ArtF wrote: I mean its great this cuts that way with the edits..but I cant count on all systems being able to remove in the tangential stage what wasnt removed in the rooting stage. ( That was the common support problem in GM...which is why the rooting is trying to take so much..
You could overcome this by making the Tan shaving start from the top segment and step across just like the rooting currently does. If each step is a fraction of the full Y and A values for that segment it can never over-cut like the rooting does.
Here's the edited code. The editing error is still there, I think it is at the end of the Tan shaving. It moves across (+x to - x) and down (+z to -z) as a diagonal before starting the rooting, instead of just down, hence it clipped the top of the tooth.
Phil :)
PS: If you want it to be applicable to the widest range of machine and set-up conditions you must give the user full control over all step sizes, or it will always be either to aggressive or to slow for somebody!!!
PPS: I think I see the problem with my proposal for stepping the tan shaving. But it still might work depending on how big of a step the user choses.
Attachments
[The extension txt has been deactivated and can no longer be displayed.]
Last edited by philbur on Mon Apr 28, 2014 8:04 pm, edited 1 time in total.
1. Run the end mill straight across the middle with a user defined step down per pass to the base diameter.
So does that mean the root side moves were responsible for the gouging in the end? Actually I'm not sure anymore, I stopped the run and re-zeroed after some editing. I had assumed that was the cause.
2. Run the tangential shaving above the base diameter with a user defined step up and across per pass.
When you say step up, what do you mean? Did you keep the depth tot he base circle no matter the Y position? Start with the lowest segment and work up, just as per the original code.
3. Run rooting below the base diameter with a user defined step across and down per pass.
Same here, was the rooting effectively changed or just some clipped out? Again no change just clipped off all code above the base diameter.
Art, are you using something like this as the basis for the Z and Y coordinates of the cutter position relative to the involute when rooting above the base diameter.
Here is the rooting of a very thin blank compared with toothing the same blank. Note that due to the virtually zero thickness on the blank the toothing tool path shows no overlap witrh the involute profile whereas the rooting does, why. The rooting profile looks like it is using the root diameter as the basis for calculating the Y and Z values rather than using the base diameter. Have you checked which diameter the rooting uses as the basis for roughing the tan shaving area. Such an error would be more noticeable with lower tooth counts.
From calculation when the involute angle pass 90 degrees Y continues to increase but Z starts to decrease. So the over extended cut near the tooth tip is possibly the last step in the process, not the second from last as it appears on the diagram. That would be the optical illusion.
For a 4 tooth helical If you are using the root diameter instead off the base diameter then the involute will pass 90 degrees before it reaches the full height of the tooth, from root to tip. So Y will still increase but Z will come back down. Voila
Just a possibility.
Phil :)
PS: well maybe not, the even vertical spacing of the seps does not support the theory!
Still trying. This rooting (again, a very thin blank) looks like it is following an involute profile all the way from the root. Does this support the theory that the calculation is based on the wrong diameter???
One of the problems with discussions such as this is the medium doesnt allow for understanding very easily
whats being communicated. It makes it hard to make a point. So forgive me if Im not explaining what was asked.
First, yes your involute diagram IS whats being used for the profile information when the gear is generated. But when its toolpathed, the actual shape is used, not a formula. The issue is that if I were to use involute formulas, only involutes could be machined, all other shapes couldn't be as they aren't involutes. GT uses the actual tooth profile
in order to allow it to try pulleys sprockets, or perhaps noncirculars in future as each tooth in an elliptical uses a different shape involute.
So since the system uses the tooth shape itself it cannot mess up as to what is the profile and what isnt. Its why I keep suggesting you look at a spur not a helical. Youll see in the spur gear there is no crossing the profiles lines. The helicals dont cross the lines either, they just look as if they do because your looking at them from the front where the tool is set to a starting point made necessary by the additional helical angle needed to hang the tool in front.
Hmm, best I draw this point, its a hard one to word.. look to the photo below. The top shot is the helical, to machine its helix properly the toolpath has to start outside the profile and end outside the profile because the tool must start in front and end in the back with the same angular offset. Its why I keep saying its an optical illusion that the profile
is being violated. Look at a spur, same code generator, notice there is no profile crossing..because there's no helix.
The toothing and the rooting both use the exact same profile information stored in the shape. Its only 1 shape.
Now it can be the rooting is getting too close to the profile, that's possible, though the numbers deny it. Its possible
because its a tangent function that determines how close to get to the profile, and as the angle of the profile approaches 90 degrees the answer is "infinite".
In any event, it seems form your last test that the tangential is fine. ( Did you get only 4 because you cut out the return paths? For 8 segments it cuts 4 times across, then back....). So at least we then know its IS the rooting getting
too close to the profile for some reason. While I could as you suggest lower the rooting to less material removed it can cause trouble in other gears which is why I have to understand the issue rather than fix it, or rather understand fully before fixing otherwise Ill end up doing it several times as other gears get messed up. This is why sometimes I know it seems as if Im not listening, a user focuses on the problem at hand, I need to focus on the problem as a symptom of a larger more encompassing issue.
I will now look deeper into the rooting to see why it apparently gouges when it shouldnt.. That display was carefully designed to show what WILL cut, so its confusing the display doesnt actually show the rooting cutting into the profile..
You ask why the root seems to cross when he toothing doesnt appear to. Actually both appear to, but neither does.
Look at the tips of the toothing path, imagine if the tool in its place, the radius of the tool would go outside the profile....same effect as above, just doesnt look as bad because its a tangential shave not a root pass, same illusion..just different. lol. .if you look at the sp[ur equivalent, the toothing never gets closer than the radisu of the bit to the profile, in a helical it appears to almost touch it, and if its a long helical it will cross over it..same illusion..
Again, look to the nonhelical spur.. its the real path, the helical display of it just messes with your head. Id really love to know how a spur of the same gear cuts without edits.. I suspect youd have the same cutouts because something I havent identified is wrong.. but the illusary nature of the profile when viewed from the front on a helix is leading away form the real problem I suspect.
You know, it was driving me crazy that while I could change a spur's thickness by changing "final Depth", the helicals were always as designed. I just uploaded a fix for that. You can now change the thickness of the helical the same way.
This makes it much easier to test various things..change the thickness as you wish from any thickness helical..
It may help. :)
>>Just out of curiosity what do you mean when you say "the actual profile is used". How do you it convert the profile >>(a diagram) into coordinates?
Yeah, I should explain.. :)
I use the tool shape drawing you'll find on the DXF's. While I could use the formulas you suggest for spurs, I couldn't use them anyway for helicals, the tooth shape of a helical is not an involute when viewed from the side. You have to turn a helical to the helix angle to see an involute shape. A helical is larger than a spur by the cos of the helical angle, so the involute shape gets stretched out of proportion when viewed transversely. But then helicals come in two flavours, transverse helicals and normal helicals. These terms refer to the way you view the tooth. If the tooth shape should be involute when viewed from the side you make a "Transverse Helical", which means you dont increase its size. (You check the box labeled "Dont resize")
If you want a helical which is involute across its normal (the helical axis), you design a "Normal Helical". (The one your cutting is a "Normal Helical", this means the tooth is not really an involute when viewed side on, which means a cutter must follow a non-involute curve to cut one.).
The tool shape stored with each gear type is stolen from the gear outline before its teeth are copied around the gear. I design one tooth and copy it in all gears except non-circulars where each tooth is different. In the case of your helical for example, the non-involute result of the calculations is stored, then re-zeroed and kept in memory as "ToothShape" - a series of points referenced to 0,0 being top center of the tooth. When the toolpather goes to make a helical toolpath( or any toolpath), it looks to that stored tooth, does collision calculations and curve fitting operations to find any point intersection with that curve. SO when its rooting for example, I start at the top and ask the intersection calculator "How far to the left before I hit the profile at this depth?" I subtract the clearance and tool radius from that and thats how far over I go. Each depth is different width of course. This allows a sprocket, pulley..anything to be machined with the same strategy.
For toothing, same deal. My intersection calculator returns not only the intersection point of the toolcurve for any given depth, but it also returns the normal for that point. So I then rotate that normal to 0 degrees, move the tools edge to that point, and do a pass. That means the tangent and rooting passes use the same points and same intersection calculator. It why I can say with some certainty that its not the points being wrong. So to check numbers, I need only to look at a spur gears toolpath. I can measure on screen using the tape how far the edge of the path is from the profile on every line on the Y cutting axis., and Im always getting toolradius+clearance distance.. BUT, as the profile lies flatter and flatter on the cutting pane, a root path looks closer and closer to the edge as we discussed on the first optical illusion. It is the right distance from the edge of profile, but AWFULLY close to the point beneath it.
The thing that confuses me the most is why your clearance appears to make the root wider...the path seems to indicate its getting narrower...
>>I will have a go at a straight spur later today.
That will be an interesting result.
>>Yes trying to have this type of discussion basically by email is very frustrating.
Been saying that for over 10 years. :) . Hey, I live this stuff, I dream in 3d at this point and normals, vectors, tangents and such roll around between my ears. I see things you cannot simply because Im involved in their math every day. On the other hand this blinds me to things I dont do every day ..like cutting gears. It makes it hard for me to see what your saying in exactly the same way its hard for you to see what Im saying. In the end its only about getting enough evidence to point to the trouble. It all helps though, I now know how many more config items I have to add when I redo the 4th axis to its own tab. I agree with you, more step size choices need to be available, Ill make that happen..
Im off insulating my attic today, so dont rush any tests on my account. Ill be sweating in other ways.
Trying to run the straight spur but there seems to be something wrong with the gcode values versus the gear blank thickness. See attached. The gear blank is 5mm thick but the x axis only cycles between X+1.5 and X-1.5, which is the tool diameter. clearance is zero!!!
Phil :)
Attachments
[The extension has been deactivated and can no longer be displayed.]
