Cutting Tool Generatin -- new name

[philbur]

The width of the diagonal between the two cutting edges should be the involute profile width at that point on the profile.  Clearly not only will the end-mill have to follow a path that is a "narrowed" involute profile but also the end-mill path will have to be distorted from the true involute path because the cutting edges are not perpendic ular to the the cutter. The issue is much clearer when you look at figure 2 in the diagram.

I know you may have answered this before but I can't get my head round how you would make these correctio ns without some very fancy maths.



Phil:)

Then rotate the bar and the shape to the relief anngle. This should all work unless you see anything Im missing.

Art
 

[philbur]

Now I'm not so sure about my second point regarding a requireme nt for distortio n compensat ion.

Phil:)

[ArtF]

Phil:

 I just upoaded a version 3.57. I verified its math and that tis properly takingn into account the
diagonal of the bar. The display also shows the thinkness, and its based properly on the tooth, not
the bar your machining down.

  I will try to run one tomorrow to verify its code on the 4th axis, but I think , unless theres a bug in there ) that this
version will properly cut tools for larger modules, and show the limitatio n in size for the smaller ones. Ill post  a
photo when I do the test cut.

Art
 

[philbur]

Hi Art:

Ref V3.57.

There is no move to safe Z after each pass of the involute profile, so when it returns to the start for the next pass it chops the cutter off the bar-stock. Ooops.

Because of the relativel y thin tool it is necessary to run small DOC and stepover to avoid deflectin g the cutter during the last passes for the flats. Roughing followed by a finishing cut would reduce the time greatly. I could have faces both sides in two minutes manually, it took 30 minutes with the program, followed by an unplanned parting off of the cutter!!!

Phil:)

Phil:

 I just upoaded a version 3.57. I verified its math and that tis properly takingn into account the
diagonal of the bar. The display also shows the thinkness, and its based properly on the tooth, not
the bar your machining down.

  I will try to run one tomorrow to verify its code on the 4th axis, but I think , unless theres a bug in there ) that this
version will properly cut tools for larger modules, and show the limitatio n in size for the smaller ones. Ill post  a
photo when I do the test cut.

Art
 

[philbur]

Hi Art:

I had a second attempt. This time I cut the flats manually and then just ran the program for the volute with safe Z's inserted for each pass.

I thin the graphical presentat ion of the cutter thickness in the volute profile needs to be the diagonal thickness of the cutter. My second attempt was still to thick to sallow the cutter to rotate without rising some way out of the tooth profile as the diagonal passed over the tooth flanks.

The final Z height when cutting the involute seems to be way high. I had to run it again with Z0 2mm lower than the top of the stock. This may have something to do with me doing the flats manually and getting resetting of Z0 wrong, but I don't think so. The low side flash came of 2 passes earlier than the high side. Looking at the code as the end mill passes the cutter tip on the last pass the end mill should at least have a Z value that is half the stock diameter plus half the tool thickness and it is not.

Cutting the involute by progressi vely lower Z passes (with the same small DOC as the flats) seems to result in deflectio n of the cutter on the last pass. If the end mill came in from the side the risk of deflectio n would be greatly reduced and the need for constantl y varying the Z height as it follows the involute profile would be unnecessa ry.

Phil:)

PS: I think a better graphical presentat ion of the cutter tip would be your diagram 3, where the circle diameter would be equal to the involute width at the cutter tip location (at the root).

[ArtF]

Phil:

   3.58 is online ot correct the oops..

 I just cut one and Im doing some measureme nts on it to see what the number show. BAck at you soon..

Art

[ArtF]

Hi Phil:

  >>I thin the graphical presentat ion of the cutter thickness in the volute profile needs to be the diagonal thickness of the cutter. My second attempt was still to thick to sallow the cutter to rotate without rising some way out of the tooth profile as the diagonal passed over the tooth flanks.


    Your probably right. The one I just cut in 3.58 does fit well though.. but then the graphic showed a clearance on either side at 25%.. so its fits as expected. Ill change the display to show the diagnonal instead though, instead of how it fits at 90 degrees. You also have to be carefull when checking them to use a gear cut with GM, as GM's roots likely dont match retail gears, roots change from maker to maker, so a test gear pretty much has to match what GM does..

>>The final Z height when cutting the involute seems to be way high. I had to run it again with Z0 2mm lower than the top of the stock.

  Mine cut properly with no flash this time.. but Ill check the numbers.. both in the program and in the final Gcode to make sure that the depths are correct.. I do see that the zero is extremely important in terms of it doing the rigth depth, it doesnt allow much for error.

Art

[ArtF]

Phil:

   I just upped 3.59 which has the diagonal of the tool thinkness as its display. It also has a finish depth per pass, which is the involutes depth per pass.
Things are still cut with the varying Z, the algorithm was designed to accept only that, but Ill look into making it do it on a flat plane, many more passes
to do that though with the finish pass depth it may not be necessary .

  It seems to cut a decent tool now, that fits properly and removed what I expect, but I havent finished crunching all the test numbers to see if its proper.
Initial measureme nts on the tool seem proper for the mod 5 Im cutting, tooth width on the diagnonal and such looks right, depth is a touch more, but that looks
like my test gear depth was .5mm out when I cut it. Other than that, this tool would definitel y cut a mod5 gear..

  Family BBQ today, so Ill be off muching for the day.. Ill do more tests later..

Thx
Art

[philbur]

Hi Art:

How does one know the correct total depth of cut when using the cutter to produce a gear.

Also the root profile on the cutter will have zero clearance, not sure how much of a problem this may be. Using a slitting saw to pre-cut the slots to depth would help.

Phil:

[Chuck]

Art,

If you do a setup in the 4th axis so you can rotate the tool you could do the  relief cut and rotate the tool 10 degrees make the next relief cut and continue around in 10 or 15 degree cuts. This would automatic ally solve the relief problem and make a full 3D relieved endmill.

For 2 or more teeth just repeat the tooth and relief process as many times as you need.

An option to use a grinding wheel in stead of the endmill to form the tool would be nice.  That way we can grind carbide blanks or hard tool steel.  I have been making single point carbide taper endmills in the 4th axis with a Dremel Tool diamond cutoff wheel. It takes lots of passes at 0.0005"/cut but on a 1/8" cutter it isn't too bad.

It would also be nice to be able to make fly cuter forms in addition to end mills.  This too may be best done in the 4th axis.  Anyone wanting to CNC gears this way will already have the 4th axis setup at least X or Y aligned.

Chuck

[ArtF]

Phil:

   I you cut a gear, the depth shoudl be set ot the "Tooth Depth" given in that gears stats. That will pretty much make sure the entire tool is used.
As to the root flat having no clearance ..quite right. Id recommend giving it a quick shave on a grinder on any flat bottom section myself. Not much
I can do on that issue I dont think..
   Preslitti ng woudl help, at least it would eliminate any bottom rub, but I suspect in most cases a quick relief on the bottom made by
runnign it across a grinder would work. ( But Im no expert on the technique .. )

Art

[ArtF]

Chuck:

  Actually, I had been thinking the same thing. Since the relief is say .. 9 degrees, I shoudl be able to cut an involute very 9 degrees to make a multi flute with greater strength. . But ive only conisdere d it breifly, Ill give it more thought once this bar technique is fully examined. I dont have a problem with offering differing technique s, just dont want to tackle more than one at a time, each time I think something shoudl work intuitive ly,
we collectiv ely discover limitatio ns not obvious when it was first considere d..

Art

[philbur]

Hi Art:

Trouble with grinding the relief angle on the end is it has to be reversed either side of the axis of rotation.

Seems the maximum theoretic al diagonal tip thickness for all spur gears is approxima tely 23%. Anything thicker is wider than the involute at that point.

The reason I ask about the depth of cut is that the cutter doesn't fit to the full depth of my reference gear. So the cutter used to produce my reference gear must have had a different full depth of cut, if you see what I mean.

Phil:)

PS: All the commercia lly produced gears I have to hand have a much more rounded root. See post 12 first photo.

[philbur]

Hi Art.

I've been doing some studying (Oh dear, always a bad sign). Root diameter of a module 1 - 30 tooth gear is 27.5 mm. Your program calculate s it as 27.6859 mm. I guess the differenc e is due to the root radius, or absence there of. However if one where to use the correct calculati on for the depth of cut it would be to deep using the toolbit wizard. To avoid confusion, if that's what it is, it might be a good idea to give the full cut depth directly on the toolbit wizard screen?

My source reference is: http://www.qtcgears.com/Q410/PDF/techsec1.pdf

Phil:)

[ArtF]

Phil:

  Part of this though, is that differing manufactu rers use different formula's for their gears. Its worse with timing pulleys, no specs exist there that
dont differ from maker to maker. Some use one scale factor, some another for addendum, dedendum and root. Mine are a little deeper than some,
deeper than your example for example. But its not only depth, the root curve is sometimes trochoida l, sometimes a simple curve.
  Its why I say its hard to judege. Using the depth listed for that gear the tool was made for shoudl always be the right depth. ( Though your right, I shoudl show it
on the page, and Ill add that as well as putting it in the Gcode file..).

   The 23% as a max will vary with tooth stubbing and width changes, or profile shifts. Its why Im trying to be carefull that all is well in all modes, not just the
general case.

   In the end, I think all we can do is make the bit work as well as it can, its pretty near impossibl e to home build otherwise . All I really wantr to ensure
is that a gear cut with such a tool will meash with other gears of the same module, so the more important thing is if a gear made with the tool will mesh
with that reference gear, not if the tool does. A deeper root for example simply gives better root clearance ..


Thx
Art