What's new
What's new

Deburring in a cnc mill tools?

Delw

Stainless
Joined
Jan 8, 2019
My time killer is deburring and I'm trying to cut that down as much as possible. most of out parts have .005 max edge breaks and are aluminum. we can run 45 degree chamfer mills on most of the features. the problem we have is where we have 2-5 ops and there are cut outs from previous ops. what are some options for slots like this?
we been using a small burr tool but its really not small enough to get the inside edge from the outside it works though and there is no room to go from the indside. I just dont want to do 1500-2000 slots every time we get a job like this, it cuts out on me running machines. lots of jobs have slots and holes though the sidewalls with 4-40 sti threads. then we mill the side walls which pushes the burr back in the hole. or slot.
On the 4-40 sti threads I found a 3/16 round burr bit works very well both in the machine and by hand. ( we have no room to get a chamfer tool in there) with the ball your able to hold it at almost angle angle to deburr the back side effectively.

any ideas?

we also tumble all our parts, but the media doesnt touch the slots do to fins close by and on the threaded holes it just pushes a burr back in.


IMG_1453a.jpg

IMG_1451a.jpg
 
I have a couple dozen different double-angle cutters that I use to back-deburr slots and holes. That would be what I would use for your sidewall slot.

For that pocket in the floor that abuts the sidewall, I use a 1/8" chamfer mill (unless the reach is more than maybe 1" then I go to a 1/4"). Put the cut way up near the top of the tool's chamfer. Lead-in perpendicular, then arc around 90* with a tight radius, 5% of the cutter diameter. Shorten the contour just enough to prevent the chamfer mill from hitting the sidewall.

Regards.

Mike
 
My time killer is deburring and I'm trying to cut that down as much as possible. most of out parts have .005 max edge breaks and are aluminum. we can run 45 degree chamfer mills on most of the features. the problem we have is where we have 2-5 ops and there are cut outs from previous ops. what are some options for slots like this?
we been using a small burr tool but its really not small enough to get the inside edge from the outside it works though and there is no room to go from the indside. I just dont want to do 1500-2000 slots every time we get a job like this, it cuts out on me running machines. lots of jobs have slots and holes though the sidewalls with 4-40 sti threads. then we mill the side walls which pushes the burr back in the hole. or slot.
On the 4-40 sti threads I found a 3/16 round burr bit works very well both in the machine and by hand. ( we have no room to get a chamfer tool in there) with the ball your able to hold it at almost angle angle to deburr the back side effectively.

any ideas?

we also tumble all our parts, but the media doesnt touch the slots do to fins close by and on the threaded holes it just pushes a burr back in.


View attachment 300305

View attachment 300306

Looking at the inside where both slots are apparent, in the floor, you can get most of that oval with a chamfer tool. Might have to detail by hand with a Vargas tool.
But in that back slot, if you set that up as in picture #2 you could drop in with a small dove-tail cutter to do an inverted chamfer..looks like you go to that position anyhow.
A non-critical observation, just out of curiosity...
There are a lot of tool marks in that cavity.
You do these by hand, right?
Or are you just going like hell?
 
I have a couple dozen different double-angle cutters that I use to back-deburr slots and holes. That would be what I would use for your sidewall slot.

For that pocket in the floor that abuts the sidewall, I use a 1/8" chamfer mill (unless the reach is more than maybe 1" then I go to a 1/4"). Put the cut way up near the top of the tool's chamfer. Lead-in perpendicular, then arc around 90* with a tight radius, 5% of the cutter diameter. Shorten the contour just enough to prevent the chamfer mill from hitting the sidewall.

Regards.

Mike

Mike
the floor slot is .100 wide, and I didnt even think of starting it right next to the dia of the chamfer tool Good Idea, Kinda feel dumb now cause I do that on one for the counter bores in this part, never even thought for the slot..

on the slot that goes in the "Z" long direction. its cut into a solid block on 1st op(like our parts with the threaded holes), I havent done a time check on it, but was thinking small angle cutter or maybe a key cutter to relieve below the required depth then hit it will a angled cutter. it shouldnt add too much to the program time size thats about a .125 wide slot was more worried about breaking tools

Thanks
 
Looking at the inside where both slots are apparent, in the floor, you can get most of that oval with a chamfer tool. Might have to detail by hand with a Vargas tool.
But in that back slot, if you set that up as in picture #2 you could drop in with a small dove-tail cutter to do an inverted chamfer..looks like you go to that position anyhow.
A non-critical observation, just out of curiosity...
There are a lot of tool marks in that cavity.
You do these by hand, right?
Or are you just going like hell?
we use a vargas tool now takes time thats what were trying to get out of.
read my reply to mike on the other slot.

on the observation, we has a few parts like that. yes going like hell with a small endmill in a fadal, but in defence of being stupid I wasnt paying attention to the tool flex in going fast on a small tool.
 
There are a lot of tool marks in that cavity.
You do these by hand, right?
Or are you just going like hell?

This.

What kind of aluminum is this? If its 6061-T6 you should be able to get edges that don't need deburring, or at least, you would at least have a worthy battle on your hands before having to give up. Did you already do some experiments to figure out what toolpath/speed/tool would give you an edge that doesn't need deburring?

If I saw tool marks in a pocket like that I would assume something isn't right, its a general red flag even if its not the geometry being discussed right now.

If that isn't-right extends to the edges you are having trouble with then it might be time to step back and evaluate your toolpaths, tools, and feeds and speeds. Are the tools dull?

If its MIC-6 or some other O temper good luck I have no advice.
 








 
Back
Top