1/4" aluminum perf with 1/2" holes

[SugarFox5]

I've got a job coming up where I need to make some perforated panels out of 1/4" aluminum. The perf holes are 1/2" diameter holes and I'm trying to figure out what sort of 1/2" bit I could use to accomplish this. One place that I get bits from recommended that I just use a 1/2" drill bit. Does anyone have experience doing this type of work or any suggestions? A single panel is going to take me 4 hours to cut if I use a 1/2" bit so I really don't want to go smaller than that but I have zero experience with 1/2" bits and aluminum. The only thing I've cut with that size bit is acrylic. Any advice is GREATLY appreciated.

Similar Threads:

• ESS .250" holes measure around .237" but a 1.00" hole comes out closer, around .997"
• Helical 1/2" 3 FLT ZrN Carbide High Perf. End Mill- for Aluminum,Non-Ferrous
• Helical 3/8" 3 FLT ZrN Carbide High Perf. End Mill for Aluminum,Non-Ferrous
• Helical 1/2" 3 FLT ZrN Carbide High Perf. End Mill- for Aluminum,Non-Ferrous
• 6 Pc Helical 1/8" 3FLT ZrN Carbide High Perf. End Mills for Aluminum,Non-Ferrous

[Jim Dawson]

You don't say what machine you are using, but I would use a 1/2 inch, 135° split point, solid carbide, screw machine bit.

[SugarFox5]

I'm using a Multicam 3000 series. Would you have a recommended rpm and plunge rate for such a bit?

[metalfixer]

Another option for clean, burr free holes.
Fractional Rotabroach Cutters

[KH0UJ]

I got a job like that a couple of months back, 4 ft.X 8 ft. plain sheet stainless, I think you can achieve a faster working time making holes on a CNC controlled plasma machine, it took me 16 minutes on putting holes on a whole 4 ft. by 8 ft. plain stainless sheet, 8mm think, aluminum is like a cake on the plasma machine, I guess you can achieve more faster cutting time on it.

[Jim Dawson]

I'm using a Multicam 3000 series. Would you have a recommended rpm and plunge rate for such a bit?

If you have enough spindle HP, I would start out at about 8000 RPM and about 40 IPM. Lots of coolant.

[SugarFox5]

Wow! 16 minutes is awesome. All we have are CNC routers. I'm not sure why my company keeps taking these jobs without bidding them to be subbed out to a plasma or waterjet cutter. It's extremely time consuming and complicated with a router. Thanks for the input!

[SugarFox5]

If you have enough spindle HP, I would start out at about 8000 RPM and about 40 IPM. Lots of coolant.

Thank you, Jim. That's very interesting... the slowest I'm used to running is around 18,000 for plastics and around 21,000 for aluminum. In my research I did find that drill bits should be run at much lower RPMs but I never imagined as slow as 8000. Thanks for the advice. I think I'll order the drill bits today and do a little playing around before all the material gets here. I should be able to cut the holes in a single pass, right? It's only .25" material with a .5" bit. When you say 40 IPM are you talking plunge or feed? I use EnRoute software and you can enter both plunge and feed but only feed is required to create the drill point or tool path. I honestly don't do anything with my plunge rate. It's always at zero in my software and I think the Multicam dictates a default plunge. I've never had any issues... seems to work fine for the materials we generally use but we don't normally do a lot of drilling.

[Jim Dawson]

Yes, feed at 40 IPM. Something like this: G81 Z-0.5 F40.0 At least I think Multicam will do a G81 drill cycle. Drilling does best with a relatively large chip load and lower RPM. Since you are only going 0.5 * dia, you should be able to do it in one pass with a G81, if that doesn't work well, then try peck drilling with a G83.

[KH0UJ]

how big is the material sir? and how many holes? and what size are the holes? I think you can achieve faster speed using the router with 1/8 carbide bit, instead of drilling the whole hole might as well as cut the hole in the router using a small bit, higher RPM spindle, with small depth increment, I can cut aluminum shape in minutes too using only cooking oil mixed with kerosene as coolant, smells like french fries by the way hehe

[SugarFox5]

Yes, feed at 40 IPM. Something like this: G81 Z-0.5 F40.0 At least I think Multicam will do a G81 drill cycle. Drilling does best with a relatively large chip load and lower RPM. Since you are only going 0.5 * dia, you should be able to do it in one pass with a G81, if that doesn't work well, then try peck drilling with a G83.

Thanks, Jim. I don't know any G-Code but I just looked up G81 and I understand what you're saying. My software does all the code for me so I just enter my depths, feeds and speeds and use the software to dictate drill points or tool paths. What do you think of this bit?
Morse Cutting Tools

[SugarFox5]

how big is the material sir? and how many holes? and what size are the holes? I think you can achieve faster speed using the router with 1/8 carbide bit, instead of drilling the whole hole might as well as cut the hole in the router using a small bit, higher RPM spindle, with small depth increment, I can cut aluminum shape in minutes too using only cooking oil mixed with kerosene as coolant, smells like french fries by the way hehe

I'm actually a woman ... name is Angela. The panels I need to cut are 27"x76". I can fit two on a 4'x8' sheet of 1/4" aluminum. The panels are completely perforated so there are probably hundreds of holes in each panel; holes are 1/2" diameter. The software is telling me that if I use a 1/4" bit to cut the holes in two passes it will take 9.75 hours to cut whereas using a 1/2" bit with one pass will knock two hours off that time. There are some tool changes in there for cutting partial holes around the perimeter because they want a solid border on the perf. I can run the machine faster with a smaller bit but the multiple passes and the fact that the tool is circling around the hole make the overall program slower. If I run an 1/8" bit I would need to make twice the passes I would with a 1/4" bit so that would add even more time. That's if I'm understanding your comment properly .

[SugarFox5]

This is the other bit I'm looking at. It's quite a bit cheaper. Thoughts?
https://drillsandcutters.com/1-2-car...drill-america/

[Jim Dawson]

The bit style is correct, but the ALTIN (ALuminium TItanium Nitride) coating is going to be an issue. The aluminum will instantly weld to the bit. I would use an uncoated bit or a TiN coated bit.

I should have asked how accurate these holes need to be. Drilling is generally considered a non-precision metal removal method, and the burr on the back of the hole is going to require a secondary operation to remove. So another option would be to use a 3/8 or 7/16, 2 or 3 flute, solid carbide, aluminum cuttinig end mill and do a spiral lead-in and a finish pass. Still about 8000-10000 RPM, and around 40 IPM

I have a customer that does a lot of 1/2 and 5/8 holes in 1/4 inch aluminum with a Multicam router, and he is using 3/8 end mills and circular interpolation. Holes are pretty accurate, and almost burr free. He is using end mills from M.A. Ford, but end mills from any quality vendor should work.

[Jim Dawson]

This is the other bit I'm looking at. It's quite a bit cheaper. Thoughts?
https://drillsandcutters.com/1-2-car...drill-america/

I don't know anything about the company or quality, but it is the correct bit.

[ger21]

You might want to check with Multicam to see if they recommend drilling 1/2" holes with that spindle.

I'd maybe drill a 3/8" hole, then clean them up with a 1/4" or 3/8" router bit, so the backside will be cleaner.

[SugarFox5]

I don't know anything about the company or quality, but it is the correct bit.

I was wondering about the coating on the other bit being a problem. I think I'll order one of these and try it out. These panels will be painted after cutting so there will be some sanding that needs to be done anyway. Our biggest concern is just getting these cut and off the table quickly. How rough a finish are we talking about? Should regular paint prep take care of it? The client want's 1/2" holes but it's all for aesthetics so they don't need to be real accurate. I use end mills almost exclusively so I have experience with them... the new method of using a 1/2" drill bit came about because I'm trying to cut down on machine time. Thanks again for all your advice!

[SugarFox5]

You might want to check with Multicam to see if they recommend drilling 1/2" holes with that spindle.

I'd maybe drill a 3/8" hole, then clean them up with a 1/4" or 3/8" router bit, so the backside will be cleaner.

Thanks for the input. Why would 1/2" holes be an issue? I use 1/2" bits for acrylic all the time but this is my first attempt using a bit that size in aluminum. As long as my speeds and feeds are good, I'm not sure why there would be a problem punching 1/2" holes in 1/4" aluminum. The issue is that we are against an extremely tight deadline and they haven't even gotten me the material yet. I often have to get creative with my cutting due to rush jobs with new materials and demands. Can you give me any detail as to why you think it may be too hard on the spindle?

[ger21]

Router spindles are not really designed for drilling. But I don't know what kind of spindle you have, so it may be fine.

[Jim Dawson]

I was wondering about the coating on the other bit being a problem. I think I'll order one of these and try it out. These panels will be painted after cutting so there will be some sanding that needs to be done anyway. Our biggest concern is just getting these cut and off the table quickly. How rough a finish are we talking about? Should regular paint prep take care of it? The client want's 1/2" holes but it's all for aesthetics so they don't need to be real accurate. I use end mills almost exclusively so I have experience with them... the new method of using a 1/2" drill bit came about because I'm trying to cut down on machine time. Thanks again for all your advice!

The finish of the hole should be good, but the burr on the back is a bit of an unknown at this point. It really depends on how gummy the aluminum is. Lowering the feed rate at the breakthrough point might be helpful in this regard. That would require some creative CAM manipulation, I don't know of any canned cycle that would do that automatically, maybe a G73 or G83 could be adjusted to do that. Not sure if Multicam will accept a G73 drill cycle. Since all of the actual drilling cycles is the same for all holes, you could put that in a subroutine and just hand write it with G1 moves to do what you want. EnRoute is a PITA to make it do non standard things.