What's new
What's new

Corner Radius End Mills and Soft Jaw Profiles

Hobbes4Pres

Plastic
Joined
Oct 25, 2023
Normally have done wood CNC work so please forgive the basic question with switching to metal. Starting out with metal CNC work at my makerspace and ordering new bits for aluminum 6061 stock. I will be cutting soft jaws as well. General guidance seems to be to purchase a corner radius end mill like this Lakeshore Carbide suggested by NYC CNC. https://www.lakeshorecarbide.com/14variablefluteendmillforaluminumzrn.aspx. I know the radius is not much, 0.003 to 0.005, but will this effect cutting soft jaws since the shoulder wont be completely square? I had planned to mill an XYZ reference area to the fixed soft jaw so not sure if the part to be placed in the jaw will end up lifting slightly.

Thoughts on my options below?
1. Buy corner radius end mills and don't worry about it
2. Buy square end mills. This is hobby use and shouldn't be too worried on tool life.
2. Buy square end mills and corner radius end mills and use accordingly
4. Buy corner radius end mills and one small square end mill to square up the shoulder when needed.
5. Other advice?
 
By "Soft Jaws," do you mean jaws for holding Op2 of your part?

I have very few square end mills in the arsenal; everything has a little corner radius on it (usually, 0.01" minimum). Op1 from raw stock is always cut on some sort of grip jaw - Talon grip jaws, or the serrations on Schunk or Lang vises. Those grip jaws are for square edge stock and the undercut on them deals with most any burrs.

For Op2 - very rarely does one have parts that lack a corner radius or chamfer on the finished surface that will easily allow the 0.01" corner radius on the soft jaw plenty of clearance.

Having said that - if you do have a part where the edge you'll be gripping has no chamfer on it - it probably isn't really a square edge! You will have *some* level of burr, even almost imperceptible. If you think you're going to drop a square edge piece of stock into a square edge soft jaw, you'll be a little shocked because it won't work very well. This is why you see most precision tooling for grinders or other tight work never have a square inside corner, they always have an undercut feature to cut out that section and prevent any contact with the part edge.

So, I would go with the corner radius end mills, but be conscious of everything, model stuff 100% to how you will machine it, and use the section view to really see what will be going on. Do not leave the model de-featured! If an edge will have a corner break on it, model it and drive the tool path with it. Don't rely on edge deburring strategies that chamfer the model in the CAM side for you with tool path until you have a very solid understanding of fundamentals and know what is going on.
 
Buy square end mills. I used radius end mills in tool making where the materials are harder and the chip comes off hotter. Aluminium you need to do some funky shit to chip a corner. I have 3mm radius end mills for 62HRC work and one aluminium job I once made apart from that everything is square unless it's a ball nose.
 
Buy square end mills. I used radius end mills in tool making where the materials are harder and the chip comes off hotter. Aluminium you need to do some funky shit to chip a corner. I have 3mm radius end mills for 62HRC work and one aluminium job I once made apart from that everything is square unless it's a ball nose.

Sure, not a totally illogical notion to just buy square end mills for aluminum. I might argue in favor of a little rad for better floor finishes and yes, even an increase in tool-robustness, but I can see the argument not to bother.

Either way - it's bad practice for someone starting out to think that putting a "square" edge into the "square" bottom of a soft-jaw pocket is a good idea. Might work just fine for home-gamer parts on home-gamer machines, but as soon as you look to step up quality, reliability, cycle-times, etc, it is a practice that will be biting you in the ass. Best to avoid it now instead of having to figure it out down the road.
 
Either way - it's bad practice for someone starting out to think that putting a "square" edge into the "square" bottom of a soft-jaw pocket is a good idea
100% in agreement. My thing about corner rads is I always hated it when I wanted to cut a square cornered pocket and I had to swap out tools. Corner rads are excellent in mould work where you really don't want blending issues swapping between square end mills for flats and ball nose for angled surfaces. Nothing like needlessly blending with a polishing stone to get your blood pressure up.
 
Thanks everyone for the responses. As I noted I'm doing this at my makerspace purely for learning/interest and not related to production work, now or in the future.

@sfriedberg & @gkoenig thank you for your answers and explanation. Yes I was referring to Op2. I model all chamfers and reference the bottom edge chamfer and let F360 do it with the chamfer tool path, with an offset to avoid the point of the tool. I do not set the chamfers manually in the CAM but let the CAD model do the work. I also 3D print to reference while I'm planning my operations and also validate my model before spending the time on the machine and aluminum. Another reason I model everything vs. doing features in the CAM only. The main thing you referenced for me that had slipped my mind is that my parts are already chamfered on the edge during Op1. To your point, when I flip it for Op2 and put it in a soft jaw that radius end mill won't matter which I had forgot about.
 
I always have some sort of sharp corner end mill for cutting soft jaws, If you want to OCD it, you can dovetail/key cut in a relief also.
As the devils advocate for above posts, some parts, especially in the tool and die world CANNOT have rounded edges, they MUST be sharp,
because they mate for shutting of into a single piece without any split line.

This is just one for instance, but I have had non tool and die parts also, where the customer insists on sharp edges for their need also.
If you always want to be covered, just always use a sharp corner end mill for cutting jaws, but also, it actually has to have sharp corners, I have a microscope to pre check any sharp corner endmill I use before cutting jaws with it.
If not I would run a dovetail cutter for a relieve corner.

But on machining I buy radius tooling, even if only .005 rad

But I also have had customers insist on sharp corners on pockets or other features in a part, so there is no blanket statement.
 
You should have a dovetail cutter in your inventory anyway. Sooner or later you will be dovetailing raw stock to hold in dovetailed vise jaws for op 1.
 
By "Soft Jaws," do you mean jaws for holding Op2 of your part?

I have very few square end mills in the arsenal; everything has a little corner radius on it (usually, 0.01" minimum). Op1 from raw stock is always cut on some sort of grip jaw - Talon grip jaws, or the serrations on Schunk or Lang vises. Those grip jaws are for square edge stock and the undercut on them deals with most any burrs.

For Op2 - very rarely does one have parts that lack a corner radius or chamfer on the finished surface that will easily allow the 0.01" corner radius on the soft jaw plenty of clearance.

Having said that - if you do have a part where the edge you'll be gripping has no chamfer on it - it probably isn't really a square edge! You will have *some* level of burr, even almost imperceptible. If you think you're going to drop a square edge piece of stock into a square edge soft jaw, you'll be a little shocked because it won't work very well. This is why you see most precision tooling for grinders or other tight work never have a square inside corner, they always have an undercut feature to cut out that section and prevent any contact with the part edge.

So, I would go with the corner radius end mills, but be conscious of everything, model stuff 100% to how you will machine it, and use the section view to really see what will be going on. Do not leave the model de-featured! If an edge will have a corner break on it, model it and drive the tool path with it. Don't rely on edge deburring strategies that chamfer the model in the CAM side for you with tool path until you have a very solid understanding of fundamentals and know what is going on.
I am the total opposite. I cut mostly aluminum and almost all of my end mills are sharp square corner. 98% of the parts I make have sharp corner edges on pockets. I also have corner radius mills in case a customer wants rounded corners, but it is rare. I cut soft jaws with square end mills. All parts are deburred before they go in the soft jaw. Corner chipping of end mills is not an issue if you’re running aluminum. Tooling lasts forever basically.

This guy should buy square if he’s doing aluminum and corner break/radius if he’s doing harder material imo.
 
How do you make stuff without lots of tooling I don’t understand you are in the game or not
Don
 

Attachments

  • IMG_0959.jpeg
    IMG_0959.jpeg
    2.9 MB · Views: 32
  • 61983611361__DAAD766C-B7AB-47A0-BDCF-59163C9AB859.jpeg
    61983611361__DAAD766C-B7AB-47A0-BDCF-59163C9AB859.jpeg
    1.7 MB · Views: 32
You should have a dovetail cutter in your inventory anyway. Sooner or later you will be dovetailing raw stock to hold in dovetailed vise jaws for op 1.
Thanks. I ended up going with small radius end mills and picked up a 1/4” back chamfer bit from Harvey. Will probably add dovetails in the future.
 
Crap! I've been doin' it all wrong for 40 years. Oh well.............. Hey if it works for ya, do it.
Hahaha, But, I have seen people been machining for close to 30 years and they were doing something incorrectly, you can do it wrong a long time.
Just because you've been doin it long doesn't mean you been doin it right, not how that works.
Seen plenty of older dudes (like me)doin stupid shit, intellect isn't for everyone.
 
It is entirely dependent on the part that you're holding on to.
Does it have a decent chamfer/radius that is smaller than the radius on the end mill? The area of the part that makes contact with the soft jaws needs to have a larger edge break than the end mill has.

Notice I said end mill and not "bit". :D
 
.003 corner rad on a .250 carbide endmill.
LOL.
Up sharp carbide end mills do not and never will make "zero" corners.
All nice in the computer. Not real world.
This is why the good Lord came up with undercuts or backtapers.
 
Last edited:








 
Back
Top