Cutting Tool Generatin -- new name

[philbur]

Hi all, I'm trying to run the demo version 3.34 using the tutorial. The tutorial appears to be for version 2.0. The screen layouts are not the same, particula rly the left hand panel in the "Spur Gears" window. For example I am currently stuck trying to find "add slave to project". Any guidance would be appreciat ed.

Here's a shot showing the left hand panel of the Demo:



-----------------------------------------------------------------------------------------------------------------------------------

Here's the tutorial window. Compare the left hand panel with the Demo above:



Phil

[John S]

Add slave to project is now "Create Pinion "

[ArtF]

Hi:

  Sorry for that, but the video will be updated soon. The GUI changes as of version 2.1 . Fucntiona llity is pretty much the same,
but the locations of certain items may have switched about. The old screens took up too much screen space for some users, the new ones allow for better viewing and usage.
I hope to have the new video soon, I did one last week but wasnt happy with it, so stay tuned ..

  Also, the help file is found under the menu item for ?.. and shows the current screens and what the buttons do..

thx
Art

[philbur]

Thanks for the feed back John/Art.

My interest is in Module gears in the range of 0.7 to 1.0 so I am particula rly intereste d to see if I can use the cutter wizard to make a single lip cutter in silver steel to an adequate precision, then to check to see how the cutter holds up on say a 60 tooth, spur gear. Just to get a grip of the process I first plan to make a Module 1.5 - 30 teeth cutter, hopefully tonight.

Phil:)

[John S]

I made a 1.5 mod 15 tooth cutter the other day but it didn't hold up very well.

Note to self : don't use brass next time 

[philbur]

OK here's my first attempt - 12mm stock - 1.5 Module - 30 teeth:



Comments:

It looks like I didn't reference the end mill sufficien tly accuratel y, see flash on the side of the cutter. There was also a thin disc of flash on the tip. It would be nice if the program allowed for removal of this, if possible.

The end mill left a very shallow step (thumb nail) across both faces of the cutter. Approxima tely 2/3 the way up the involute curve, not my fault.

The significa nce of the collar ratio is not clear to me.

The program leaves the operator to select cutter thickness as a percentag e of the stock diameter. It seems to me that the cutter would not function correctly if this thickness is to great. Conversel y you don't want the cutter thickness to thin for reasons of strength. Surely there is a optimum thickness, could this not be calculate d and input automatic ally or at least suggested .

No complaint s just comments.

Phil:)

[ArtF]

Hi Phil:

  Interesti ng..

 Firstly.. the flash may be my fault... I got it as well on  a coupel of mine and Im still trying to figure out why...
Some of mine have no flash, some have it.. Ill look again at the final depth calculati on..

  Second.. Colar Ratio is the amount of bar flattened above the involute section. It seemed to me that Id want a bit of clearance bar above the tooth,
so a colar ratio of 1.0 woudl mean 5 mm's of flat bar above a 5mm involute section. Acollar ratio of 2.0 woudl be 10mm's..ect..

  Thickness is soemthing I was wondering about, and your right, too thin and its too weak, too thick and it would overcut.. And since the shape
varies Ive yet to think up a equation for that.. the default of 25% seems to work on all examples Ive tried.. so I left it there till I see enough examples
to give me a hint as to how to deal with that one. ( As I said, there doesnt seem to be any literatur e on this methodolo gy.. suggestio ns are welcome. )

  As to the "thumbnail" , do you mean at the tip the bar seems to be thinner? IF so, thats a bar that beding under cutting stress, beacuse if you look to the
Gcode, youll find its all on a plane, so it cant cut other than flat for any reason other than bending.. I dont think....

  I REALLY appreciat e the photo, it helps to see what you get vs what I get from softer material. Ill do some work on the flashign problem, funny thing is I
calculate the final depth properly and add 10% for safety..s o Im messing up somewhere .. or, bending is more of an issue than I thought.. I notice the flashing seems non existant at the base, and grows towards the thumbnail effect.. SO Im thinking its related. I wonder if the depth per pass has an effect there. You might try lowering the depth per pass to see if it rectifies .. Ill try it here as well.. Now that I think about it, the flash is worst when I do a 1.5mm per pass as opposed to my .5mm per pass runs.. ( Different for all materials obviously .)

 Again, thanks for the photo and the test, Ill make changes for a new release to rectify it as much as I can. If anyone has suggestio ns on bar thinkness Id love to hear them. TO me, the thickness shoudl probably be a function of the smallest diamter section.. Perhaps we shoudl be cuttong not a flat bar, but a bar that thins as the section narrows.

Thx

Art

[philbur]

Surely the flash can be avoided by just lowing the Z position a bit more for the final pass. The disc flash on the tip could be avoided by adjusting the x axis tool offset by say 0.1mm. The flashing on the cutting edge occurred only on the low side, due to the clearance angle rotation I guess.

There is no physical relations hip between the stock diameter and the maximum allowable thickness of the cutter. The cutter thickness has to at least be equal to or less than the diagonal width of the cutter at the tip.

I also though about thinning toward the tip. However that will require tilting the RT (pain in the neck) or motorizin g a BS dividing head. Possibly worthwhil e or even necessary on smaller cutters.

It seems to me that the cutter is a two lip cutter. If this is the case the the generated tooth profile will be according to the diagonal plane through the two cutting edges and not according to a plane parallel to the cutter face, if you see what I mean. Correctin g this would make for some pretty tough mathemati cs though. The thinner the cutter the closer it will be to the correct profile I guess. A single lip cutter would also solve this but cutter life would be reduced. A two lip cutter however also requires much, much higher precision if it is going to be effective on both edges.

Just some thoughts.

Another question: Does the code for direction of approach minimize any issues with respect to backlash/lost motion in the machine.

Phil:)

[philbur]

It just occurred to me that for the smaller module cutters it getting more like an engraving cutter. These are single lip which avoids the precision issue and the diagonal profile issue. Conical improves the stength issue.

Phil:

[ArtF]

Phil:

>>If this is the case the the generated tooth profile will be according to the diagonal plane through the two cutting edges and not according to a plane parallel to the cutter face, if you see what I mean. Correctin g this would make for some pretty tough mathemati cs though. The thinner the cutter the closer it will be to the correct profile I guess

   Thats already done. The profile thats cut takes into account the relief angle and is on the diagnonal plane. Its not the involute itself. Look at my photo of one held in a tooth of a gear. It shows the profile is actually seen by casting the a shadow of the cutter, not the flat plane shape. The math isnt that bad..

 The flash shouldnt exist. The math of the depth is also done to correct for the relief tilt. But I may have screwed that up somehow.. Im still checking. . I even cut it 10% deeper than the math calls for..so I having a bit of trouble figureing out where I must have messed up.. more later..

Art
 

[philbur]

I guess I started this thread in the wrong place, sorry. Move it if you prefer.

So you are saying the tool path doesn't follow the involute profile but an involute profile adjusted to take acount of the clearance angle and the diagonal length (edge to edge) due to cutter thickness .

Phil:)

[ArtF]

Phil:

>>So you are saying the tool path doesn't follow the involute profile but an involute profile adjusted to take acount of the clearance angle and the diagonal length (edge to edge) due to cutter thickness .


   Yes. Just to be clear, heres how it works. When you design the gear, a single tooths full shape is snapshott ed, thats the shape you see in the small graphics box.

  This is a bit oversimpl ified.. but that snapshot in on a flat plane of course. The shape then has a collar added to it, ( which is bascially a line thats vertical from the top edges upwards by the defined ratio.)

  The next step is to rotate this structure by the relief angle. This gives us not only a new X and Y coordinat e, but a Z coordinat e based on the rotation.

  Then, this rotated plane of data, temporari ly has its Z coordinat es zeroed. A tool offset is done to this new flat plane coordinat e data, and then the Z data is added back in. This creates a toolpath that is properly at the height of the cut on the inside tip of the cutting tool.

  I say this is simplifie d because the bar thickness is taken into account for the Z coordinat e data
of the cut. But the end result is a tool path that is properly offset after rotation to the relief angles plane.  So the end involute shape is corrected fully for the rotation of its data. It is not the involute shape per say that you started with, but rather the shape the cutter would need to generate that original shape.

   I suspect, but Im unsure, that a problem may be in the algorithm for the bar thickness correctio n, which could explain the flash.. but bending of the material while cutting could also explain flash.

  The last version modified the cutting of the bar to make the tool move in from the side during bar creation to lessen any effect of bending while cutting the flats.

 When doing the actual profile ( whicch youll notice follows the Z cooridnat es of the bend also moves in from the side to try to eliminate bending, but due to the nature of the moves in the final machining its hard to eliminate bending posibilit ies.

 Our end result is that when each lip moves to the flat plane, it then represent s the original involute shape only on that lip..


Art

[philbur]

Possibly I'm doing something wrong but the two photos below seem to show that the cutter could not cut the profile it was made for. Clearly the cutter thickness is to great, however if the thickness is compensat ed for it should not look like it does. This is an example of the issue I raised about compensat ing for the diagonal distance from ledge to edge. Obviously the thicker the cutter the greater the distance from edge to edge that needs to be compensat ed for if the width of the tooth profile is be as required. The profile of the two adjacent tooth flanks may be correct but their separatio n will definitel y be to great. Theoretic ally if the cutter width is greater than the tooth tip face width then the program should have removed all of the cutter material at that point.

This possibly returns us to my points about the advantage s of a single lip cutter.

Face on:


Side on:


Phil:)

[ArtF]

Phil:

  Entirely correct. I dont think you did anything wrong at all. The thickness IS an issue.
I dont think theres any way to go other than for me to figure out by algorithm the
proper thickness .

  I think the theory of it all holds together except that the thickness has a maximum that must be contained .
Ill try a rewrite tonight of the thickness determina tion, lets see what I can come up with.  All of mine were done
from stock not much larger than the tooth, which may have made the differenc e in how they came out.

Art

[ArtF]

Phil:

 Thinking a bit more about it, and I think a signle lip cutter woudl have the same issue. ( If by single lip you mean basically cutting that tool in half..)
That tool you made looks as if it woudl work, if it were about half the thickness it is..

  I guess one way to think about it, is that if we were making a tool to cut a v shaped tooth, with no flat, the requireme nt would be a cutter that is basically a VBit.. so a bar type of bit just wouldnt work. No matter what to use a bar type of bit, the bottom of the tooth must have some width otherwise the bar must be infinitel y thin..

 SO to me it seems there are some shapes that just woudlnt support this method of making a tool. That having been said, there has to be a formulaic way fo telling just how thick the bar must be.  Im thinking the method has to be to figure the root clearance from left to rigth involute, and the thickness must be less than or equal to that distance. So for this method to work best, the tooth must have a flat root ( or near flat ) and the thckness should be clipped to that width.

Your thoughts?

As to the shape, the thickness determine s it. The shape will actually cxhange as the bar becomes thinner due to the way the math works out in the rotations .

Thx
Art


Ill try to do soemthign tonight and see what it shows.