roll die

[HEAVY METAL]

I have not used this opiton in a long time. roll die c-hook. could anyone tell me if I am going about it the right way. what i'm doing is cutting a helix with a 560 deg wrap and .1063 pitch. bottm of helix is .49815 radius. I created the helix like it would look on the part and used this as my chain. Is this right or should i unroll the geo.one problem that i see is my z depth is shallow all I wantt to do is take a ball mill right down center of thread to rough it out.any ideas

Thanks heavy

[Colin Gilchrist]

Hi Heavy,

 

If I remember right, Roll die is for offsetting the endmill so you can cut with the side of the tool. If you just want to stay on center, use the "roll/unroll" options in the contour toolpath. This will let you roll the tool around your rotary axis, with the tool centerline on your geometry...

 

HTH,

[JDowe]

If it is essentially milling a thread

write a contour toolpath and under rotary axis

substitute the Y axis - assuming the part axis

is X - and unroll the path to the diameter -

set contour depth deeper if the thread is shallow

 

I think the purpose of roll die is to align the

OD of the cutter with the ceterline of the part

as opposed to the axis of the cutter aligned with centerline of the part

[HEAVY METAL]

So do i draw a 3d helix or a straight line representing the helix

[HEAVY METAL]

i think im over thinking this i am just going to program this helix at the contol . should be a lot less lines of code

[John Summers]

A layout in the flat is a nice check to make sure you have the right numbers.

560 deg. / 360 deg. = 1.5555 turns.

1.5555 * .1033 = .1654 total X travel.

In the flat, lay out a rectangle X=.1654,

Y=1.5555 * pi * diameter.

The helix is a diagonal line corner to corner (you didn't say right or left hand).

Use the same diameter for axis substitution.

You only need 2 points, the first and last.

[John Summers]

Whoops. Y should simply be the circumference, pi*dia.

I hate to cut with the end of the ball. For this kind of cut, I much prefer to cut, say, 45 degrees from vertical. You can, of course, jimmy up a post, or you can post to BALL CENTER (not to tip), and rotate the two points in the side view.

[John Summers]

So Sorry. I was right the first time. I'm fighting some serious med's. Really.

When you establish a helix in the flat, the basic rectangle is X=pitch, Y=circumference. The helix is the diagonal. Now the X travel is 1.5555 * pitch. The helix angle doesn't change. Just extend it to the total X travel.

[Mic6]

My head just exploded

[John Summers]

Mic6, if you send me an email, I'll send you a picture, well, a part file.

[HEAVY METAL]

I got the code i need by using mastercam and john's method except my post puts out A0 then A200 instead of A560. is this a setting in the control def that needs to be changed

[John Summers]

Yes. But you only need 2 points. You could change the end point by hand. I guess you're going to skip the 45 deg. option. It's really a form of lead/lag machining. The chip making process is much better.

[John Summers]

Sorry, Heavy, I should have metioned that if you change the control def, you would have to change the machine setting, which is apparently 'short way'. Just break the line into 6 pieces or so, and everything should be OK.

[ThRaSH]

John, could this be applied to machining the flutes of a drill or cutter body. Where I work (Spec-Tool) we mill our flutes in a Mazak. Our Mazak's conversational makes it somewhat easy to do this. Just plug in your numbers and go.

 

From what I understand past attempts (at our shop) to program flutes in Mastercam have led to NC code that has a lot of points to mill the helix. MDI at the control results in a lot less code, but drill and cutter body flutes can be big and require multiple passesdepthsoffsets to mill the flute complete. Would rather leave this to Mastercam to figure out.

 

What would be the best way to do this in Mastercam? Roll die? A a contour toolpath like Dowe suggests?

 

Our prints typically will give 4 dimensions for the flutes.

 

1) Total deg wrap - Ex: 560 deg.

2) Flute length - Ex: 7 7/8" long

3) Distance from center to side wall of flute

4) Distance from center to bottom of flute

[HEAVY METAL]

my thread starts at -10 degs how can i force the helix to start at A-10 and finsh at A550 right now it starts at A0 -to B560

[John Summers]

If you unrolled the helix and used axis substitution, you could just translate the helix 10 degrees. You need to be able to convert the 10 degrees into a Y dimension.

Y/(pi*dia) = A/360 sets up the basic proportions. Then Y=A*pi*dia/360

The inverse of this, A=Y*360/(pi*dia) is also useful. If the rolled helix is in the right place, it should land in the right place if you use CW,-90 for unrolling parameters. I'd send you a drawing, but I don't know the part diameter. The advantage of working in the flat is that you can break the helix line into just a few pieces. If the mill is set up for 'short way', each segment must be less than 180 deg.

THRASH, I think I could help you if I had a sketch with all the dimensions. I'd also like to know what cutter you would be using.

[ThRaSH]

 

Sorry I didn't get right back to you, but here is a sketch of a cross-section view of a typical drill flute. The cutters we use to mill the flutes range from .500 to 1.25, but all use the same octagon shaped insert which we make (insert and cutters).

 

Dimensions vary, but from your previous post it looks like your looking for a pitch dimension to plug into your formula? It's possible that could be obtained from our CAD Dept. Really, just wondering what would be the best approach to doing this in Mastercam?

[John Summers]

Thrash,

That drill flute section is unique. Unless I'm really mixed up, it appears that you can cut half the flute from one side (with the cutting edge 'up'), then cut the other half with the non-cutting edge 'up'. It looks like a job for ROLLDIE. The geometry is on centerline, and the distance from side wall to centerline is expressed as XY stock thickness. For all depth cuts, the helical cut would be the same -- in other words, each start position would be a point in the main, followed by a helical cut sub. I need a little help myself, and I'll send you a file when I get this organized.