What's new
What's new

.063 Radius in a long slot

blackwolf4278

Aluminum
Joined
Oct 1, 2020
Hi. I have a question how one would machine a .400 wide by 2.3” long slot that requires a .063” radius in corners while the depth of the slot is 1.4” in Aluminum 6061

I’ve tried many different things and keep getting a very aweful finish in the corners.

Here’s my most recent attempt where the finish cale out much better than before but still not so good.

I drill 4 holes with a .125” endmill, and then cut the slot to finish with a .25” endmill, which obviously leaves some steps around the corner, then i plunge with a .125” endmill(4times in one corner) to get rid of the steps, this way the finish is okay but still not really 😂

Any suggestions?
 

Zeuserdoo

Aluminum
Joined
Aug 31, 2015
Location
The Moridor
When I get a part that calls out a .063 corner radius, I use a 3mm (Ø.118) endmill so that I can "drive" the corners. It prevents corner chatter almost every time.
 

dandrummerman21

Stainless
Joined
Feb 5, 2008
Location
MI, USA
A couple things:

Do as zeuserdoo said above, use a smaller endmill than the radius.

In addition to that, if you have, say, +/- .010 on that radius size, program it bigger, like .068, and use the 1/8 endmill (or 3mm would be even better). The more you can convert it to a circular interpolation, the better your outcome.


The last thing: slap the engineer. It PROBABLY could be changed where the corners were drilled out a bigger size, so your endmill wouldn't even cut the corners. I assume something is fitting inside this slot and they just want to make sure the corners of the "plug" don't interfere with the corners of your pocket. The "plug" probably has a decent chamfer on it too.

Without seeing the part, I obviously can't be certain this idea would fly, but if you had any input on the design, that's something to consider. If you have no input on design, then bummer.
 

michiganbuck

Diamond
Joined
Jun 28, 2012
Location
Mt Clemens, Michigan 48035
Back in the day, we would likely put a radius on a 3 or 4 flute end mill and run the part.
That would be altered on the surface grinder or a TC grinder...or would hand bump a 1/32 rad with the bench grinder, and then put it on the comparator and hand hone the radius to .063.
 

White Lightning

Aluminum
Joined
Jan 21, 2018
Back in the day, we would likely put a radius on a 3 or 4 flute end mill and run the part.
That would be altered on the surface grinder or a TC grinder...or would hand bump a 1/32 rad with the bench grinder, and then put it on the comparator and hand hone the radius to .063.
And another hat is handed out.

12x depth is difficult. Drill it close, possibly plunge with a relieved flute 3mm small step over to reduce chatter. Production guys will laugh, I'm a mold maker so I only get one shot so speed isn't the key.

Sent from my SM-G960U using Tapatalk
 

Shawnrs

Stainless
Joined
Mar 30, 2016
Hi. I have a question how one would machine a .400 wide by 2.3” long slot that requires a .063” radius in corners while the depth of the slot is 1.4” in Aluminum 6061

I’ve tried many different things and keep getting a very aweful finish in the corners.

Here’s my most recent attempt where the finish cale out much better than before but still not so good.

I drill 4 holes with a .125” endmill, and then cut the slot to finish with a .25” endmill, which obviously leaves some steps around the corner, then i plunge with a .125” endmill(4times in one corner) to get rid of the steps, this way the finish is okay but still not really 😂

Any suggestions?

I would punch the designer of this slot.
 

michiganbuck

Diamond
Joined
Jun 28, 2012
Location
Mt Clemens, Michigan 48035
Could be the customer wants no interference at the corner..but .063 seems an odd call.
I could see that (a radius) in steel or CI but not in aluminum.

Re: ? [And another hat is handed out.]
Just offering another method..buying a radius corner end mill is another..a local cutter grinder might provide such as an altered standard ..or even a used altered standard.
 

Milland

Diamond
Joined
Jul 6, 2006
Location
Hillsboro, New Hampshire
Could be the customer wants no interference at the corner..but .063 seems an odd call.
I could see that (a radius) in steel or CI but not in aluminum.

Re: ? [And another hat is handed out.]
Just offering another method..buying a radius corner end mill is another..a local cutter grinder might provide such as an altered standard ..or even a used altered standard.

The OP is asking about an enclosed pocket or slot, you're milling from the top, not the sides. There's no "endmill corner radius" involved, it's all cutter diameter/radius.
 

MCritchley

Hot Rolled
Joined
Mar 22, 2007
Location
Milwaukee
Is the pocket blind or through? If its through send it out for EDM. A 5 axis mill might help you if ones available.
I had to do a similar part not that long ago but with a 6 to 1 depth to dia. It was a pain but worked well once i turned the speed way down. I had some custom cutters make with a relived shank and a dia. .015 smaller than the corner radius.
 








 
Top