CNC Gears and CAM

[apples000]

This year, for our rotating arm, our team needed a 17 tooth 20 DP gear, so I cut them, on a bridgeport, using an involute gear cutter we had laying around. I made 3 2 inch long gears and parted off individual gears on the lathe. This worked really well, and was way cheaper than buying gears, so our team is spending time this offseason to find a way to make cheap gears.

Making the gears was unimaginably time consuming and boring, especially on a mill without a DRO, so we wanted to do the same thing, but with a 4th axis on a CNC machine (which we have). We have no idea where to start with generating the g-code with this in MasterCAM. Has anybody found a way to do this, or are we better off writing the gcode ourselves?

Our second question deals with the actual cutting. We've found that with our CNC machine (it's a Tormach) some of the more aggressive cuts that work just fine on our bridgeport result in a lot of screeching from the whole machine just warping and being sloppy. It's not nearly as rigid as our bridgeport. I can actually do climb milling (which probably isn't a great idea) on a bridgeport faster and at a larger depth than we can on our CNC, so I'm kind of worried that the involute cutter won't work so well cutting steel gears. Could we make aluminum ones with the same cutter?

[Alan Ing]

Originally Posted by apples000

This year, for our rotating arm, our team needed a 17 tooth 20 DP gear, so I cut them, on a bridgeport, using an involute gear cutter we had laying around. I made 3 2 inch long gears and parted off individual gears on the lathe. This worked really well, and was way cheaper than buying gears, so our team is spending time this offseason to find a way to make cheap gears.

Making the gears was unimaginably time consuming and boring, especially on a mill without a DRO, so we wanted to do the same thing, but with a 4th axis on a CNC machine (which we have). We have no idea where to start with generating the g-code with this in MasterCAM. Has anybody found a way to do this, or are we better off writing the gcode ourselves?

Our second question deals with the actual cutting. We've found that with our CNC machine (it's a Tormach) some of the more aggressive cuts that work just fine on our bridgeport result in a lot of screeching from the whole machine just warping and being sloppy. It's not nearly as rigid as our bridgeport. I can actually do climb milling (which probably isn't a great idea) on a bridgeport faster and at a larger depth than we can on our CNC, so I'm kind of worried that the involute cutter won't work so well cutting steel gears. Could we make aluminum ones with the same cutter?

Cutting gears with a Tormach and a 4th axis should be fairly easy without having to go into mastercam. The Tormach comes with some preset wizards which are accessible from the control panel. I can't remember what its exactly called, but it probably is named "gear wizard". Just enter the parameters, upload the generated g-code and mount your 4th axis. Cutting aluminum gears is easier than steel using the same cutter. We actually cut gears using a diy homemade gear hobbing attachment for our Bridgeport style vertical mill. It's much faster than cutting the gear on our Tormach as we rotate the gear blank while cutting all the teeth a little at a time. Since you have the Tormach and a 4th axis, I would just use that as it should be easy to set up and run.

Alan

[Andy A.]

Originally Posted by apples000

We have no idea where to start with generating the g-code with this in MasterCAM. Has anybody found a way to do this, or are we better off writing the gcode ourselves?

Gearotic is awesome software for gear design. It can also generate g-code, but I believe will do so only for 2d or 2.5d type work. That limits it's built in CAM usefulness to fairly large gears (unless you're willing to run a very small cutter).

Running the fourth axis and gear cutting tool profile should be possible using mastercam, however a generic post file may or may not handle it well. Check to see if Tormach has any guidance on this. As for the specific steps involved in getting the right operations set up in mastercam take a look at youtube. If you happened to have bought Sprutcam along with the mill check that out too; it's actually pretty capable for 4th axis work.

Originally Posted by apples000

Our second question deals with the actual cutting. We've found that with our CNC machine (it's a Tormach) some of the more aggressive cuts that work just fine on our bridgeport result in a lot of screeching from the whole machine just warping and being sloppy.

As to the performance of the Tormach: it doesn't cut like a larger mill because it's not a larger mill. Mass helps smooth a mill out a lot (though smoothness is not necessarily an indication that the cut parameters are good!). You may need to better match your expectations for cut speed with the size of the machine. Rigidity in machine tools is a complicated thing. In my experience with a series 3 1100 machine rigidity is rarely ever a factor. Things like spindle power and tooling are almost always the limiting factors.

How are you calculating your feeds and speeds?

[sanddrag]

Alan, do you have a picture of your gear cutting setup?

[apples000]

Originally Posted by Andy A.

Gearotic is awesome software for gear design. It can also generate g-code, but I believe will do so only for 2d or 2.5d type work. That limits it's built in CAM usefulness to fairly large gears (unless you're willing to run a very small cutter).

Running the fourth axis and gear cutting tool profile should be possible using mastercam, however a generic post file may or may not handle it well. Check to see if Tormach has any guidance on this. As for the specific steps involved in getting the right operations set up in mastercam take a look at youtube. If you happened to have bought Sprutcam along with the mill check that out too; it's actually pretty capable for 4th axis work.



As to the performance of the Tormach: it doesn't cut like a larger mill because it's not a larger mill. Mass helps smooth a mill out a lot (though smoothness is not necessarily an indication that the cut parameters are good!). You may need to better match your expectations for cut speed with the size of the machine. Rigidity in machine tools is a complicated thing. In my experience with a series 3 1100 machine rigidity is rarely ever a factor. Things like spindle power and tooling are almost always the limiting factors.

How are you calculating your feeds and speeds?

We discovered last night that the poor performance we had been experiencing with the tormach only happens when we travel in the y axis. It also appears that the shaft off of the motor that drives the the y axis is not concentric with the shaft coupler that drives the ball screw. Our old limit going through aluminum with a 3 flute, 3/8 roughing bit, at a depth of .080, was about 2 ipm, which is really slow. Just making cuts in the x axis tonight, we were able to up the speed to about 8 before it started pulling the bit straight out of the (very cheap) tool holder. Once we get the y axis issue fixed, we should be all set to cut gears.

I've checked around in MasterCAM, and I haven't found a way to do what I want. We do have MasterCAM x3, which is really old.

[Andy A.]

Originally Posted by apples000

We discovered last night that the poor performance we had been experiencing with the tormach only happens when we travel in the y axis. It also appears that the shaft off of the motor that drives the the y axis is not concentric with the shaft coupler that drives the ball screw. Our old limit going through aluminum with a 3 flute, 3/8 roughing bit, at a depth of .080, was about 2 ipm, which is really slow.

The Y and X axis motion control and screw design are essentially identical except for length. You should see the same performance in both, so obviously, this isn't up to spec. The shaft coupler can tolerate some misalignment but there shouldn't be much. Was the Y axis motor removed during installation (I had to pull mine off to fit through a tight door)? If so, I vaguely recall there being some wiggle room in the motor mount screws that might account for the misalignment.

There are a litany of other things that could cause poor performance in one axis- bearing preload and gib adjustments being the two big items. The manual covers checking and adjusting those. A call to Tormach would probably be a good idea.

Originally Posted by apples000

Just making cuts in the x axis tonight, we were able to up the speed to about 8 before it started pulling the bit straight out of the (very cheap) tool holder. Once we get the y axis issue fixed, we should be all set to cut gears.

What were the parameters of your cut? Using the 3 flute 3/8ths cutter you mentioned before, and making some broad assumptions, the limiting factor in your cut should be spindle speed. A full WOC roughing pass at .080 DOC could run at 5100 RPM, and better than 70ipm and you'd only be loaded to about .5hp. Gwizard suggests a deeper depth of cut but, depending on your priorities and tool, ~40 ipm is in the ballpark.

What kind of tool holder are you using? I've had very positive results using TTS style holders of all types. If you're using a set screw holder you must make sure that your tool has a flat on the shank for the screw to set on. Not all tools do and a setscrew will not adequately hold a round shank. For those you must use a collet; either in the R8 spindle or in a ER collet TTS holder.

[apples000]

Originally Posted by Andy A.

The Y and X axis motion control and screw design are essentially identical except for length. You should see the same performance in both, so obviously, this isn't up to spec. The shaft coupler can tolerate some misalignment but there shouldn't be much. Was the Y axis motor removed during installation (I had to pull mine off to fit through a tight door)? If so, I vaguely recall there being some wiggle room in the motor mount screws that might account for the misalignment.

There are a litany of other things that could cause poor performance in one axis- bearing preload and gib adjustments being the two big items. The manual covers checking and adjusting those. A call to Tormach would probably be a good idea.



What were the parameters of your cut? Using the 3 flute 3/8ths cutter you mentioned before, and making some broad assumptions, the limiting factor in your cut should be spindle speed. A full WOC roughing pass at .080 DOC could run at 5100 RPM, and better than 70ipm and you'd only be loaded to about .5hp. Gwizard suggests a deeper depth of cut but, depending on your priorities and tool, ~40 ipm is in the ballpark.

What kind of tool holder are you using? I've had very positive results using TTS style holders of all types. If you're using a set screw holder you must make sure that your tool has a flat on the shank for the screw to set on. Not all tools do and a setscrew will not adequately hold a round shank. For those you must use a collet; either in the R8 spindle or in a ER collet TTS holder.

I wasn't actually there when the cut happened, but I'm assuming they did what you said, and used a set screw where there wasn't a flat. We'll be getting in touch with Tormach soon to try to fix the issue with the y axis.