enter the hole to start with, and the ID would be the bottom diam of the broach tooth form.

If you bore the hole too small you won't get the broach to enter the hole, and more than likely the end of the broach is the bottom diam of the splines, so you will need to make the ID a close fit, couple of thou clear so that the broach will be guided for centrality by the broach end diam.

If the broach does not have an end pilot to guide you, make the hole diam to the bottom of the broach teeth diam.....a couple of thou doesn't matter.

If you make the hole too big the broach will not centralise and the teeth will be more in one side than the other.....it'll still fit and won't make a lot of difference.
Ian.

[JohnToner]

We did an internal spline in school with a BP. First using the appropriate circle pattern from the DRO and the largest drill bit that will fit inside the grooves of the spline, drill a hole where each groove will be. Next, grind a broaching tool and broach each groove. Last, bore out the center hole. Not really hard to do.