Flip Milling Process

[groucho]

I laminated several sheets of rectangular 1/2" marine plywood sheets together to form a 3 1/2" thick slab. The first goal is to clean up the vertical edges with a 1/2" carbide end mill with two flutes. I want to create a clean block with true vertical faces on all four sides so I can flip mill it with accuracy. This is my first experience using more than the first 7/8" of a bit and it didn't go so well. I oversized the stock about a 3/16" +/-on all four sides and thought the 1/2" bit would have no trouble trimming out the block as it dropped 1/2" per pass and ate about 3/16" into the wood as it cut rectangular toolpaths around the perimeter of the stock. I ran the router at 18000 rpm using my 2.5 HP spindled PRS Standard machine. Here is a picture of the block after the procedure and another block before being trimmed:

Trimmed Piece.jpgPretrimmed piece.jpg

The bit only had 2 1/2" of actual blade so I didn't cut all the way down the side of the block and cleaned up the remaining material with a flush trim bit in my router. In the attached picture you can see the rippled face where the shopbot milled it and the smooth face where the router bit surfaced it.

Maybe this procedure is inherently loud because the bit is eccentrically loaded in a trimming operation but from the very beginning of the tool path the bit was loud trimming out the material and by the time it was almost done the bit was really loud. It finished the routine but the bit wound up sitting on the part at the end of the process. It was still in the collet but it turns out it had wiggled loose a bit. I'd like my next results to be more like that router bit and a lot safer . Maybe the answer is self explanatory. I need to tighten up the bit more when I play with a 1/2" bit instead of my usual 1/4" fair?! Maybe longer router bits also just produce a less quality cut because they have to extend so far out from the spindle? I'm really hoping this kind of performance is not something I should get used to. The large bits are expensive and I'd like to produce something with more accuracy. I wound up tossing the collet and the bit. The bit was chipped on the end.

IMG_9420.jpgIMG_9418.jpg

I've purchased another bit. Can anyone give any advice on how to do this right? Maybe make toolpath passes in smaller vertical increments? 1/4"? Maybe I just need to make sure that collet nut is tight? Any help is greatly appreciated.

[steve_g]

Michael…
This is asking a lot from a machine that cost less than 100K... But it can be done using the proper techniques! First, the part must be held down absolutely solid! Second, because of the tremendous mechanical advantage the wood has when using a long bit, take smaller bites. Third, use a “onion skin” cutting strategy. By “onion skin” I mean cut over size about .01” with a climb cut, followed by a final finish pass in the conventional direction.
I don’t know how old your machine is… but it must be “tight” for success with this operation. Try these suggestions and let us know how it went! Oh, and your bit must be TIGHT in the collet!
SG

[jerry_stanek]

Also a spiral bit may be a better choice

[steve_g]

Michael…
I’ve been thinking about your question and re-read your post… somehow it got past me that this was cut with a ¼” bit. I’m not sure you will ever be happy with the cut quality using this bit! Was your flush trim bit a ½” one?
The adage “when you’re a hammer, everything looks like a nail” may apply here. If you have a table saw, it’s the better tool for this job! If you’re determined to do the job on the bot, a half inch spiral bit would be a good investment!

https://www.magnate.net/ProductDetails.asp?ProductCode=2011

https://www.centuriontools.com/router-bits-toolcase/solid-carbide-wood-router-bits.html?sku=12US22.1254&pcn=Upshear&pid=779&sat= 1

Also, a down cut bit would be a good investment…
SG

[groucho]

Sorry I wasn't clear. I AM using a 1/2" bit.

[groucho]

Step cut.jpg

I do have a tablesaw and I was worried about the imprecision of the tall vertical cut but I take your point. Much more expedient and I can always measure things with the calipers and take my time to get it close. Yes, I definitely have my "shopbot goggles" on these days.

Attached is an image of a cup design (only one half of it actually). This is what I'm ultimately heading toward producing in Fusion 360. The machine hasn't been used a lot and I think it is in relatively good shape (with the possible exception of that bit incident ). Do you think flip milling a cup part like the one I'm showing is possible if I onion skin as you say? It measures about 3" tall.

Thank you so much for your response.

[steve_g]

Michael…
I’m not a fan of flip ops… I’ve used steel dowel locater pins, and other “precise” locating methods, sometimes it works and other times with the same jig, the result is less than stellar. I just finished a chair design that I spent “extra” time designing to avoid cutting from two sides. I’m convinced that my poor success rate has nothing to do with my locating method and everything to do with the nature of wood… it moves when stress points are cut! Sometimes you have to think outside the box… here’s a 10” deep “Vase” I made by stacking rings and cutting the exterior on my indexer…
SG

[Burkhardt]

Right now I am working on a set of very thin walled lamp shades 3.5" diameter and 3.7" tall. In a way similar to your project but with a kind of tulip shape, i.e. the wall have varying slope (not vertical).
For such things (or similar deep bowls) I usually cut the inside cavity of all the parts first without much regard to positioning. Then I machine a plug from scrap wood which is exactly the negative shape of the cavity but only 1 or 2 inches tall and drill a hole in the middle for a vacuum connection. Now I can machine the outside of all parts one after the other by seating the cavity onto the plug, if necessary with a thin gasket on the bottom. This guarantees precise position of the outside relative to the inside, even if the wall is less than 1/10" like my lamp shades.

But even with a 1/2" bit it becomes difficult to go deeper than maybe 4 inches because the long leverage often makes it chatter and pit the surface. As mentioned previously the straight flute bit that you have been using also contributes to noise and vibration since it smashes the entire length of the flute into the material in one impact.

[groucho]

Cup Shot.jpg

Interesting. That is actually very similar to what I'm working on (see fusion rendering above) and would be very interested in any wisdom you have to share. That plug idea is great! Wish I had a vacuum table but it sounds like you might even consider it with a shopvac. Just started my second pass on the cup tonight with a much less noising bit. I think the trick with this vertical milling work is to just do much less ambitious passes than one usually would when one is cutting panels and working flatter. This small pass approach just seems to traumatize the bit less as the mechanical advantage of the work imposes itself on the tip of the bit. The wall of this cup is a 1/4". Glad to hear you're able to get the wall as little as 1/10" of an inch.

[Keith Larrett]

A different approach to this project would be to slice the model into seven 1/2" sections. Just cut the seven cross sections out of a 1/2" sheet of your marine plywood, glue them together and all you will need is a bit of light sanding inside and outside of the vessel.

I'm not familiar with Fusion 360, but I've used the slice function in Aspire on a project when I didn't have a long bit available.

That's a nice looking vessel.