Option 1: Lollipop Cutter, Option 2: Custom Sine Plate Fixture

I have a one off aluminum part approx 12" x 40" 4". Its one in a set of several but they are all different and this is the only one with this particular issue.
Notice the overhanging part of the radius. This is just a quick representative model of the problem feature for clarity.
The others parts I have done with a 1" carbide ball. All good. Now that this one is roughed out I set it to the side until I come up with a finishing plan.
Option 1: Order a spherical or lollipop cutter.
Pros-
-No complex fixturing,
-faster setup,
Cons-
-I am Having slight trouble with HSMWorks getting the exact tool path I want (but can prob get there),
-expensive(ish) cutter,
-need ~4" reach so need carbide, and bigger than 1" wasn't coming up on first searches.

Option 2: Laser cut and weld up sine plate fixture for positioning about 20deg angle.
Pros-
-Simple reliable toolpath with existing tooling
Cons
-Cost in money and time of fabbing/designing one time fixture
-More complicated setup but I did leave two pin holes in remaining stock, so could use tooling balls for indicating.

Altered option 2:
I feel comfortable designing some laser cut plates with interlocking tabs and welding together. For the tolerances needed on this part I can rely on the lasered angle being accurate enough. But also I have no experience with real SINE bars. Would a few of these be a better choice than a one time fixture?
1x11" Sine Bar
I'm not taking too many heavy cuts now that it's mostly roughed, but I worry about rigidity if th setup is too hacked together.
Thanks for any push int he right direction you can give.

Hi vmipacman:
You wrote:
"I am Having slight trouble with HSMWorks getting the exact tool path I want"

Have you tried running a 3D contour toolpath on that undercut?
Give it a go...I've had good success using it with lollipop cutters for undercuts.
You don't even need to spend the cash for the cutter yet...program it first and see if you like the look of the simulation.
If it doesn't do it for you, you can still spend the time and the bucks to build a big sine plate, or better yet, a pair.

But if I had my way on that job, I wouldn't want to tilt it up if I could avoid it.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Assuming no 4th is available...........
My first instinct because it is a one-off, was sine bars. With lots of stops & clamps to keep the part stationary.
But, I really kind of like your idea of a simple weldment fixture.

implmex said:

Hi vmipacman:
You wrote:
"I am Having slight trouble with HSMWorks getting the exact tool path I want"

Have you tried running a 3D contour toolpath on that undercut?
Give it a go...I've had good success using it with lollipop cutters for undercuts.
You don't even need to spend the cash for the cutter yet...program it first and see if you like the look of the simulation.
If it doesn't do it for you, you can still spend the time and the bucks to build a big sine plate, or better yet, a pair.

But if I had my way on that job, I wouldn't want to tilt it up if I could avoid it.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

Click to expand...

3D Contour was the only toolpath I could get to undercut. My go to for that shape would be FLOW but it doesn't make use of the lollipop, treats it like a 1" ball tool best I can tell. I was thinking of isolating that curve becasaue maybe some other features in the model are messing it up. I'll play with it more, but if 3D CONTOUR is the only one that can make use of the undercut tooling then that makes a difference.

wheelieking71 said:

Assuming no 4th is available...........
My first instinct because it is a one-off, was sine bars. With lots of stops & clamps to keep the part stationary.
But, I really kind of like your idea of a simple weldment fixture.

Click to expand...

Fourth is a possibility, but all that would buy me is precise angle adjustment. I’d still need to rig a fixture plate and tail stock, and I’d want to tie it to the table since 40” is a long span to go unsupported.

I would be inclined to go the lollipop rout. Assuming you can get an acceptable tool path it's going to be quicker and easier then setting up a sine plate.

As for the lollipop I've always had them ground as specials. One thing to look out for is whether the grinder is able to grind a correct spherical shape. I would run the lollipop along a piece of stock leaving min clearance to the shank and check the radius cut with a radius gage to see how accurate it is. Also run the end thru a piece of stock and make sure the end is a perfect ball shape. Quite often their not.

Hi triumph406:
You bring up an excellent point, and one that doesn't get talked about often enough in my opinion.
We often talk a good game about how accurate our work is, while not acknowledging how critical the contribution of those who make the cutters is.

So to the OP; is there a form tolerance for the surface, or is "close enough good enough"?
Must it be visually perfect or does it go somewhere that no one will ever see it, and nothing matters within 0.005".
Definitely on a piece this big, you want to mill everything in one setup...I doubt you'll ever get a good match if you even change cutters during the finishing, never mind re-fixturing the part.

So as Triumph remarked, I'd be aware of how good, or not my cutter is, and I'd try to mill everything in one shot if I can.
In a perverse way, that argues for tipping the job and using a sine plate (or any other method actually...so long as you KNOW the angle of tilt, you don't actually care what it is...you can tip your CAM model the same amount and have at 'er.)

You could buy a heavy plate. split it diagonally on the bandsaw, bolt the halves on the mill table with the wedges standing up, surface mill both angled faces in one go and have an accurate inclined surface to bolt the job to that would be rigid as hell compared to something fabricated .
You could place a couple more intermediate wedges if the two on the ends don't feel like they'd be enough.

I say this about the better accuracy of a ball cutter because I presume the motions the cutter grinder has to make are simpler for the ball cutter, and so far as I can tell, involve presenting only one face of the diamond wheel to the developing cutter for a ball cutter.
I'm speculating wildly here...in fact I've never even seen a ball cutter or a lollipop being ground on a CNC cutter grinder.

Maybe Carbide Bob will chime in and set the record straight on that subject.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

implmex said:

Hi triumph406:
You bring up an excellent point, and one that doesn't get talked about often enough in my opinion.
We often talk a good game about how accurate our work is, while not acknowledging how critical the contribution of those who make the cutters is.

Click to expand...

I worked at one company that had a requirement that before final contouring the ball endmill to be used had to be run thru a piece of Ren shape, and the resulting shape had to be checked with radius gages, or on a comparator.

If I'm contouring a part with a tight surface tolerance I use Dapra insert cutters. So far their the most accurate I've found. Also as the shank has a smaller diameter than the insert you can use them for mild undercuts. Although not enough for the OP's part.

On the other hand I machine a lot of highly 3D contoured decorative parts, where there is no tolerance, they get contoured with whatever ball end mill is in the ATC.

Why wouldnt you use 3 vises with whatever angle machined in matching jaws..
The drawing looks as if the back is a flat surface with a parallel face if so its a 2-3 hour setup

cmccull166 said:

Why wouldnt you use 3 vises with whatever angle machined in matching jaws..
The drawing looks as if the back is a flat surface with a parallel face if so its a 2-3 hour setup

Click to expand...

There’s only one flat surface, the bottom. My graphic is just representative of the undercut feature.
Sadly, I don’t think vises are the answer

Hi cmccull166:
I can't figure how you propose to tip the job up 20 degrees in three vises to get at that undercut with a ballcutter.
The high end is up over 4" in the air at 20 degrees, so it's going to involve some goofy looking jaws that I'm not sure will have much holding power at such a big angle.
Unless there's something I'm not seeing in your plan??

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

implmex said:

Hi triumph406:

We often talk a good game about how accurate our work is, while not acknowledging how critical the contribution of those who make the cutters is.
Marcus

Click to expand...

Nobody cares.
The assumption in CAD/CAM is that all cutters are made sub-micron accurate and no mounting run out during the grind.
Bob

I've used lollipops several times to get out of a jam like that.

Lollipops are not super common. Ive used router bits meant for wood on aluminum and plastic with great results, as long as your not too agressive. The ones from Lee valley work great. I made shrink fit extensions for them to get the length I need.

May want to also just look into a custom lollipop cutter. Contact AB Tools with a drawing and have them quote you. Might be relatively reasonable and then you could get exactly what you want with the clearance and length that you need.

mmurray70 said:

Lollipops are not super common.

Click to expand...

Huh? Yes they are.

CarbideBob said:

Nobody cares.
The assumption in CAD/CAM is that all cutters are made sub-micron accurate and no mounting run out during the grind.
Bob

Click to expand...

C'mon Bob!!

Yes, "we" likely don't care in the programming stage, but most of us (I ass-u-me) are inspecting our parts..

OP, is there something like gouge check in your surfacing parameters? Sometimes in MCX I've had to turn this off to get what I want.

@Mtndew, I agree in general about the lollipop endmills, but a quick search doesn't come up with much over 1/2".

Mtndew said:

Huh? Yes they are.

Click to expand...

Please enlighten me. Where can you get a good deal on a 1" lollipop? Only place I could find was Harvey tool, and they want $600 for it. Not cheap.

Lee valley has a 1" lollipop carbide router bit for $50 and they work fine on softer materials. Original poster is only cutting aluminum. Just thought I would share in case it helps some people. I've used them several times with great results.

mmurray70 said:

Please enlighten me. Where can you get a good deal on a 1" lollipop? Only place I could find was Harvey tool, and they want $600 for it. Not cheap.

Lee valley has a 1" lollipop carbide router bit for $50 and they work fine on softer materials. Original poster is only cutting aluminum. Just thought I would share in case it helps some people. I've used them several times with great results.

Click to expand...

You don't need a 1" lollipop to cut that surface, A 1/2" will work with a 3d surface cut.

The undercut is such that with a 1" sphere, I can access it with a .675 shank. This is because of the amount of undercut. The reach out of the tool holder is like 3" to stay clear of the top stock too. I think I would not go smaller than say 5/8" shank. My first thought was to increase the ball size, thus allowing me to increase the shank. But my CAM gacks at a ball bigger than 1-1/8". Plus, the bigger the ball the more flute engagement I will get, thus increasing the need for a larger shank. It all goes around in circles.

I decided to tilt the part. I have fixturing on the way and will snap a picture when I get it setup. I get to use the tooling I know and a sturdy setup. It's a pain, but not as much as scrapping this part would be. After looking at the lollipop option a few different ways, its literally less work to tilt it, even with the one off fixturing.

Hi vmipacman:
What sort of fixturing did you buy?
If it's sine bars like you showed in your first post, how will you tie the job to the sine bars and the sine bars to the table?
Did you consider the idea of wedge shaped sacrificial plates that you can just mill to the correct angle once you've bolted them to the machine table? (as I broached in post #7)

What's super attractive about doing it that way as opposed to a sine plate or sine bars is two key things:
1) It's really really rigid compared to the flimsy floppy "balance it on sine bars propped up at one end with gauge blocks" approach.
You also don't have to screw around aligning the sine bars...you're going to mill the reference surface in place so it'll be as accurate as the mill is accurate, and you get it for no extra effort

2) It's super easy to put Mitee Bites all the way around the periphery of the parts...you can drill and tap them into place anywhere you want them.
To support the center of the parts, make four equally spaced wedges instead of just two, all 3D surface milled on the angle you want, after you've bolted them on the machine table, then cover each surface with a strip of double sided carpet tape, then drop your block in place and then engage the Mitee Bites around the edges.
The carpet tape will hold the center enough to keep the block from vibrating.
In fact, if your finishing cuts are modest, I bet you could get away with just the tape and ignore the Mitee Bites completely, but personally I'm not that brave.

Your job will be rock solid for the cost of two 3" x 6" x 12" aluminum blocks split on the diagonal and bolted down.
You can reach all of the top surfaces of the job in one go, you don't have to shift clamps around, and when it's time to take it all apart again, you can unbolt the wedges from the mill table, flip the job and knock them free individually from the carpet tape with a big rubber hammer.
Of course you have to bolt them to the table in such a way as to be able to un-bolt them again with the workpiece still stuck on top of them, but it's not hard to figure out how to do that.
Since you're going to mill the precision reference surface after all the sawn wedges are bolted down and not move them until you pull off the finished job, you can just mill in a few slots and bolt them down with strap clamps, so you can reach in and undo them after you're done.
If you bolt right through them, you'll be screwed if the carpet tape sticks really well and you can't break the bond without wrecking the part.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining