Cutting Tool Generatin -- new name

[philbur]

Art,

I think the single lip would basically be a Vee shaped engraving bit with the involute profile where the the straight cutting edge is on an engraving bit. One point about a single lip engraving bit is that it has effective ly zero cutter thickness as there is no need for a second cutting edge on the back side, the face of the cutter runs through the rotationa l axis, which is not possible on a 2 lip cutter.

The second advantage is the conical shape imparts maximum possible strength/stiffness. The cutter is going to need reasonabl e stength because it has to cut over a relativel y long cutting edge.

To get a small cutter to cut on two edges is going to require concentri city much better than 0.01mm. This level of concentri city is normally achieved on a precision grinder. Most people are not going to manage that kind of precision on their CNC mill, so even though it may look like a two lip cutter in practice it will only cut on one lip.

For your "spade" shaped 2 lip cutter the cutter thickness must be less than the gear tooth root width which for small module gears is going to give a cutter thickness significa ntly less than 1.0mm. This is not going to be very strong for what is effective ly a form cutting tool. Also a simple "spade" shaped 2 lip cutter must, by concequen ce of it's design, be a negative rake cutter.

One possible process for a single lip conical cutter might be to use your program to cut an involute profile lathe form tool. Use it to turn an offset involute (conical) profile on the end of suitable bar stock, the offset in order to provide the necessary relief angle. Then face the conical section in the mill (orientate d correctly to ensure the correct relief) to produce a conical, single lip "D" bit arrangeme nt. Then harden and temper.

John Stevenson showed a hand formed two lip spade shaped cutter on the HSM site, maybe he can say something about it's form and function.

Johns Spade bit:


Phil

[ArtF]

Phil:

 Im thinking I agree. This bar type of cutter DOES work.. but only if the module is high enough to allow the thickness to be enough for the strength required.
This seems be true of both involutes and timing pulleys. As long as the mod is large enough they become possible. Too small and they become impossibl e.
(Amazing how confusing the topic is, isnt it?, you wouldnt think it being as they seem simple devices..).

   This method was basically derived from Johns idea as posted, and I suspect it works well as long as the mod is large enough as I said. The involutes Ive cut are module 5, and sure enough they do work, at least as far as spinning them in the gear I use for testing.. But your also correct that likely only one lip will cut unless one was very accurate as to center of cut. Thats the drawback of not actually being much of a machinist when I try to do such routines, I hadnt considere d first the centering problem, and second the small module effect on the bar size..

>>I think the single lip would basically be a Vee shaped engraving bit with the involute profile where the the straight cutting edge is on an engraving bit. One point about a single lip engraving bit is that it has effective ly zero cutter thickness as there is no need for a second cutting edge on the back side, the face of the cutter runs through the rotationa l axis, which is not possible on a 2 lip cutter.

    Hmm, do we have any balance considera tions to worry about if I retool this to a single lip? DO you have anything that shows me graphical ly what to try for in that
event? I do have some engraving bits, so I think I know what to aim for, Ill give this some serious thought before I attempt it. The good thing is, even if this current method cant be saved, the boilerpla te is all done and its liekly just a retooling of the way I do it.. 

  Your helping a great deal, I appreciat e your input..
Art



 

[ArtF]

Phil:

   I found that indeed, the code wasnt correctin g properly for the diagonal. Basically, the rotated tooth data had to be rotated by an additiona l correctio n angle that is equivalen t to the asin of the half thickness of the bar divided by the width of the flat plane toolpath.
Ive corrected that, leaving the thickness of the bar being the thing thats variable. This means as you say that small gears will be troubleso me due to too thin a bar being necessary . I suspect we'll need a different type of cutter for those as you figured . But for larger gears this method should still work, so Ill finish this code, test it and see about a thickness being auto calcuated, if too thin for a person, then we'll have to make an option 2 for smaller gears.. What amazes me is how well mine fit anyway for a mod5.. I hate tryign to think in multiple dimension s.. hurts my head..

 more later,
Art

[philbur]

Art: I think if you are also able to auto calc the correct thickness then that will help greatly in demonstra ting the lower limit on size.

Phil:)

[philbur]

Some more ramblings:

For your spade bit the diagonal across the cutter tip (from cutting edge to edge) must equal the gear tooth root width. Also the cross-section of the cutter tip is a parallelo gram. So you now have the length of the major diagonal of the parallelo gram. The included angle of the parallelo gram is set by whatever you calculate as the correct angle for the cutter face when machining the involute. These two values should allow you to calculate the optimum tool thickness (height of the parallelo gram). Oops, the machining angle partly depends on the tool thickness, but I’m sure you can solve that equation.

I think an additiona l issue that needs to be addressed is that the 2 none cutting edges need some clearance such that after the cutting edge has passed, and the tool continues to feed into the work, you don’t want the trailing, none cutting edge to contact the work piece. So somewhere in there is a calculati on related to tool tip geometry that can tell the user the maximum allowable feed rate. You could of course further improve this clearance by taking the edge of the none cutting lips, either manually or, with the correct maths, the mill (a tough piece of maths I think).

It’s much easier finding problems than solving them. The photo of John’s spade bit keeps saying “I see no problem”. I think some of John’s practical input is maybe needed.

[philbur]

Correctio n to the ramblings:

I don't think the length of the parallelo gram major diagonal and the included angle is enough informati on to fully define the parallelo gram geometry. However if you make an initial guess at the tool thickness, which must be less than the major diagonal (see next paragraph) then that gives you enough informati on to check the "feed rate" clearance for the none cutting edge. then you can adjust the tool thickness input to give a reasonabl e compromis e between tool thickness and not cutting edge clearance .

With a couple of quick sketches it seems that the tool thickness must actually be less the the length of the major diagonal x sin(machining angle as measured from the horizonta l)

PS: The known angle is not the included angle its the angle from the horizonta l!

My head hurts!

Phil:)

[philbur]

John's video also says "What's your problem":

http://www.youtube.com/watch?v=fps0OR1eF_s

It would be extemely interesti ng to see that cutter up close.

Phil:)

[ArtF]

Phil:

   I just added that last night. IT turns out I messed up in the code on
that, The 25% default was supposed to apply to the tooth width, not the
stock width.
Since most involutes have a root space of about 25%, ( which is why I chose
that default ) that would allow the tool to fit normally. In fact when I
check as
to why my bits appeared to work I found that the 25% of the stock I was
using turned out to be about 3.9mm thick, and 25% of the tooth width was
3.84.. which is why my tools appeared good, when others woudlnt. Just bad
luck. Turns out my bar stock was close enough to the tooth width to mask the
error.

  I cannot make it automatic it turns out..this is because various teeth
and timing pulley teeth dont have easily determina ble root section width..
BUT,
I did find by locking the thickness percentag e to the actual tooth, the
numbers work much better. AND its much easier since Im adding lines in the
small iconic drawing to show how the tool will fit when that thickness is
applied. It allows the default 25% to look pretty good, and allows you to
change it and see the end effect. So if cutting something perhaps a bit too
thin, you can thicken it up and see just how much your killing the bottom of
an involute for example.

  In other words the thickness, when too thick, has the effect of flattenin g
the root section, just how much it will flatten will now be shown
graphical ly.

Ive also modified the math so that the diagnonal section of the thickness is
taken into account. I hope to have it out in a day or two after testing. So
I wouldnt
bother cutting any more tools till I confirm that math on my indexer to make
sure this next version works better. As I say , at the moment I think the
cutting will work, but will be limited by end thickness to usefullne ss
depending on how small a tool one can make in terms of strength. Im not done
as yet, because curiously, it looks to me like when properly compensat ed for
the diagnonal, a relif exist without tilting the bar.. for example if the
diagnonal correctio n is a bar is done, then cut on the flat, a relif angle
exists which is the diagonal sections angle. So Im not sure how Ill handle
that as yet. Ill see if I can make up a cad phot to show what I mean.. and
we'll discuss it further..

  My head hurts too.. its AMAZING how hard this really is...



Thanks,
Art
www.gearo tic.com




----- Original Message -----

[ArtF]

Phil.. et al..

  Heres what Im looking at for the next version. This shoudl correct for all but the problem to a bit beign too small to make.

The first photo is the new display. As you change the bar thickness percentag e, you see graphical ly how the bar at 90 degree's will fit in the tooth.

The second photo explains the process. Do you see any error Im missing?

Thx
Art

[ArtF]

More explanati on..

   I used a simple rectangua r shaped tooth for this example just for ease of display. Item 1 shows the bar thickness, then I rotate the rect shape to the diagnonal s. Then rotate the bar and the shape to the relief anngle. This should all work unless you see anything Im missing.

John? How about you, does this look as youd expect the math to work?

 The display now shows two lines to represent the fit when the bit is at 90 degrees' making it much easier to visualise the end effect..

Art
 

[Wod]

Call me crazy Art, but couldn't you just use your original shape in a fly cutter, and cut the gear tooth on the side instead of the top?

[ArtF]

Wod:

   I think the problem is you need the relief angles to actually do the cut, otherwise youd bind.. If Im undertsan ding the question.
(Its the hardest thing about these discussio ns, graphical ly its much easier..)

Art

[philbur]

I might be wrong, but I don't think you can cut helical gears with a fly cutter. I think fly cutting spur gears is a common technique . However the point is an interesti ng one. I believe the original reason for vertical was to allow the use of a standard end mill, eliminati ng the need to resort to special cutters. However with a program that will mill you an involute curve at the press of a button all kinds of possibili ties for making different t style gear cutters opens up.

Phil:)

[philbur]

Going right back to the start. Most HSM’ers will have a fairly light weight CNC machine so nibbling away with a standard end mill for the large module gears has a number of significa nt advantage s and you should stick with that. However the core problem for smaller module gears is the strength of the end mill. A conical shaped cutter will give the best strength and nibbling (rather than trying you taking the full profile at a single swipe) will further reduce the risk of breaking the cutter. To minimise the inconveni ence of needing a special cutter stick with using th CNC machine to make the cutter or make it work with engraving type cutters, which can be had in carbide. Also this way means one cutter can suit a whole range of gear teeth sizes and profiles.

Conclusio n:

For small modules start with a single lip, conical cutter with a straight (no involute) cutting edge that nibbles away at the tooth profile in the same manner as the plain end mill solution. If you can’t make this work then the other alternati ves are even less likely to be successfu l. The only disadvant age I see is that the milling time will be much longer. However once you make this process work you can work on clever stuff to reduce the time required. This solution would have the potential to fit the widest range of needs, from the watch maker all the way up to larger, steel gears.

For larger modules stick with the plain end mill solution until you see some clear advantage s appearing in the small module solution.

Phil:)

[philbur]

Hi Art:

I can't see anything wrong (but that's no guarantee) with your current plan other than some possible presentat ion tidy ups that can come later and the other issues previousl y highlight ed.

Let see how it runs.