Rounding edges on plaque

[applik]

I read some older posts on using roundover bits but didn't find much on actually making the SB do it. I have the oval carved and cut out with tabs holding it. Can I run another file on the same vector used to cut it out but use a 1/2" roundover bit on it? I don't have a router table so thought maybe I could get the bot to do it. Time isn't the issue here, just getting it done with what tools I have available (the bot). I have AC Pro and ran a couple of toolpath simulations with the roundover in the tool directory. Looks ok but not sure what I need to do mechanically. Can the roundover bit plunge down into the wood ok? Any ideas on feed rate and stepdown?

If it won't work, I'll just have to have a square edge. I'm waaay to new at this to know what to try next, but I'm experimenting and learning a LOT!

You folks are a wealth of knowledge. Much better than manuals.
Thanks,
Shari

[richards]

Shari,
You could let the Shopbot do it, exactly as you've described, but watch the Z-height carefully. On the round-over cutters that I use, there seems to be little room between too little and too much depth.

It is much easier to do that on a router table. Why not use your Shopbot to cut out a router table for you. Right now Woodcraft has the PC-690 router on sale for $109.00, so your total investment, figuring 1/2-sheet of MDF would be around $125.

[harryball]

I fiddled with this idea too... I have a very nice router table setup with a router lift and Incra system. I still don't enjoy standing there rounding 42 plaques when I could be painting or some such. The way I see it, the plaques are already on the table and this is what the bot is for.

Cutting the round over first, then cutting out the profile might be a better approach, haven't tried it yet but for my next batch that's my plan.

Mike is right about the z-height. I finally just ran the depth down and left a profile line instead of trying for a round edge with no profile line.

There must be a round over bit without a profile edge that feathers out for use on CNC machines... at least you'd think there was.

Robert

[waynelocke]

It is a different look, but, if you use a 90º bit for the lettering, you can bevel the edges with the same bit and setup.
Wayne

[andyb]

I've used Wayne sugestion several time using a 90 or a 60 degree bit, just depended on what bit I was using at the time. They both came out looking good.

Andy B.

[joewino]

This question is similar to what is being discussed here.

Many of my dimensional signs are produced with a half inch cove around the outside edge. Can that cove be routed using a ball end bit that follows the vector line of the shape of the panel and then do a profile cut using the same vector line. In other words, can the center of the bit follow the vector line so that half of the "ball" is on the inside of the vector and the other half is on the outside?

[mikejohn]

Yes

[jhicks]

Ray and Shari, we have accomplished both techniques as well as V edges. Hybrids also make sense sometimes like a v border offset inside maybe 1/2" then a v or Roundover border on the outside edge to frame and edge the piece.
The basic approach is as one might logically assume but to confirm here is our method.
1) Round over edges. we use a 1/2" round over from Magnate who makes several unique plunge bits for the legacy ornamental Mill. The bit has a 1/2" round over profile with a 1/4" plunge tip between the 2 round over sides.
We run the profile in 2 passes. 1st pass at about .325 to .350 deep, the 2nd pass to .485 (under .500" so we don't get any cuts too deep and create an edge marks on top of the piece)
Once this is complete, we cut along the same ouside vector profile with a 1/4" end mill all the way through in one pass by setting our bit depth per pass at .76" since we have already removed the .485" from that area.
2) Cove cut out edges. This technique is essentially the same as the round over except rather than cutting the ball nose on the "outside profile" one would cut "on the vector" to end up with the desired radius after cutting it out. 2nd step is essentially the same but use the final cut out on "outside vector" strategy and it should give you the 1/2 cove diameter of your core box bit.
3_ V bit, same as core box cove. Use a 90 V to machine along your vector or offset it and run "outside vector" strategy. A 1/4" depth will leave a 1/4" chamfer on both sides of the centerline so with 1/2" material the cut out will follow the appropriate centerline of the V and cut the final 1/4" out with any size bit using an outside profile cut.
Heres an example of the roundover on a redwood sign with 60V art and 90V letters FYI

Ray, nice article in Sign Business.
4732

[phil_o]

You could use a "point rounover bit" to achieve a radius on the edge. http://www.woodline.com/scripts/prodView.asp?idproduct=384

[tomj]

how about this one from onsrud? I'm guessing you could do the cut out and round over in one shot.

https://www.onsrud.com/oc/pdf/OC_Solid_Surface_Brochure.pdf see bottom

[mikejohn]

Tom,
I guess the only problem with your 'one shot' is the depth the bit may have to cut into the spoil board.
Of course, there's nothing stopping you using a 'false' spoil board for one offs, or a dedicated jig if making many.

.........Mike

[tomj]

I guess I didn't look too close at the length. Maybe there's something that may fit the bill along the same concept though.

[waynelocke]

You should be able to have a sharpening service cut it down to the length you want and perhaps have it modified to have a point so that you could do the lettering then cutout and profile the sign edges. You could for sure have a bit made to do this which might be worth it if you do a lot of these.
Wayne