Spot drilling/chip dragging

[fpworks]

Does anybody have any techniques to eliminate chip sticking/dragging during spot drilling gummy aluminum? (produces scratches around holes)

I almost always use 12mm Minimaster with 90 degree spot inserts for all my spot drilling and chamfering. I've tried the following parameters(all have a 3 revolution dwell at bottom)

1500 rpm @ 5 ipm
1500 rpm @ 12 ipm
6000 rpm @ 10 ipm
6000 rpm @ 45 ipm

The results for all the above are exactly the same, with the exception of speed, of course. The last is my favorite.

I have also tried pecking, but same results.

Normally, this isn't a problem since the scratches are light enough to be removed by the etching process before anodizing. However, I have a part that cannot be anodized and requires a cosmetic machined finish, and has a lot of little holes with required edge chamfers. Obviously, I cannot have these little scraches around the holes.

I hope to be able to spot/chamfer in one shot, then drill, and be done. (rather spot, drill, then chamfer)

Any advice on this matter is appreciated.

Justin

[Chris64]

Just an idea...can you put down a layer of masking tape and drill through it?

[Geof]

Use a spot drill no bigger than the drill (if possible), spot drill only to the drill diameter, then lift the spot drill slightly and interpolate the chamfer using G03. During the interpolation the spot drill is doing only an intermittent cut so the chips are not as long and do not get stuck and carried around with the tool so much.

[fpworks]

Chris,
I never thought of the masking tape...it should protect the surface. I am concerned that the coolant might attack the adhesive and it might come off. But worth a try.

Geof,
Glad you mentioned the spot drill size...I suspect the tool as the main problem. I am using a 12mm diameter spotting insert, and the holes are only 3.0mm, and the spot diameter is 3.4mm.

The 12mm/90 degree spot Minimaster insert is a fairly heavy duty spotting tool. It has a very thick web and very little relief on the cutting edges, which could be holding in the heat and causing the chips to stick. It may be oversized for this application. I am hoping that somebody else can recommend a tool that they have had success with.

I normally interpolate chamfers, but I've never considered interpolating a spot/chamfer. I would guess that the quality of the spot could be compromised here. ?

[Geof]

Originally Posted by fpworks Glad you mentioned the spot drill size...I suspect the tool as the main problem. I am using a 12mm diameter spotting insert, and the holes are only 3.0mm, and the spot diameter is 3.4mm......I normally interpolate chamfers, but I've never considered interpolating a spot/chamfer. I would guess that the quality of the spot could be compromised here. ?

Stop suspecting; the web on your spot drill is a large fraction of the hole size. We use plain ordinary carbide 90 degree spot drills for spotting and chamferin. You should be able to do you spot and chamfer with a 1/4 one; run rpm as fast as you can go but keep the ipm lowish at around 10. The spot should not be affected but if it is by a burr being thrown into toward the center during the chamfer interpolation just reverse the sequence and do the chamfer first.

[big_mak]

Guehring makes some really nice countesinks, extremely free cutting.

We do cosmetic aluminum parts all day. We also use an OSG solid carbide 6 flute countersink as a chamfermill/countersink tool. These are great and don't generally cause chips/swarf to marr the finished surfaces.

[big_mak]

MA Ford makes some 3 flute solid carbide drills that don't require spot drilling. They work a hot damn. I've used the 1/8" verison 15000 RPM and 3000mm\min.

[pp-TG]

Originally Posted by fpworks Does anybody have any techniques to eliminate chip sticking/dragging during spot drilling gummy aluminum? (produces scratches around holes) I almost always use 12mm Minimaster with 90 degree spot inserts for all my spot drilling and chamfering. I've tried the following parameters(all have a 3 revolution dwell at bottom) 1500 rpm @ 5 ipm 1500 rpm @ 12 ipm 6000 rpm @ 10 ipm 6000 rpm @ 45 ipm The results for all the above are exactly the same, with the exception of speed, of course. The last is my favorite. I have also tried pecking, but same results. Normally, this isn't a problem since the scratches are light enough to be removed by the etching process before anodizing. However, I have a part that cannot be anodized and requires a cosmetic machined finish, and has a lot of little holes with required edge chamfers. Obviously, I cannot have these little scraches around the holes. I hope to be able to spot/chamfer in one shot, then drill, and be done. (rather spot, drill, then chamfer) Any advice on this matter is appreciated. Justin

I also do a lot of spot drilling in aluminum with a cosmetic machined finish i use a 1/8" carbide Drill mill and use a G3 for the chamfering.... The drill mill has a very sharp edge and brakes the chips very well....

[fpworks]

Thanks for all the advice. I did not mention that I have to do this on ~12,000 holes, so my goal is to combine the spot and chamfer in one shot without scratching the surrounding surface before drilling. I really hope to do this without any follow up operation such as an interpolation or a countersink for the sake of efficiency.

The only thing keeping me from doing this succesfully is the scratches. I think Geof is pointing in the right direction to simply use a smaller tool. I may also be able to spot/drill before facing the material, but I've never had good luck interrupting a face mill cut. (expect finishing problems)

I like big maks idea, but I'm not crazy about switching drill brands, since the current ones are giving me consistent hole tolerances better than 0.0003" total, as long as I keep the bits new and holes shallow. I also be using these holes for locating for subsequent operations without reaming. (Guhring parabolic flute)

I'll order some tools today so I can start this job next week. I'll post a follow up.

Justin

[dertsap]

Originally Posted by fpworks . I may also be able to spot/drill before facing the material, but I've never had good luck interrupting a face mill cut. (expect finishing problems) Justin

the facing tool will push a burr into the countersink , if you don t want a lot of hand work ,i would suggest not doing that
hss spot drills are dirt cheap
bump up your coolant comsentrate

[fpworks]

Originally Posted by dertsap the facing tool will push a burr into the countersink , if you don t want a lot of hand work ,i would suggest not doing that hss spot drills are dirt cheap bump up your coolant comsentrate

The chip/burr from that occurrence is held on really weak and can be broken off with an air blast. (as long as you take a light finish pass) My concern is how the face mill will [sometimes] tear the surface when it passes over each hole.

[ctate2000]

12,000 holes!!!! Buy a three flute cardide in diameter equal to dia of chamfer. Have it ground to drilled hole dia leaving and include the chamfer where drill dia terminates. Forget spot driling and drill entire shape in one pass. Three or four drils should be all you need in AL. The three flute drill leaves a round hole and you get the chamfer for free. Three flute carbide should not have any issues starting and drilling straight with out spotting. If you want the ultimate buy a burnish drill with pcd inserts brazed on and you can do it with one tool and hold excellent finish and size. Reid Tool can manufacture the tool. Should cost $250 or so. Not bad $ per hole. You will be able to spin it at highest RPM avaiable.