[cbryeaw]

I am creating an enclosure for an electric vehicle charger (OpenEVSE), and it is my first time using a Tormach. I am creating holes for a display, button, wire grommets, and circuit board mounting in a Hammond aluminum enclosure. It is between 2 and 4mm thick. For the larger areas I am cutting out, I was planning on buying a 0.25" 2 flute HSS uncoated square end mill from Enco. Then run it at 4000rpm, 16in/min feed rate. Does this sound reasonable?

Also there are some through holes I need to drill. They are for 4/40 aluminum fasteners. This ends up being I think right about 3mm diameter holes. It doesn't look like Enco or McMaster-Carr have metric Drill Mills. Any suggestions for doing these? Should I just get a 1/16" Drill Mill and then use a drill press with a 3mm bit to make the holes larger?

Thanks for any advice, I want to make sure I am ordering mills that make sense and my experience is lacking.

Dan

[WOTDesigns]

You don't need a mill /drill. A regular drill bit works on the mill same as a drill press. A mill drill is for spot drilling, chamfering and milling down to a 45* chamfer.

EDIT : look for correct size drill in stub length so u don't need to spot. I run 2-56 all the time by the thousands without spot

Brian
WOT Designs

[WOTDesigns]

Can't help on mm feed without converting and I never use HSS anyways

Brian
WOT Designs

[SCzEngrgGroup]

Both Enco and McMaster certainly do sell both Imperial and Metric drill bits but it really doesn't matter. For screw holes, even if you're tapping them, the size does not have to be terribly precise. A 3mm drill is the same size as 1/8" drill, within a few thou. Your Tormach is perfectly capable of drilling holes using either bit.

Your feeds and speeds for the 1/4" endmill are at least in the ballpark, depending on the exact aluminum alloy. You will likely need coolant, to prevent clogging and welding, as those enclosures often are made with a soft, gummy alloy. If you get chips welding to the tool, DO NOT increase RPM, or reduce feed. If anything, do just the opposite, to increase the chipload. Use a short endmill to reduce flex, and ideally a carbide endmill, for added stiffness, though HSS will work just fine on that thin material.

Regards,
Ray L.

[kirk_wallace]

Off hand, from my limited experience, for milling enclosure openings a .25" HSS 2-flute sounds fine, but I would tend to use 2000 RPM. Some cast or extruded aluminum materials can be gummy, so brushing or spraying cutting fluid on the tool while cutting may help keep the cutter from loading up.

For drilling holes in the mill, I usually use a spot drill to to make a dimple to start each hole, then use a drill chuck with a drill bit in a tool holder to drill the dimpled holes. Finishing with a counter-sink in a tool holder to break the edge or deburr the holes is good too. Often I'll just put a counter-sink bit in a hand drill, set it to slow RPM and deburr the holes by hand. I also use drill pecking to keep the chips short and keep the hole clear while drilling. Long or small holes tend to have the chips bind up in the hole which can break the bit or make a rough finish. Pecking helps prevent this.

[kirk_wallace]

I forgot to mention that I tend to use the short split point screw machine drill bits with the mill. Drill Set, 115 Piece Screw Machine Length HSS 2827 - LittleMachineShop.com I haven't found an especially good source for these. I usually get just the small number of bits I need from McMaster-Carr. See "High-Speed Steel Short-Length Drill Bits" here: McMaster-Carr

[kstrauss]

Your profile doesn't give your location but from your mention of Enco I assume that you are in the US or Canada. If so I think that you will save money and frustration by forgetting metric and using number size drills. Assuming that by "4/40" you mean "4-40", I usually use a #32 drill for a close fit or #29 for a sloppy fit. As others have mentioned, using screw-machine length drills will mean that you probably don't need to spot the holes.

[cbryeaw]

Thanks everyone for the great info!

[UniqueMachining]

Your profile doesn't give your location but from your mention of Enco I assume that you are in the US or Canada. If so I think that you will save money and frustration by forgetting metric and using number size drills. Assuming that by "4/40" you mean "4-40", I usually use a #32 drill for a close fit or #29 for a sloppy fit. As others have mentioned, using screw-machine length drills will mean that you probably don't need to spot the holes.

I think there is a typo on the numbered drill sizes. A # 29 would typically be used for 8-32. A # 43 would typically be used for 4-40.

John

[kstrauss]

I think there is a typo on the numbered drill sizes. A # 29 would typically be used for 8-32. A # 43 would typically be used for 4-40.

John

Yes, a #43 will give about 75% thread for a #4-40 screw and a #29 is correct for an #8-32 screw. However, the original poster was contemplating using a 3mm drill (0.118 inch) which is about right for a clearance hole but is far too large for a tap drill since the OD of a #4 screw is only 0.114. In an effort to answer the original query the drills that I mentioned were for close and sloppy clearance rather than tapping. I apologize for the confusion!

I'm about 60 miles east of Toronto. Where in Canada are you?

[UniqueMachining]

Yes, a #43 will give about 75% thread for a #4-40 screw and a #29 is correct for an #8-32 screw. However, the original poster was contemplating using a 3mm drill (0.118 inch) which is about right for a clearance hole but is far too large for a tap drill since the OD of a #4 screw is only 0.114. In an effort to answer the original query the drills that I mentioned were for close and sloppy clearance rather than tapping. I apologize for the confusion!

I'm about 60 miles east of Toronto. Where in Canada are you?

Should have picked up on that.

I'm 40 minutes north of Toronto in Holland Landing (Just north of Newmarket).
If you are ever in the area feel free to pop in.

John

[davidbaeley]

I can suggest you can try to use oilfield drilling tools and equipments.