Best / proper machining method to make this part

eac67gt

eac67gt

Registered
Registered
I have been helping my son make these laser focus knobs and we have always had some minor issues maching them. Below is pictures of a couple of the parts. Two of then have 1/8" slots where the other has 3/16" slots. How I make these is starting on the lathe with trueing them up and drilling the center hole. Then I take the chuck with the part off the lathe and mount it on the rotary table on the mill. Here is where the problems begin especially with the 1/8" end mill. The knob with the not open end slots tends to build up with to much material and either binds and breaks or wobbles and causes uneven slots. I keep the work well oiled and cleaned out best I can but being the slots are pointing up I have found no easy way to get all the debris out. At least with the open end slot the debris can be pushed out the side periodically.
Being I am fairly new to this I honestly have no idea what I am doing. What would be the best way to go about this? I may have not given enough info so just ask and I will try to fill in the holes.

Thanks!

Ed
 
Have you ever considered using a ID pin vise or expanding mandrel to hold the part?

It sounds like you mill from the side how about boring down from the top with a 2 fluted carbide end mill. You may want to design a pin point air nozzle combination Trico type mister made from a 1/8 steel tube to blow air/coolant directly at the cut or from below if your milling from the side. I am also thinking you may want to design a indexing cam fixture or a index plate with hardened pin and bushings. so you can index the part instead of turning a rotary table. I think some of the other guys in your last post mentioned an EDM machine too. Or keep an eye open for a small Brothers CNC Mill Drill.
 
Hi Richard King!
Thanks for your reply. I mill the slots out of the squared off round stock vertically on the mill. I use the rotary table so I can get my slots all at 60 degrees. When I am done milling the slots I take the lathe chuck back off the rotary table and mount it back to the lathe and then turn the face down to a 45 degree angle.

No I have not tried either of the things you asked about in the first question but then I am not totally sure what they are because I am so new to this but they do sound self explanatory.

I am using the 2 flute bit.

I kind of thought about the mister but wasn't sure what kind of issues I would get into with mess. I didn't know how much fluid comes out in that mist and there is no pan under my son's mini-mill.

This is all great input and I will consider all of them. As I said I am real new to this and am quickly learning but there is a lot to learn. I worked as a electronics technician for Honeywell for 30 years until I became disabled.
Helping my son is my way of keeping busy.

Thanks for your help.
Ed
 
It sounds like your setup is exactly what I'd use...

I tend to think you're running your mill too slow cutting those slots. Also, don't try to take the full depth in one pass. No more than 1 mill diameter at a time.

If you need 1/8 slots, don't use a 1/8" mill. Choose 1/32" smaller, make your slots, then go back and clean up the sides. You might even have better luck plunging the ends out first then going back and opening up the center.

In any case, you need to keep the cutter free of chips else they'll get drawn back into the cutter and make a mess of things. I use compressed air, but that's controversial for safety and "chips getting where they don't belong" reasons. If you use it, make sure you're wearing safely goggles (not glasses).

Let us see a photo of the end mill you're using... Maybe a fast spiral mill would work better for you.

John
 
... Didn't read the other posts so I hope I'm repeating what others said...

I'd make the pointy part on the lathe and bore it there too.

Make a mandrel of some sort to fixture it in a vertical mill. Find the center and use DRO to calculate coordinates for the desired number of holes/slots. Plunge cut with 2 flute carbide of the desired thickness to make the holes. Once the holes are bored, fixture it an indexer of some sort, drop the endmill back into a hole and pull the table straight out in either the X or Y direction.

If you don't have DRO, you could manually calculate the coordinates or, if you have a rotary table, you could use that instead.


Ray
 
Aluminum likes coolant, mainly because it's "sticky" and the chips like to weld together when things get hot. A shop vac works pretty well for clearing chips, but those slots are so narrow that it may not be enough. It may depend on the direction of cutting. For example, if you are cutting from the outside in, then (because the part is tapered) it would tend to throw the chips clear, and you can nab them with a shop vac.

The best bet would be a fogbuster type of setup, which gives you a bit of coolant, and an air blast which clears chips. You can build a reasonable facsimile. Mine cost about $80 in parts, and works great.
 
Ed,

First of all, what alloy of aluminum are you using? Alloys such as 6061 and 2024 machine well, but some alloys, such as 6063 don't machine well at all. When you machine the slots, either the open ones or the closed ones, use the end mill like a drill and plunge cut most of the material out, then you can finish the slot to size by side milling. As was already mentioned, you'll need to use an end mill slightly smaller than the finished width of the slot, or if you can live with it make your slots slightly wider to accommodate the 1/8" and 3'16" end mills. Also, you'll get a nicer finish if you climb mill around the slot once it's roughed out. Coolant will also help, use either a mist coolant or just squirt on some WD-40. That stuff works great on aluminum. I would recommend sticking with HSS ends mills for this job. Carbide is great, but if you are having trouble with chips plugging the end mill, a carbide end mill has zero flex and will break.

Tom
 
Sorry I have not been answering questions or updating anything I have been deathly ill. Get back to the topic soon.
Thanks,

Ed
 
You must log in or register to reply here.
Back
Top