How do I machine an Accelerating Pitched Scroll?

[pbd1971]

Hi to you all, hope I am in the right place to ask this question. We have a job coming up soon which I could do with taking some advise on. Sorry, I don’t have a drawing at the moment but will do my best to describe the component.

The component is 150mm (6”) dia. 600mm(24”) long Acetal bar. It is a Scroll used for transferring bottles on a bottling plant line from one rotating wheel to another.(Imagine a big worm with a wheel at either end) The bottles are 76mm (3”) dia so the scroll form required cutting around the outside of the bar is a 38mm (1.5”) radius.

This is where it gets tricky, the wheels at either end of the scroll will be rotating at different speeds so the pitch of the scroll needs to accelerate from 100mm (4”) pitch to 125mm (5”) pitch over the 600mm (24”) length.

We do not have a lathe mill so will hope to produce this component on a Haas VMC using the rotating 4th axis. Another factor is the cutters to use, we have a 20mm (.75”) ball nose cutter. The reason I have selected this cutter is that we will have some variations on this component with different radii required for different bottles which we will be producing in the future.

Are we looking at CAM software or could this component be produced using G Code programming?

Many thanks.

[Geof]

Interesting challenge. I think the elegant solution would be a macro but in these modern times probably CAM is the answer. However, my math skills long ago became too rusty to figure out a macro for a varying pitch screw, I never learned CAM and don't intend to start now. So I would approximate it by writing a lot, but not an unmanageable amount of, G code.

The ends are easy because you want the bottle moving at a constant speed there, so you only have 15 inches of length to be covered at an average pitch of 4.5 inches.

This is three and one third revolutions or ten thirds of a revolution which can be covered by ten moves of 120 degrees.

Each of the ten moves would have the pitch increased by one tenth of the difference.

Each 120 degree segment is the increased pitch divided by three and added to the exisiting position:

I suppose in a macro it would be written as X = X + (4.05/3)

Starting at the 4 inch pitch end the first move would be G01 X4.0 A360. followed by X5.35 A480. then X6.7167 A600. then X8.1000 A720. etc, etc until 5 inch pitch is reached.


This gives ten lines of varying pitch code and two lines for the ends to give a total of twelve lines for a single pass. Which is why I say it is manageable.

Stepping over and down to generate the 1.5 inch radius from the 3/4 inch ball nose would take more lines but I also think this is manageable because you are working on a Haas and these moves are in Y and Z.

All the screw cutting moves (incidentally you call it a scroll but it isn't) would be in a subroutine which would be called after moving Y and Z to the appropriate position. For instance the first pass could probably be done at full depth exactly on center. If the Z offset was placed to put the center of the ballnose at the OD of the work with the Y offset on the centerline the first subroutine call would be:

G00 Y0. Z-1.125 M97 P1000

Each Y Z position would have to be calculated using a bit of trig. Probably twelve passes each side of the centerline would generate an acceptable profile so this would only need six calculations. Actually I would plot the locations in the simple little sketching program I use and just read off the location of the center of the ballnose for each pass so I wouldn't do any trig.


I think this would work and I don't think it would be at all easy to see that it was a ten segment approximation rather than a constantly varying pitch.

[pbd1971]

Thanks for the reply Geof, I am sure you are quite right in stating its not a scroll. I just started work at a new place and they refer to these components as scrolls so I guess its rubbed off on me.

I have to explain to you I have just returned to G Code programming after 7 lazy years on a CAM system so still very rusty with anything but simple code but its all coming back slowly.

I have been thinking along similar lines to what you wrote. The main thing is the ends are right and because of that, we can of course generate a series of fixed sections of pitch, gradually increasing between the 2 ends rather than a constant acceleration. I am sure a constant acceleration would just be thousands of times smaller moves to what you suggest anyway. Also we wouldn’t have to worry too much about creating a perfect radius for the bottle, the examples I have seen have been quite rough to say the least.

One thing that had me slightly confused is why would we move in Y and Z instead of X and Z during the stepping over and down but the more I think about it the more I am starting to visualise it, stepping in Y will increase the length in X too.

Yes a sketch for the ball nose positions sound like a good idea to begin with and as my confidence and skill develops over time, I will attempt a stepping parametric program using variable programming for the stepping so I can in future generate code for different components on the similar theme. That’s for the future though, got to learn to walk before I can run.

ps. It is a very interesting challenge and I have to say, I am sure I will get a great deal of satisfaction if I am able do create a G code program to make these components.

Thanks

[HuFlungDung]

I think Geof has outlined a decent method.

Rather than using a ballnose tool, I'd be tempted to use a tool with the proper diameter to machine the radius of the screw flute. To do this, you'd offset the tool on the Y axis so that you machined along the side of the part with the OD of the cutter. You can then control the depth of cut for succeeding passes with simple changes in Y. You could also step down in Z if your tool or setup lacked rigidity to do full chordal depth of cut.

[Geof]

Originally Posted by pbd1971 ....One thing that had me slightly confused is why would we move in Y and Z instead of X and Z during the stepping over and down but the more I think about it the more I am starting to visualise it, stepping in Y will increase the length in X too.....Thanks

So you should be confused. I was also, the steps should be in X of course.

HuFlungDung's suggestion to mill along the side would probably work very well on acetal because it is so easy to machine. Also this would automatically generate a profile that would be correct for a cylinder sitting at ninety degrees to the axis of the screw. And even if a cutter smaller than the bottle diameter was used I think there would be fewer steps needed to get an acceptable profile.

[Kiwi]

Here is a VB program that may be of some help.

[BigNizzy]

Normally I try and Cylindrically map anything I have to do around diameters.

I do a lot of double helix jobs were a helix goes in 2 opposotite directions creating a point. I write a simple macro taking the tool height as my radius and working it all out from there.

[Kiwi]

Here is a another VB program that may be of some help.

[pbd1971]

Thanks everyone for the replies, all very helpful.

@Kiwi, thanks for the generators, just having a go with them.........must admit I am not sure how to use them properly (with only just getting back into the "G Code" programming, my minds a little frazzled at the moment.)

@Geof & Hu flung Dung, I think the side cutting option is the one we will be going with. I will probably be using a 2" endmill to produce radii of between 1.25" up to 1.75"

Would I be right in assuming the way to create a bigger radius with a smaller cutter would be to first off, rough out with the cutter on the centre line of the radius and then start the position each successive cut at various points around the arc....say from 3 o'clock back round to 9o'clock........of course I would have to work these start positions out but it should be bog standard trig.

Thanks

[Kiwi]

Originally Posted by pbd1971 ......think the side cutting option is the one we will be going with. I will probably be using a 2" endmill to produce radii of between 1.25" up to 1.75"

You will probably need a flycutter as an end mill may foul the edge of the helix.
See green areas in picture.

[HuFlungDung]

Maybe you could rig up some extra large endmills by running a helical cut HSS slabbing mill on a short arbor. Just a thought, but interpolating with a smaller tool will probably work ok, too.

Kiwi, considering that some sort of bottle or cylindrical container is going to be moved along by this screw, I don't think the shape of the helical flute matters all that much, and an endmill should automatically generate the correct clearance, however it looks when machined.

[Geof]

I realised I had screwed up on the math in my first post so I looked at it a bit deeper; like about four hours deeper. You don't need fancy cutters and you don't need trig, just a long end mill practically any diameter.

My program is in the text file and my bottle screw is in the pictures. The faceting from using 10 degree increments is easy to see but not very noticeable to touch. You can see the increase in pitch by the flat on the crest of the thread.

I did it in two cuts because I thought a single cut would be too much. However the second tool actually had to do a full depth cut during the little bit right at the end and it was fine so one long cutter would work.

The running time was about 30 minutes. Obviously my screw is not 24 inches, the length is 8 inches and the bottle diameter is 1.2 inches. My Delrin bottle fits perfectly and as Hu mentions, and I mentioned in an earlier post, doing the milling from the side does generate the correct profile.

I uploaded the pictures in reverse order.