View Full Version : Machining or Routing a Radius

08-07-2005, 12:30 PM
What would be the smart efficient way to accurately and consistently place a 1/8” radius on all 4 sides of 3/8” thick by 4” wide by 10'-0” long lengths of aluminum flat stock. I don't need aerospace quality accuracy but it definitely needs to be perfect visually.


08-07-2005, 12:43 PM
try building a jig and using a router using a bit with a follower bearing on the end.

good luck.

[This message has been edited by tattoomike68 (edited 08-07-2005).]

08-07-2005, 12:47 PM

Mike Burdick
08-07-2005, 01:04 PM
Since it’s aluminum I’d just get a carbide router bit with a ball bearing guide and put that in the mill or router.

Paul Alciatore
08-07-2005, 03:19 PM
Yes, since it is aluminum I would consider using a router with a ball bearing rounding cutter. I would also set up my router table with some guides so I could do the job faster and easier. I would use a rip fence along with the bb guide on the cutter and a couple of feather boards, one on top and one opposite the cutter to hold the stock against the fence and table. Set up in about 30 minutes (15 if your router table is not buried under a 8' high pile like mine is) and about 10 minutes to do the cut.

[This message has been edited by Paul Alciatore (edited 08-07-2005).]

08-08-2005, 09:24 AM
If you opt for the router method, (which I use ocassionaly) be careful of chip weld. It will create a poor finish. I climb the edge I am routing to eliminate this. Would not advise climbing on a router table though.

09-02-2005, 10:39 PM
I bought a couple carbide corner rounding end mills with a 3/16” shank and 1/16” radius, similar in looks to the one posted above. It works perfect with a glass like machined radius on a aluminum rectangle. The only problem now is how do I indicate (if that's the proper terminology) the bit in the Z direction and the X,Y direction to keep from cutting “to deep” into the plane or surface and to make a consistent radius around all 12 sides of a rectangle?


Paul Alciatore
09-03-2005, 02:05 AM
I've never tried it but the router and router table thing sounds tempting. I think I might try to add a coolant spray to keep the chips from building up on the cutter.

I did put rounded corners on a project a couple of years ago using one of the corner rounding milling cutters pictured above. My parts had fairly consistent dimensions so I set up the vise on the milling machine to use the fixed, rear jaw as my outside edge and I used a couple of 1-2-3 blocks and a straight piece of flat ground stock to align the top edge. I put one block on each side of the vise and the straight stock above it (about 1/2"). I then mounted the work in the vise with the tip against the straight stock and tightened. I pulled the blocks and straight stock off and set up the first edge carefully. It is easy to go too deep or too far into the workpiece so setting up on a piece of scrap is a good idea. Once you have the proper set-up, it is easy to mount the workpiece with each edge up in turn to round it. Just use the blocks and straight stock. If it is just for appearance, you can stop a few thousanths shy of a perfect radius and no one will ever know.

Paul A.

09-03-2005, 01:33 PM

Do this all the time using a rounding tool like machinist suggested.

The trick, as others have suggested, is not to overcut the top or side. What I do is offset the center of the radius by .005” to .010” towards the two intersecting planes that are being cut. What you give up in doing this is that the tangent points are just shy of the theoretical 90 degree points but, on visual inspection is not noticeable.

Here is a link to a drawing of a part that I make all the time and shows how the radius edges of the part are dimensioned to show you what I mean:


Hope this helps.


09-03-2005, 02:39 PM
Thanks for the suggestions,

Man, it's extremely time consuming, especially doing all 12 sides. I have a ton of them to do and being a novice to machining doesn’t help matters.

I wonder if CNCing the radii on the perimeters is possible? I have a Taig on order but that will be a new adventure as well.


How do you accomplish the offset scenario you mentioned? Meaning setting up the tool bit in relationship to the part to keep from cutting to deep? BTW, I've never even used an edge finder but I'm more than willing to learn. Keep in mind that I’m a novice?


[This message has been edited by Smokedaddy (edited 09-03-2005).]

09-03-2005, 05:33 PM

First, let me say that I do this part on a CNC, so the initial profile (the L shape) has some of the rounded corners taken care of by the endmill and the remaining edges are done with the rounding tool – it takes two setups to do this part. On the CNC, I index all the tools to a fixed location and adjust them, relative to where the part is sitting, with a Z offset adjustment setting. But for the doing this manually, the end result you are trying to achieve is the same and I will try to explain in terms of a manual machine setup.

First, for a 1/8” radius, the corner rounding tool is designated as a CR4-3. The cutter portion of this tool has an OD of 5/8” in an ID of 1/4”. You will see that the (OD-ID)/2 is 3/16” and not 1/8”; there is an extra 1/16” extended from tangent point of the upper portion of the radius to the OD. If you have the Machinery’s Handbook, or something like it, there will be diagrams and dimensions for corner rounding tools you can refer to.

For indexing the tool to one of the sides and, lets assume you are doing one of the setups that does one side of the 4” x 10” rectangle (4 edges to cut), you will need to use an edge finder for locating at least two edge of your material; one along the X axis and one along the Y axis. If the material dimensions are accurate, you can use math and crank your handles to locate the tool for cutting the other two edges on the X & Y axis edges or, just use your center finder again for the two other edges.

To locate the tool to the edge, first locate the edge of your material with your edge finder. Now replace your edge finder with your rounding tool – the center of the tool is now sitting over the edge of your material. Now you need to locate the correct location of the center of the tool out from the edge of your material. Remember the 1/4” ID mentioned above, that is the amount, plus a few thousands for an overcut margin, that you want to crank your handle to position the tool away from the edge of the material. Remember this position on the appropriate handle so you can return to this location after setting the Z height position.

For indexing the tool to the top of the part, the Z height, you want to use the extra 1/16” portion of the tool that was mentioned above and bring the tool down to just above the top of your part. To be safe, as you bring the tool down, make sure the OD of the tool clears the edge of the material - as you start to get close to the top of the material, crank your tool in to where you are within that 1/16” portion; this is usually easy enough to eyeball. Now you need to crank down the tool to where it is sitting a few thousands above the top of your material. Several ways to do this; if your eyeballs are good, you can place some white paper behind the tool and see the gap to set; and, another method is to use a shim (aluminum foil folded to suited thickness) can be placed on the material and lower the tool until just touching the shim. Also remember this location on your Z handle; you will use this position for all edges you cut on this setup. Now return your X or Y position to the correct handle setting from above.

Now you have your tool indexed to one side of our rectangle. Make the cut along that axis and, as mentioned above, to do the other parallel edge, crank the appropriate handle over by the amount of your material dimension plus 1/2” (two 1/4" ID’s) plus two of the dimension you are using for overcut margin – cut the other edge. Repeat the above procedure for locating the edge on the other axis. Not to complicate things, but when you locate the edge of one axis you might as well locate the edge of the other axis – this will save you some time in tool changing – just remember all the locations so you can easily come back to them.

You can start a new thread on how to use an edge finder or, search the archives – there are a lot of good people on this board willing to help – don’t be shy about your questions.

Anyway, this is one way of doing it and I hope I was clear. Shout if you have questions.


09-03-2005, 08:52 PM

Here's my radius tool:


Just for clarification, the original posting stated a .125 radius but I ended up buying a .0625 radius tool due to hold down problems.

I searched the BBS and found several threads on using an edge finder. I still can’t believe how time consuming it is to accomplish this task … at least for me. Thanks for taking the time to explain your setup it’s appreciated.