Problem with depth of cut in 4D

[Stephen Fornelius]

I'm making an 84 tooth sprocket and using a fly cutter.  The gear is generated properly, but the depth of cut will not go past 0.15" no matter what I set the total depth.  I'm using a #25 chain and because of the size of the sprocket, I can't cut it horizontally so I have to use a Sherline rotary table offset from my TAIG bed.  So far that seems to be rigid enough, but this depth of cut issue is a game stopper.

(Gearotic Thoughts Version 1.12 )
(Object Name:  Sprocket-#25 )
(4th axis gear generation: Blank Radius: 3.43  Thickness of Blank:0.25 )
(Max Depth of cut for this file: 0.00 )
(Depth Per Pass: 0.05 )
(Spindle Speed: 5000  Feedrate: 10.00 )
(Tool Diameter: 0.2000 )
(Tangental shaving with involute shaped saw-flycutter.)

G20 S5000
          (Prolog Begins)

(  No Epilog set )

          (Program Begins)

G0        X -0.0250  Y 0.5000 Z 0.0000  A0.0000
          X -0.0250  Y -0.0500 Z 0.0000  A0.0000
G1 F10.0X 0.0250  Y -0.0500 Z 0.0000 A 0.0000
G0        X 0.0250  Y -0.1000 Z 0.0000  A0.0000
G1 F10.0X -0.0250  Y -0.1000 Z 0.0000 A 0.0000
G0        X -0.0250  Y -0.1500 Z 0.0000  A0.0000  Here's where I have the problem.  It will cut .05, .1, .15 and then it moves on to the next gear
G1 F10.0X 0.0250  Y -0.1500 Z 0.0000 A 0.0000
G0        X 0.0250  Y -0.1504 Z 0.0000  A0.0000
G1 F10.0X -0.0250  Y -0.1504 Z 0.0000 A 0.0000
G0        X -0.0250  Y 0.5000 Z 0.0000  A0.0000
          X -0.0250  Y 0.5000 Z 0.0000  A4.2857
          X -0.0250  Y -0.0500 Z 0.0000  A4.2857

[ArtF]

Hi Steven:

I cant repeat this one, but my version is a bit newer than yours. Please try it with a fresh download, the depth should be 3.05
or so with that sprocket. Mine does this at that depth.
  The Gcode module will be overhauled this summer, its a bit hard to manage I find, its all one class and it should be
at least 4. But, your sprocket should cut as your doing it at the proper 3.05 depth. Total depth sets the actual width
of a 4th axis cut, not its depth. The tooth depth is actually calculated from the tooth, it cannot be changed by the user.

Art

[Stephen Fornelius]

Thanks for the quick response Art.

I downloaded the new version.  Looks the same to me, but this is my first LARGE gear using 4th axis.  As I understand what you say, the cutter thickness is the criteria, not the depth of cut.  So if I change the cutter thickness from 0.2 to something larger, it should cut deeper?

I'll give it a try today with the G-code output and see what it looks like.  I have the chain already, but I also have to face the material down about .015 to get it thin enough to go between the links.  After I face it, I can test the fit.  Its going in a clock, so its not super critical how much the teeth engage the chain.

This is part of my chain-and-sprocket concept for a wall clock.  Instead of gears that mesh, I want to see if this idea is possible.

Steve

[ArtF]

  Its really that 4th should be on a different screen than 2.5D for example so the labeling works. The Max Depth setting is the thickness of the stock really.. As you change it youll notice the sprocket gets thicker... The actual cut depth into the sprockets tooth towards blank center is controlled by the actual depth that tooth is by its design. If useing an end mill then it may not fit to the bottom of the tooth
and so the code may not go so deep, but if using an involute cutter of some sort, then it should always go to the right depth. In your example you stated a #25 Sprocket which has a tooth depth of about 3.05 or so, and thats what comes out on my Gcode...

>>G0        X 3.0000  Y 0.0000 Z 5.0000  A0.0000
          X 3.0000  Y 0.0000 Z -1.0000  A0.0000
G1 F600.0X -3.0000  Y 0.0000 Z -1.0000 A 0.0000
G0        X -3.0000  Y 0.0000 Z -2.0000  A0.0000
G1 F600.0X 3.0000  Y 0.0000 Z -2.0000 A 0.0000
G0        X 3.0000  Y 0.0000 Z -3.0000  A0.0000
G1 F600.0X -3.0000  Y 0.0000 Z -3.0000 A 0.0000
G0        X -3.0000  Y 0.0000 Z -3.0980  A0.0000
G1 F600.0X 3.0000  Y 0.0000 Z -3.0980 A 0.0000
G0        X 3.0000  Y 0.0000 Z 5.0000  A0.0000

Art

[Stephen Fornelius]

Plan A didn't work - the fly cutter isn't cutting and the tool actually gets knocked back into the cutter holder.  Tightened the screw till it snapped off so that's one thing I have to work on.

Plan B - my original idea.  Is these a way to use the rotary table horizontally instead of vertically?  Something like "table aligned to z-axis" instead of y or x axis.  Were this possible, I could position the zero at the y-axis center of the table, then the tool could cut into the edge and a combination of x and y movement could form the profile.  Just for giggles I switched the motor cables to see what would happen.  Switching x and z gave me little blocks indicating the depth of cut, but tangential to the circle.  Switching z and y gave me a drilling pattern.  I used a pencil in my collet to test this BTW.

Plan C - export the DFX to BobCAD, then delete 1/2 of the gear.  Cut 1/2 and then rotate the table 180 degrees and repeat the machining.  If nothing moves, I think this would be fairly accurate IF I can make BobCAD only cut 1/2 at a time.


Steve

[ArtF]

Steven:

    While I admit it would be possible to have the rotary do that, it'd likely take alot of work
to do so. ( Though I do see merit in it for smaller worktables with rotaries to be able to do larger gears.. so
Ill add it to the development list..). I dont think a simple swapping of axis would help, but you could always
take a 2.5D Gcode output, take the cutting of say 45 degrees of teeth and remove all else from the program.
Run that code, then simply rotate your blank 45 degrees and repeat. Be the same thing wouldnt it?

Art

[Stephen Fornelius]

Plan C worked pretty well.  My Taig has some significant limitations in its work envelope.  I tried to do tangential milling from the top of the blank (cutting in air) but the blank hits the headstock bracket when it tries to cut the side of the gear - so that's not going to work with anything much larger than maybe 4 or 5 inches.  To even get to this stage of testing, I built an offset bracket and raised the Sherline rotary table 1".  That gave me vertical and horizontal clearance for my fly cutting test.

Using the DFX from Gearotic and running it through BobCAD to selectively mill 1/2 the gear teeth actually works pretty well.  The 180 rotation of the table  worked fine (realizing that the number of teeth were even).  If the number of teeth were odd, then at least one of the teeth would have to be cut twice obviously.

I still think being able to use the rotary table horizontally to do tangential cutting on the side of the tool would be a very handy update.  The concept would have to have the milling cutter on the y-axis and the size limitation would be the distance between the center of the y-axis and the z-column. 

Steve

[ArtF]

Hi Steven:

  Thanks, I will keep on my development list a way to do a larger gear on a flat rotary..
Glad to hear one of the plans worked..

Art

[Stephen Fornelius]

There were a couple of issues with my plan C.  Had to buy y-axis extender from Wildhorse Enterprises and then made a 1" copy of their extender.  Ran the program and it BARELY cuts the 6 7/8" gear, but it does cut it :).

Did an interesting experiment too.  I wanted to do a finishing on the surface to reduce the thickness to .11".  I used a mill first and cut across the gear, but didn't really like that pattern on the big gear.  A friend said to try a fly cutter, so while I had the piece bolted to the rotary table, I used the fly cutter and rotated the piece 360 and then 0 degrees.  Made a VERY nice guilloche pattern.  Then I moved in from the rim and used a mill to cut the spokes and hub with the rotary table doing 360, then move 1/2 the cutter and rotate in the opposite direction.  Very pleasing effect.

Wish I could find an EASY way to learn CNC programming so I could automate these tasks.  Do you recommend anything?

Steve

[ArtF]

>>Wish I could find an EASY way to learn CNC programmi ng so I could automate these tasks.

  In my experience its easier to learn CAM in the context of one software or another and use that to
generate the code, G-code programming with logic is an esoteric art nearly dead..

Art

[Mooselake]

For a couple ideas heekscad/heekscam is a usable open source product, if a bit quirky, with a newly released modest cost upgrade.  CamBAM has an older version that's free and quite usable.  There's an inkscape add-on that's usable; I use it for engraving.  All will let you experiment and get started while investing only your time, and (in my experience) a bit of adult language and possibly some hair pulling.

Somebody else can chime in for commercial products.

Kirk

[JustinO]

Stephen,
LinuxCNC can be fun to "hand code" if you are a programmer. It has embedded math and parameters, and embedded structured programming. I do wacko stuff with it that can't be done vie the normal CAD | CAM pipeline. If you're a nerd and enjoy trig and loops, it might be worth playing with.

I'll check in later to see if my account here is still active....

[Stephen Fornelius]

Thanks for all the replies.  I was thinking about cnccookbook's g-code editor and conversational program.  My main brain-farts are I don't follow how the variables work.  I remember DOS and the thick manual on how to run it.  They gave a command, and then some variables but the book explained what the variables were. 

Things like incremental move - I was thinking about jeweling a flat piece - where you tell the program to execute a command like z=0, and then return to z=.25, move from x=0 to x=.25 and repeat.  Then the next line to be surfaced would be x -.25 for a start point and then repeat.  Things like that.  And especially doing things with the A-axis (I bought the rotary table and I'm damned if I don't use it for something!).

I'll keep looking around to see what's available for learning - some of the books look interesting, but I'm not sure the direction I should be taking in that kind of education.  Right now I keep fiddling with BobCAM until I get something that looks right and let the program do the g-code.  I can sort of read through the g-code step by step, but the headers etc. are a mystery to me right now.  I also realize I've only been working with CNC for a few months too.

[ArtF]

>>I'll check in later to see if my account here is still active... .

lol.. Your account is safe. Ive never had a problem with LinuxCNC, hell Mach3 was based on it
and Ive met its developers, all pretty good people. Ive been away from Mach3 now for years,
though I still have very fond memories of the hectic times I had in its development.

  So if your a LinuxCNC guy, feel free to extoll its virtues here, Im truly an equal opportunity
CNC-er. ( Actually I use a version of Mach3 (version 7.777) no-one else has or has ever
seen... :-) ).

Art

[Wod]

You cut me deep Art. I don't feel esoteric or nearly dead either one.
Wiley