Gear cutting with cnc 4th axis

[ownthesky2010]

Hi All
I am posting this in case its of use to anyone.
I have an emco pcmill 50 and a homemade 4th axis and this is how i ended up machining cam gears for a model engine.
I have already tried all sorts of methods using homemade tools after a ton of research but I found that they work well on non ferrous materials but not on steel.
A hob would have been first choice but they require the spindle to be synced to the rotary axis and my machine cant do that. Besides, they dont come cheap.
Limited to single point tools ruled out any hss or tool steel cutters as they wore out too fast.
In the end I settled on mounting a carbide vbmt turning insert on its side, off centre in a homemade holder. The inserts are easy to get and have a 35 degree point which is fine for gears. I found the smallest corner radius of 0.4mm to be to big for small gears so I grind 2mm off the last 5mm of the face and the radius is reduced to about 0.2mm
This also means I can recycle used inserts.
Initially I used the tool to take 5 passes along each tooth while moving the z axis and rotating a tiny bit after each cut.
This all needed to be carfully calculated to simulate the gear tooth profile and did sort of work but I never quite got a good profile.
I came up with the current method to simulate the rolling cutting action of a hob but with a single point tool by synchronizing the z axis and the rotary axis. .
It works very well and the gears mesh perfectly and needs much less calculation.
The tools last a long time and its reasonably quick.
Also, I can cut any size or number of teeth with one tool, as long as they all use the same contact angle.
I have attached a video to help explain.

[ame]https://www.youtube.com/watch?v=zPCEf7UqQC4[/ame]

 

[DICKEYBIRD]

That's awesome! Did you use a CAM program or hand write the code.

Great job!

 

[ownthesky2010]

Thanks Mate.
I just programmed it long hand. The program is pretty simple. Just 3 steps in and then 6 across. With each step You rotate by 5 teeth and move in z by 5 teeth, changing direction after each pass. I do it all incrementally in g91 and the you only need to program 1 tooth and copy/paste for all the others

 

[canadianhorsepower]

Thanks Mate.
I just programmed it long hand. The program is pretty simple. Just 3 steps in and then 6 across. With each step You rotate by 5 teeth and move in z by 5 teeth, changing direction after each pass. I do it all incrementally in g91 and the you only need to program 1 tooth and copy/paste for all the others

Nice work I have the same mill and love it
cheers

Luc

 

[GLCarlson]

Picture of the tool NOT rotating? And it'd be nice to see the code....

 

[dr_kingston]

Is there any movement along the A axis or just plunge cutting to get the right tooth profile.
Regards Dale

 

[ownthesky2010]

Hi Luc
Its a great mill. I am often surprised by how capable it is.
Are you using Mach3 on yours.
I have a cheap stepper kit from logsmotor in china and its not very fast but its powerful and very accurate.
GLCarlson, I will attach a pic of the tool and the program.
The program is for a 26 tooth 0.6 mod gear.
The insert pocket in the tool is a simple parallel sided pocket, not tapered like it should be, and is intentionally off centre so that only one edge touches the workpiece.
Dr Kingston, the tool takes 3 plunging cuts into the material to get to the correct depth and then steps along the tooth in the x axis in 0.5mm steps.
The shape of the tooth profile comes from the fact that its rolling in and out of cut.
I have combined the motion in all 3 axes at the same time to keep it simple and short.
In theory the steps should leave a scollop in the face but in practice its so small you cant even see it.

View attachment GEAR LATEST.doc

 

[jimjam66]

Excuse my ignorance (I've never cut a gear tooth) but why is the A axis rotating through the cut? I would have thought that this would make the gear profile slightly helical? Or was that your intention?

 

[kvom]

If I understand this, then he drew the tooth form as several straight segments to approximate it. Then after cutting the center to depth, he rotates the great and adjusts Z so that the straight edge of the cutter cuts each segment in turn. The part doesn't rotate during the cut.

 

[ownthesky2010]

Sorry gents, I am not explaining myself very well.
My first attempts at gear machining were as described by kvom, a series of cuts along the tooth that created facets that to approximate the proper tooth form. The more cuts you take, the closer to the correct form you get. The result was usable but not great and if the tool height was not set perfectly the form of the tooth was all wrong. This is especially difficult with small teeth.
When gears are machined with a proper helical hob the cutter has a rack tooth form. The material is rotated at the same pitch as the helix of the hob so that it cuts the correct number of teeth for the diameter of the material.
The rack shape of the hob creates the rounded shape of the gear teeth as each cutting edge rolls in and out of the material while the material is rotated at the same time.
This smooth rounded gear tooth meshes well with other gears made with the same hob.
My method uses the same principal as the hob method by feeding the cutter through the material in the vertical (z) axis while rotating the material in the rotary (a) axis in the same direction and at the same pitch.
The first 3 cuts in my program move closer into the material (y axis) to get to the correct depth of cut.
The next 8 cuts move along the tooth (x axis) to machine the tooth the the correct depth along the whole thickness on the gear.
The important thing is that every cut you take you must rotate the material while you move in z at the same time.

 

[jimjam66]

Thanks for that explanation. I did think of the helical hob scenario, so not terribly surprised. I had expected it to be easier to emulate the spherical hob approach, where the gear blank is stationary during the cut. But I get that you are using a cutter which doesn't itself create the 'tooth' shape, so you are reliant on a number of passes to get the final shape.

Kvom, if you watch the video you will see that the A axis does indeed rotate during the cut.

 

[mu38&Bg#]

That's great! I have had the same idea rolling around in the back of my head but haven't sat down to write the code the way I want to (macro). My thoughts were to use something like a thread mill but with a 40° form. The problem is they all have very sharp tips and wouldn't last long. I quoted a custom tool, but it's costly. As a side note, last night I cut my first part in the PC Mill 125 I brought home last month.

Greg