Success CNC roughing a straight cut bevel gear. Gearotic + SheetCAM TNG

[ADH]

Hey Everybody .  I'm Andrew.  And in this post I'm going to ramble on about how you can CNC cut a straight cut bevel gear on a 3 axis machine with help from Gearotic and Sheetcam TNG.
  
Step 1 : Design your Bevel Gear in Gearotic.  Its mostly about the tooth count and shaft angles at this point . Do yourself a favor and make the gear significa ntly wider than the finished gear you will be needing, as you will need the extra data further along for the machining process.  As long as the tooth count and shaft angles are correct, the gear you need will be somewhere in there, within the extra long gear you just created.
  
Step 2 : Select your gear and go to the DFX output in Gearotic and spit out a 2D drawing of your gear. Use the side on view of this drawing as a guide to manually machine a gear blank out of whatever material it is that you desire to make your gear from.  Make sure to center drill the gear blank or make your shaft bore.  Just remember you will want some way of indicatin g where your center point is for setup later in the CNC.  Also make sure you have a way of mounting this blank later on in your cnc mill. Usually the gear will need a shoulder on the backside anyway.

Step 3:  In Gearotic, right click on your gear in the project tree and click "send selected to slicing module".   Flip the gear using the perspecti ve controls so you are looking at the gear from the back side.  You do this as slicing starts from the bottom up, as would be needed for 3d printing.  But we need the informati on in reverse, as cnc milling is generally done from top down.  Next set your slice thickness .  Keep in mind that the slice thickness you use now will also need to be your cutting depth for each pass on in your machining operation .   Thinner slices will equal better resolutio n and less finish work on your gear later.  But your CAD and program files will be much larger and your machining process will also be longer with very thin slices.  My happy medium so far is .020 thickness . Go ahead and hit that slice button.  Then you go down to the slice viewer slide bar, and have a look at how many slices you will need to form your gear. Make a note of what slice number that the outside contour  starts to go back under  the outside tip of the gear teeth.  Any slice number past this will be no good as a milling tool cannot reach underneat h the tip of the tooth and if these slices were programme d for milling, the machine would in turn mill off the majority of your outer tooth profile.  Remember in step 1, when I said make your gear thicker than what you need?  This is why.  You need that thick gear design so you have a contour to follow all the way down to the root of the teeth.  The last several passes of your machining operation your cutter will be "out in space" machining the tips of imaginary teeth as the real teeth ended long ago, but the cutter will be then coming back in and cutting metal out from the root area.  Now you can select "0,0,0" option under "output slice" and click the "DFX Out" button.
 
Step 4:  Go ahead and fire up SheetCam TNG! everybody's got sheetcam, right?  Next Import your new sliced up gear drawing into Sheetcam.  Make sure to select "Center Drawing on 0,0" when importing .  This will automatic ally put the centre of your gear on x0,y0. Making everythin g way easier for setup and machining .  Also For some reason, Gearotic puts loads of empty layers in its DFX output file.  If you wanna be a rockstar, you can first use your favourite 2d CAD and delete all that extra crap before loading it into Sheetcam.  You can also delete the slices that go back underneat h the lower gear tip that I described in step 3.  Now comes the really AWFUL NASTY TERRIBLE PART. You've gotta program a separate outside contour operation in Sheetcam for each slice, starting at slice 1 and going all the way down till the last slice before your contour starts to go underneat h the outer tooth tips. ( if you didn't already delete them).  IT IS SUPER IMPORTANT that you program each operation's depth of cut to the exact thickness that you made your slices in step 3.  And that each successiv e slice's starting depth is exactly that of the previous slice's finish depth.  If you don't do it right your gear will come out dis-proportioned or you'll break some stuff.  Then go ahead and post your G-code with whatever post processor your mill unit can read.

Step 5:  Mount your gear blank in your CNC mill. I clamp a 3 jaw to the mill table and grab onto the shoulder of the gear, of course with the bevel facing up toward the spindle.  Zero everythin g up in the center of your blank, cross your fingers and hit the whatever it is you got for a go-go button.  See what happens!

AFTERTHOU GHTS:
You may want to program a large endmill to make a few laps around the largest contour of the drawing towards the bottom of the gear in an effort to make less work for the tiny cutter your going to need to fit into the root areas of the teeth.

If you don't mind running the death out of your cnc mill, you can skip the part about manually making a blank.  You can add a square or ring around your gear on each layer of your cad drawing to represent your piece of stock, then program each slice as a inside pocket operation .
    
Also, when designing my gear in Gearotic, I set shaft size to 0. That way after slicing it up, I don't have to worry about getting rid of the shaft holes in the cad drawing.
      
I grew a bunch of extra grey hairs trying figure out how to do this.  Hopefully you guys won't!

Cheers,
      
 

[ArtF]

Andrew:

  Awesome job. Its been discussed many times here how difficult it is to
make a bevel. Your the first to figure out a sliced bevel has the data required to mill
one that way. Very nice!

   Im working on a related method here as well , youll notice a cylindica l slicer in Vexx
as of last update,. The data in that file basically shows what sections to remove or cut at what
radius for any 3d object when considere d as a cylidrica lly sliced object. ( A cylidrica lly sliced
object is basically a 4th axis toopath at various depths. if you think of it.)

  I plan to cut a material using this data and wrap it onto an arbor, but used different ly
it basically is data to be used to do kinda as you did. It occured to me that when one slices a file
as a cylidrica l object, the resultant slices are actual tooltip locations of a fine tool
that would end up cutting that object. I had never seen the capabilit y to slice an object as a 4th axis slice, so I added it to see what I could make of it. Im in the build phase of a 3d printer
that wraps any material into a 3d object cutting the material using the new slice data. Having slice data in this format seems to allow for 4th axis capabilit ies I hadnt considere d before now.

  Your experienc e shows me how perhaps I could use it for 4th axis toolpaths for beveling and such, Ill have to give it more though as I go. Try using a bevel imported with "top" orientati on
into Vexx so the axis of the shaft is in the Y direction and the X,Z plane is the tooth cone, slice it
as a cylinder using Vexx's slicing tool button and look at the slices, I think youll find they are pretty much what your formattin g yours as but already tuned to a 4th axis setup. This similarit y to what you accomplis hed making your bevel is interesti ng. When view as unwrapped data, you'll
see the slices are actually a pyramid of ever longer toolpaths from the short bottom paths for a small diameter close to Z zero, to longer toolpaths as the diameter increases . (Sorry if this
is actually just confusing, I have a strong mental image of it as Im currently coding it, but
the match with what you did is amazingly close)

Thanks for the notice, I like seeing data such as this, makes the mind work.

Art

[ADH]

Thanks Art.

I'm sure others have figured this out as well, although I may be the first to post a large piece on the forum about how to do it.

I haven't got into Vexx yet as I am just starting to learn this great software package you have put together. Definitel y something I should look into.

You are certainly correct that the slices represent tooltip locations .  I was consideri ng how a small ball mill would do the job, as a ball mill would result in a much better finish. I at first thought that you could program a ball mill with slightly less offset than the maximum radius of the mill to accommoda te the bevel angle of the gear. First problem with that is that is that the bevel angle is different from the root of the teeth, than from the tips of the teeth. Second and much worse would be the distortio n that would occur on the face of the teeth. As the angle on the face of the teeth is drastical ly different than the bevel angle.

The software you have is super close to being able to do a 4 axis bevel cut for a straight cut gear.
If you could make it so that you could hold the "perspecti ve" of the gear in the slicing module, so that the root bevel angle on the far side of the gear is horizonta l and centered on one tooth valley. Then you could slice that up and have the data you need to do the faces and root of one tooth. Then its just a matter of tilting your rotary axis to the angle of the root bevel on your mill table. Build a program out of a small portion of the data from that drawing that represent s the tooth valley. Easy.  I have no idea what it would take to modify Gearotic in that manner though.   

I'm pretty sure I understan d what you are saying about the drawings forming pyramids. As in a properly formed bevel gear the teeth could just carry on and get smaller and smaller until everythin g came to a point at the theoretic al center intersect ion point of the mounting shafts.

Another point I forgot to mention in my first post is that I omitted the layers that represent ed the tips on the small end of the gear, mainly because they were unnecessa ry for my applicati on. Although they could still be used, a different machining strategy would have to be employed until the depth was reached that the drawing formed an uninterru pted contour around the outside of the gear.
     
 Attached is a pic of Sheetcam with each layer programme d with an outside contour operation at each layers correspon ding depth. Figured I'd post it so others could see what they're getting into.

[ArtF]

  Makes sense. Thanks for the details on how to do it. 

The data that Vexx puts out coud be used for machining 4th axis on near anything
with a bit of work I think.But not much loads a .cli file so its a module Ill have to add.

 Heres an example of what I mean. Notice in the slicing photo that the bevel is basically reduced to a contour(s) for each radius or Z depth in 4th axis. To understan d it better look to the unwrapped sliced bevel gear photo. In this view, the contours for each radius is displayed . The bottom lines are straight lines ,being the edge of the gear on each radius level, they are short lines due to small radius in the center, but as you move up on that view its a larger diameter, the contours on it longer as a result, basically each level on that view, from bottom up is a contour that would wrap that radius of cylinder. So if only considers only the contours at a particula r Z (radius) level, it correspon ds to the necessary cuts at a given depth.

  Probably be awhile before I do a module to use that kind of data, but I think it'd be
a usefull 4th axis stategy.

Art

[bogus105]

Guys, nice topic. Any changes ArtF regarding bevel gears cutting? I bougt my licence in Feb 2012 as i wanted to make some bevels... Now after almost 9 years i'd love to see working solution:D

Got question: i've created my bevel gear and wanted to use "Send to 3 axis" option. Then 3-axis CNC tab appeared with my gear on the grid. I've set my tool as 1mm dia endmill, set over pass, spindle parameter s and Z-Dn/pass (0.1mm).  
Then in 'Job Settings':
- what is actually 'depth'? Initially i thought it is similar Z-Dn/pass but now i'm not sure
- tabs - are they to hold material, like bridges?

Worst thing: in 'Output Options' all the icons are grey out but one - 'Engrave'. When i hit 'Engrave' message pop out 'Engraving not released'. So how to activate the options here? So far i can do nothing further.

 

[ArtF]

Hi:

  Yes, bevels cannot be machined by the 3 axis machining, and an engrave option was not developed .
The problem is that I see it as one of those problems not solvable in a useful way.  Its very hard to
get around the way bevels are actually made and the axis control required.
   Ive investiga ted code wise methods to do them as simple engraving s, just normal 3d milling for that
option basically, but your left with a bevel that needs a lot of work unless it takes days to machine with a
small ball endmill. Even then the face surface isn't likely to be great.
  The only way to do bevels at this point is to load a 3d model of one into a proper cnc software to generate
3d milling paths for it. Depending on the bevel I think it'd be a not particula rly nice experienc e making one
that way. Im thinking 3d models will be the normal way in near future given the strides they are making.

Art