PDA

View Full Version : How would I mill this?



cncJim
16-10-2014, 12:58 PM
Hi everyone,

Sorry, this is probably very simple but....
I would like to make a pen holder for my cnc machine - Like this:-

13634

I'm not too bothered about the pen holder really, just want to understand and gain some knowledge of milling techniques involved in creating something like this. I would like to mill this out of aluminium and be as accurate as possible. So if someone could break down the idiot proof steps needed to complete the job I would be very grateful! :)

Im guessing starting with a piece of aluminium like this maybe:-

13635

Thanks for any advice,
Jim

mekanik
16-10-2014, 03:47 PM
Hi Jim
If you are fortunate enough to have a band saw, rough it out leaving a couple of mm green, then setup in your vice and with a pin stuck with blue tack onto your cutter adjust the position of the job in the vice with lead block till you have the pin running horizontal to your marking off, do same with the rest.
Mike

cncJim
16-10-2014, 04:13 PM
Hi Jim
If you are fortunate enough to have a band saw, rough it out leaving a couple of mm green, then setup in your vice and with a pin stuck with blue tack onto your cutter adjust the position of the job in the vice with lead block till you have the pin running horizontal to your marking off, do same with the rest.
Mike

Hi Mike,

I did not even think about roughing it out before even bringing it to the mill! :hopelessness:

Thanks for the tip with the pin - good idea.

What do you mean with "adjust the position of the job in the vice with lead block"?

Thanks again,
Jim

mekanik
16-10-2014, 04:47 PM
Job in vice and nipped, eye ball the marking off so that it as near horizontal by eye, then bring the stick pin upto the marking off adjust height of head or table so sticky pin lines up with marking off @ one end of the job, traverse table to other end and tap the job to remove error, go back and forward till pin indicates job horizontal.
Mike

cncJim
21-10-2014, 10:31 AM
Sorry Mike! did not notice that you had replied to the thread.

Thanks for breaking it down for me, I will hopefully give it a go this weekend.

Cheers,
Jim

corkcnc
21-10-2014, 11:16 PM
Sorry Mike! did not notice that you had replied to the thread.

Thanks for breaking it down for me, I will hopefully give it a go this weekend.

Cheers,
Jim

Hi Jim,

Mikes idea sounds good. However if you already have a cnc I'd start with a block about 5mm thicker than the finished thickness, clamp this in the vice and program in the profile you require. Use a profile left cycle if you have one so that you keep the width of the cuts manageable; to about 30% of the cutter, if not, cut it with G41 / RL cutter comp left and leave a generous finishing allowance,then finish, then do a final spring pass.
Then flip the part, clamp either of the paralell sided pairs with a spacer block extending out past the end of the vice to support the underneath and face off the extra 5mm with a few 2mm passes with a facemill or mill it out with a pocket canned cycle that will cover the whole part.
If your controller is a bit more basic but you have a copy and paste facility, put in the profile using comp left and use a 10mm diameter cutter but tell the machine you have a 20mm cutter in. Then copy and paste a few times and change the cutter diameter to 16,12 and then 10. This will generate 4 paths with the first one cutting a mix of heavy cuts and thin air and the rest will have a nice 2mm width of cut.
For the side with the "internal corner" use an endmill that has a rad a mm less that the sweep radius to avoid chatter and where possible use the full lenght of the cutter.
Just a few basic tips. If you are starting off, get a bar of 6082 T6 ally so you are not worried about it sticking to tool and use a bit of wd40 if the spindle isn't enclosed. Buy a few two flute cutters and just start making chips. Avoid full diameter cuts for the moment till you get an idea of the power of your machine and your ability to evacuate chips.
I won't type anymore cnc stuff incase I confuse things but feel free to pm me if you have any specific questions.
If I got you wrong and you don't have a cnc but are building one, then stick to Mikes idea. For the line up though I like to mark it out, then put a paralell block on the top of the (good) vice and tap the block till the line is spot on the top of the paralell, then bring the quill down (WITH THE SPINDLE OFF :) ) and lightly touch it off the paralell and lock it. Remove paralell and machine using about 30% of the cutter or so. Climb mill it so start on the right with the tool in front of the centerline and cut till the tool is now on the left, then move the tool back behind the part and cut back, keep doing this till all the material is removed. The tool path should look something like a clockwise spiral with straight lines instead of curves.
Best of luck with it.
Noel.