.005 radii on a .270 dia

I'm trying to put two little .005" radii on a .270 diameter part. No matter what I try it will not work. I only program at the machine with the conversationaly programming. I am using a .04 wide groove tool with sharp corners. Here is a program I thought would work but it doesn't. I don't know why the picture is sideways. Its perfect everywhere else.

Probably because your groove tool doesn't have sharp corners. Did you look at it on a comparator? My experience is they usually have .006/.008 radius from the mfg.

What he said.

Also you cannot have ANY run-out. Also zero deflection from pressure. When you do actually have sharp* corners, the feed needs to be about 15% of the corner radius for a decent finish. Sooo with a zero radius corner, that's way slower than .0005".

*There's no such thing as zero radius.

R

Hey Rob, is that "feed 15% of radius" thing for real? I had never heard it before. So a CNMG431 should be programmed at about 0.0025 ipr? Seems a bit light, but I do like the idea of the feed being some percentage of the cutting tool radius. I'll have to experiment with it.

wmpy said:

Hey Rob, is that "feed 15% of radius" thing for real? I had never heard it before. So a CNMG431 should be programmed at about 0.0025 ipr? Seems a bit light, but I do like the idea of the feed being some percentage of the cutting tool radius. I'll have to experiment with it.

Click to expand...

Yes but radius to be cut. Otherwise you sort of "thread" it and it won't be a nice radius.
A .005 rad is easy to skip over in one or two revs so you never see a radius produced.
Stop/dwell or in position check before the rad is not a bad idea also as servo lag and acc/dec can mess with small features like this.

Mostly I suspect the cutting tool has a .006 rad on it so a .005 call without cutter comp pulls it away leaving a sharp corner.
Change that to .011 and see what happens.
Bob

what is the rad of your groove tool you didnt state it, nor did you state the rad of the part you made.

also how come you have the .050 Rads programmed with a g1? and not with a g03 like the other edge breaks your starting point of the 0.050R should be .170 NOT .160
Im having trouble visualizing this part by your program. it doesnt look right

CarbideBob said:

Yes but radius to be cut. Otherwise you sort of "thread" it and it won't be a nice radius.
A .005 rad is easy to skip over in one or two revs so you never see a radius produced.
Stop/dwell or in position check before the rad is not a bad idea also as servo lag and acc/dec can mess with small features like this
Bob

Click to expand...

exactly
we feed .0001-.0005 on all our stuff with .007 or less rads

Your code had me curious is this what your trying to created?
I plugged the Dims and came up with this.
if thats the cause you need to rough out all corners,leaving .001 max stock on the walls , then feed in and dwell at each fillet.
also if you have any rad over .005 on your tool you will have to trig it out or cam it out because if your groove tool has a bigger than 0 rad you cant use a rad of .005 to make a .005 rad. for example if you have a .005 rad on the tool and you want a .005 break on the edge you will need to have a .010 rad in your program.
Now if this isnt what your part looks like your program is 100% wrong.

.
conversational have a hard time using other than corner breaks where the dias are less than what rad you need to generate, you need to use the arc section in them if yours has one.

wmpy said:

Hey Rob, is that "feed 15% of radius" thing for real? I had never heard it before. So a CNMG431 should be programmed at about 0.0025 ipr? Seems a bit light, but I do like the idea of the feed being some percentage of the cutting tool radius. I'll have to experiment with it.

Click to expand...

Generally accepted for Finish cuts. But there are loads of variables too.

R