Rounding Over Part Edges on a CNC
From contributor J:
Do you have a tool changer? You could do the cutting and drilling and still hand round over the part. If you want to do this on your CNC, you would most likely have to use tabs to hold the piece in place until after you round over it.
From contributor I:
If the price is right, you can buy (or have made up) a combination downcutter with roundover.
From contributor V:
You might try setting up an MDF jig with some bolts to hold down the parts that have been cut with square edges (in the bolt holes that have been cut on the machine). Then take a regular, hand-held round-over bit and remove the bearing and grind off the center pin where the bearing was. Use an offset tool path for the outside of the part (careful measurement or trial and error) to get the proper distance and depth for your roundover. Once you have the jig and the roundover program, you can run the parts quickly. Set up a spot on the machine with some stops or pins, so the jig can be removed and replaced in the same spot each time.
From contributor J:
I think it still would be faster to just use a hand held router or a router table to do these. The cleanup and reloading would take longer than the routing.
From contributor V:
It depends on your setup. If you're doing a lot of these, and you have a tool-changer and a big enough table, you can be loading the round-over jig(s) on one side of the table while the part cycle is cutting. While you are unloading the parts and cleaning up, the round-over program is running for finished parts.
Once this is set up, the parameters would be known for round-overs on other parts, and the tool would be available; this could come in handy in the future.
From contributor W:
If the material thickness varies, it's not going to come out correctly. You need to do all the operations on the CNC. First you need to take the blank, surface it to the finished thickness, do all your cut outs, then round over.
From contributor D:
Yes, you can do a roundover on a CNC. Onsrud makes some tooling that will allow this, but it is material width dependant.
We do a fair amount of work that requires a 1/4 radius on the edges and have found that it is more cost effective to have the CNC operator do it manually on a router table while waiting for the next parts to be machined.
We don't have a toolchanger. If we did, I'm not sure we'd do any different. Feed rates for a radius profile bit are significantly lower than for a chipbreaker compression bit, 0.006 chip load compared to 0.025 or so. It'd take 3 or 4 times as long to radius the edges than to machine out the part itself.
From the original questioner:
I do have a tool changer. I'm thinking the only tool that would take advantage of the CNC would be a combination cutting and roundover bit? The customer is already set up to do the roundover manually, he just wondered if I could do it on my machine while still on the spoilboard. He doesn't want to pay me to do the same thing he's capable of doing. I'm cutting these in 6 sheet lots for him, 6 parts to a sheet of 3/4" plywood and 36 parts to a sheet of 1/2" (different size and shaped parts but one each required per chair). I think I'll tell him that on this first batch, he'll have to do the roundover himself, which is what our original agreement was, and I'll do some research on a combination bit and maybe have it figured out by the time he is ready for a second run.
Contributor D, what feed rate would you use for the combination bit? Also, since this piece will be upholstered and not visible, a little variance in the material thickness would not be a concern. Just need an eased edge to pull the foam and fabric over.
Contributor M, your idea is what I was hoping to be able to do, just haven't seen any bits other than the insert bits. Thanks for the input, everyone.
From contributor D:
Based on my experience (you should check with a tool supplier), I'd guess 0.006 chip load, so for 18,000 RPM that'd be 216 IPM.
From contributor S:
Onsrud has a number 40-50 series Round & Rout bit with a 1/4" CE rad and up to 1-11/16" CEL. At 18,000 RPM the recommended rate is 180 IPM for soft plywood. I think it would run faster, but you would have to experiment.
From contributor H:
We can help you with that, but it would be custom if you want downshear on the roundover. We do have some standard roundovers also that roundover and trim the edge at the same time.
From contributor T:
Be sure to check the overall length of the tool. If it's 3/4" material, you need the roundover plus the straight section to be .75 plus whatever you use to get through the part (.010). If it's longer, you will cut deeper into the spoilboard. Might want to use a dedicated one for these parts. We had custom inserts made to just get through the part.
From contributor N:
You can cut out and round over at the same time with a standard plunging round over bit from Amana, white side.
From contributor E:
He says he has a tool changer. I wouldn't over think this for the few sheets he's doing. He can cut these in two passes and get both the round over and his profile cutout using standard bits. When I cut this way I use a standard white-side center cutting round over bit. It has a cutting length of 5/8... 1/2" deep gets you the full round over and a 1/4" groove. Do a tool change and cut the part out. No special tool required. Now if he starts cutting a lot, he needs to look at good tooling.
From contributor K:
I have been down this road. We were cutting parts for Kawasaki third party for a shop that did upholstery. These were seats for their mule line. We needed an eased edge for the part so it wouldn't cut the fabric when wrapped around the piece. I was taking a 3/8 bit and cutting the part, then another pass with a 45 degree bit to ease the edge. It got the job done to keep up with the orders. I went with a company that made me a custom cutter with C4 carbide. It worked but the cutting speed was slow. But remember, the part was done when off the router.
I was in Atlanta and ran across Vortex tooling. They had a stock cutter which they could grind for my application (1/2" plywood). It worked really well, and they are a very knowledgeable company. I ran a lot of dry runs on the router using the tooling company's feet per minute specs, and made decisions from there.
From contributor Z:
I'd recommend a look at Amana tools. I used some recently and was really impressed. The speeds I ran at were much faster than mentioned earlier in this thread. My impression was that they had really improved their tools.
Insert or not is a cost and quantity issue mostly. The insert tool holders are more expensive, but the inserts are less expensive than braised tools. I'd consider cutting the radius first, then tool change and cut the part through.
Would you like to add information to this article?
Interested in writing or submitting an article?
Have a question about this article?
Have you reviewed the related Knowledge Base areas below?