Crazy Slot

[Colin Gilchrist]

Ok, so I just got a sweet part dropped in my lap. 48" diameter OD. It is a fan assembly with some of the craziest features I've ever encountered.

 

The part is 17-4 SS. It has been roughed and finished turned, and now it has been passed on to me.

 

There are 4 slots, 1.028-1.038 wide, with full a full radius of .200 at either end. So .400 wide, by 1.033 wide, by.... wait for it... 18" deep.

 

So looks like the max width tool I could fit into the slot would be .375 diameter. This is a 48:1, depth to diameter ratio.

 

Any ideas on a method to cut this in 17-4 SS? My first thought is to try and have the top and bottom holes gun drilled. Then come in with a .375 Feed Mill. I am thinking about using the replaceable heads (Iscar? Kennametal?), and having a custom Tool Steel shank made that is about 21" long. That would give me three inches in the holder, but still. It is going to be hanging out like a wet noodle...

 

I was thinking Sinker EDM, but who would have a tank that can go 48" deep, and still have around 20" of Z travel?

 

It isn't just 1 slot either, it is 4 slots. And... to top it all off... the icing on the cake... is that we've got about .09 wall thickness on either side.

 

God help me...

 

:-)

[Leigh @ Kodiak]

Have fun with that...

 

Sorry I don't have anything more to offer, but I think you are on the right track with the feed mill, but still...

[GoetzInd]

No chance of milling that. Start research sinker EDM vendor. EDM's that big are defiantly out there although not in every mold shop on the block.

 

Mike

[jlw™]

Oh snap! Good luck brother.

[taperlength]

I'd be talking to the engineer who designed it.  If the slots are there just to lighten it up, they might be amenable to replacing each slot with a few holes, which could be gundrilled.

[MIL-TFP-41]

Yikes. Tho a creative EDM place could do it on a machine that has 18" of travel in Y. Just have to burn sideways. un-submerged. sounds like a fvcking mess.

 

so yea...gundrill out the ends, and sounds like you have room to fit a 3rd hole between the other 2. Then maybe rough down as far as you can. Then sinker time. 5"-6" deep with a 3/8 tool is really pushing it, especially in 17-4. 18" deep...Yikes again.

[Colin Gilchrist]

No chance at a redesign. This is already a highly engineered component. Every hole, every radius, everything; is important. Although the features are difficult to machine, they aren't technically impossible. This wasn't designed by some wet behind the ears engineer either. It is from a major jet engine manufacturer.

 

Looks like this is going to a vendor for Gun Drilling and EDM. I've got enough other really difficult features to worry about. How about a 1.67 diameter back counter bore, with only .95 diameter "clearance" hole. (There is an angled flange that intersects the angled hole, and prevents a normal tool from being used.) So I've got enough to worry about without the gun drilled holes, or crazy slots. The rest of the part itself will be challenging enough. My guess is 40-50K worth of custom tooling to get these "almost impossible" features cut. There is one place where I will need to come up with some kind of "drill jig" that can be mounted to the part, and we'll use a hand-drill with an aircraft extension drill to get to the hole. I can't reach it with a Right Angle Head, the clearance is just too great. I absolutely hate the idea of doing anything on the part "by hand", but I just don't see another way to get the hole and still hit the true position callout. I think we'll put these holes in manually (just the hole itself), then come back with a lollipop cutter and do the chamfers. I'm not about to scrap a part because a .02 chamfer is over size, and this hole has a chamfer on both sides.

[jlw™]

Ashton Kutcher is gonna jump out and yell "YOU JUST GOT PUNK'D!" any minute.

[Sticky]

Is it through or blind?

 

I'd gun drill the corners and as much of the center as possible, then attack it with several different lengths of feed mills.

 

Chip thinning is your friend, you'll need it with such a huge tool engagement angle. Internal corrected feed is Nominal feed * (minor diameter- cutter diameter) / minor diameter.

 

I've done 30:1 milling in 15-5 on a 40 taper, maintaining the proper chip thinning for the engaged angle is the trick. But at 48:1...D@mn

 

IMO the L:D ratio isn't as much of a problem as your proposed tool engagement.

 

If I could find some sucker to edm that part and accept all the associated liability I'd deliver that sh!t myself!

[Mic6]

Can you plunge mill it out?

[Guest]

ECM Machining?

[SpacePilotPro]

My first thought was also sink EDM. I am glad that isn't on my to do list...maybe let us know how you pulled it off...?

[Matthew Hajicek - Singularity]

 

 

Yikes. Tho a creative EDM place could do it on a machine that has 18" of travel in Y. Just have to burn sideways. un-submerged. sounds like a fvcking mess.

 

What he said.  Stick a solid electrode on a WEDM and plunge in X or Y.

[bd41612]

No chance at a redesign. This is already a highly engineered component. Every hole, every radius, everything; is important. Although the features are difficult to machine, they aren't technically impossible. This wasn't designed by some wet behind the ears engineer either. It is from a major jet engine manufacturer.

 

Looks like this is going to a vendor for Gun Drilling and EDM. I've got enough other really difficult features to worry about. How about a 1.67 diameter back counter bore, with only .95 diameter "clearance" hole. (There is an angled flange that intersects the angled hole, and prevents a normal tool from being used.) So I've got enough to worry about without the gun drilled holes, or crazy slots. The rest of the part itself will be challenging enough. My guess is 40-50K worth of custom tooling to get these "almost impossible" features cut. There is one place where I will need to come up with some kind of "drill jig" that can be mounted to the part, and we'll use a hand-drill with an aircraft extension drill to get to the hole. I can't reach it with a Right Angle Head, the clearance is just too great. I absolutely hate the idea of doing anything on the part "by hand", but I just don't see another way to get the hole and still hit the true position callout. I think we'll put these holes in manually (just the hole itself), then come back with a lollipop cutter and do the chamfers. I'm not about to scrap a part because a .02 chamfer is over size, and this hole has a chamfer on both sides.

 

http://www.steinertechnologies.com/automatic_back_spotfacer

 

I bet that the .95 clearance won't be an issue.  This is what these guys specialize in.

[?Mark]

I'm with Mike on this one...don't even dare put an endmill on this one...ouch

edm only imo

[Del.]

http://www.steinertechnologies.com/automatic_back_spotfacer

 

I bet that the .95 clearance won't be an issue.  This is what these guys specialize in.

Thats cool.

[Newbeeee™]

No chance at a redesign. This is already a highly engineered component. Every hole, every radius, everything; is important. Although the features are difficult to machine, they aren't technically impossible. This wasn't designed by some wet behind the ears engineer either. It is from a major jet engine manufacturer.

 

Looks like this is going to a vendor for Gun Drilling and EDM. I've got enough other really difficult features to worry about. How about a 1.67 diameter back counter bore, with only .95 diameter "clearance" hole. (There is an angled flange that intersects the angled hole, and prevents a normal tool from being used.) So I've got enough to worry about without the gun drilled holes, or crazy slots. The rest of the part itself will be challenging enough. My guess is 40-50K worth of custom tooling to get these "almost impossible" features cut. There is one place where I will need to come up with some kind of "drill jig" that can be mounted to the part, and we'll use a hand-drill with an aircraft extension drill to get to the hole. I can't reach it with a Right Angle Head, the clearance is just too great. I absolutely hate the idea of doing anything on the part "by hand", but I just don't see another way to get the hole and still hit the true position callout. I think we'll put these holes in manually (just the hole itself), then come back with a lollipop cutter and do the chamfers. I'm not about to scrap a part because a .02 chamfer is over size, and this hole has a chamfer on both sides.

Times like today when the stresses of post writing pale into insignificance...

I definitely wouldn't try to cut - I wouldn't even attempt that dia to depth in aluminium!

+1 to the flyout spotface tools.

+1 to a localised drill jig. I wouldn't be frightened of going this route but I would ensure the job/route/planning card had a separate operation on it so it didn't get missed. 

All the best with this Colin.

[Colin Gilchrist]

Is it through or blind?

 

I'd gun drill the corners and as much of the center as possible, then attack it with several different lengths of feed mills.

 

Chip thinning is your friend, you'll need it with such a huge tool engagement angle. Internal corrected feed is Nominal feed * (minor diameter- cutter diameter) / minor diameter.

 

I've done 30:1 milling in 15-5 on a 40 taper, maintaining the proper chip thinning for the engaged angle is the trick. But at 48:1...D@mn

 

IMO the L:D ratio isn't as much of a problem as your proposed tool engagement.

 

If I could find some sucker to edm that part and accept all the associated liability I'd deliver that sh!t myself!

 

The slots are "through", because there is a center hole in the hub, but the slot/channel itself is through the part at an angle. So while it is "through", the part on the "backside" makes it hard to position no matter how you cut it.

 

I'd love to use a smaller tool, but any decrease in diameter means an increase in Depth to Diameter ratio. 48:1 is crazy enough. If I went down to a .25 tool, that is 72:1.

 

We are going to send it out to EDM. It is the only reliable way at this point. This part already costs more than my house. I'm not going to be the one to scrap it...

 

 

 

 

Can you plunge mill it out?

 

Perhaps, but oh man, the pucker factor on that would still be crazy high. I do like the idea that all the force would be directed into the spindle. The bad part for us (and the reason we are sending this to EDM) is that we only have a horizontal machine that would even accommodate the size of the part, with the orientation we need. If we used a vertical, we would run out of Z travel, since the part sits up at 50" tall. (actually, about 54" because of the flange orientation on one of the slots)

 

 

ECM Machining?

 

Perhaps, but the biggest issue is still the same issue we face with EDM, namely, that the size of the part is just massive. We need a giant machine to fit the part, and most ECM machines just don't have the working envelope needed.

 

 

My first thought was also sink EDM. I am glad that isn't on my to do list...maybe let us know how you pulled it off...?

 

Oh, its EDM for sure. Trying to machine that slot in any conventional sense would be the stuff of nightmares. Knowing my luck, I'd actually get through the first three slots, and then the tool would wander on the 4th and blow through a wall.

 

 

What he said.  Stick a solid electrode on a WEDM and plunge in X or Y.

 

This is what we are going with. We have a couple vendors with tanks that are big enough, and although they don't have enough Z travel, by feeding in X, we can make it work.

 

 

http://www.steinertechnologies.com/automatic_back_spotfacer

 

I bet that the .95 clearance won't be an issue.  This is what these guys specialize in.

 

These look sweet! Thanks for the link and info. We've used Heule tools in the past, and they work great, but the size of the C-bore diameter to tool body diameter isn't as great as the Steiner tools, so thanks!

 

 

I'm with Mike on this one...don't even dare put an endmill on this one...ouch

edm only imo

 

Agree 100%

 

 

Times like today when the stresses of post writing pale into insignificance...

I definitely wouldn't try to cut - I wouldn't even attempt that dia to depth in aluminium!

+1 to the flyout spotface tools.

+1 to a localised drill jig. I wouldn't be frightened of going this route but I would ensure the job/route/planning card had a separate operation on it so it didn't get missed. 

All the best with this Colin.

 

Yep. "Hey, can you cut this impossible feature in unobtanium? Oh yeah, we can't buy any tools, just use whatever you can find. Make it work!"...  "Oh, and we really need this, like, two weeks ago. So yeah, no pressure or anything. The customer is going to be here tomorrow and they want to see it running on the machine. Any yeah, the block was about $150K before we put a tool to it, so like, don't screw it up or anything..."

[MrFish]

How about plunge milling approach to rough and then edm to finish ?

 

whoops, slow to the party , see it's been suggested

[Matthew Hajicek - Singularity]

Now for your next trick cut it in ceramic!

[specv]

+1000 on the steiner tools, currently using them to cut a 1.500 counterbore and .594 diameter pilot diameter.

[Teh Bear without Brains kinda idiot]

Perhaps, but oh man, the pucker factor on that would still be crazy high. I do like the idea that all the force would be directed into the spindle. The bad part for us (and the reason we are sending this to EDM) is that we only have a horizontal machine that would even accommodate the size of the part, with the orientation we need. If we used a vertical, we would run out of Z travel, since the part sits

~```````~~~~~~~~~~~~~~~~

Can you use angled head 90 degrees ?

[Colin Gilchrist]

Can you use angled head 90 degrees ?

 

Hi Alex,

 

Perhaps, but EDM is really the way to go on this part. There are 8 - .375 through holes, and 4 - .400 x 1.028 slots. So we are going to set the part up in a Gun Drill machine, and we will just Gun Drill 16 - .375 through holes. That will be followed up by sending the part out to EDM those 4 slots.

 

Since the slots will be EDM'ed instead of machining with an end mill, I won't even have to worry about trying to mill these using a Right Angled Head. Instead I just have to worry about some crazy back counter bored holes, and some other fun features. There is enough on this part to do without having to worry about these crazy slots.