CNC Router for cutting out ribs

[Jflyer]

Just ordered my Bearhawk 4-Place plans tonight. I've been reading and researching for about a year. I have the world famous Eric Newton's building manuals. I play with CNC machines and am presently finishing the build on CNC router that I will use to cut out the form blocks and rib sections.

[X'N]

Let me know if you need any tips or tricks. FYI the old Yahoo site had a wing rib and spar DFX posted in the files for the 4-place. I cut all my stuff out on my cnc router as well. IMO don't waste your time on trying to cut out your sheets without a vacuum table. I made one from MDF and use 2 shop vacs for a vac source. I found that a 1/8 single O-flute up cut bit worked the best for me (down cuts would pack up with chips and gum up too fast). I'd have to look at the feeds and speeds but if I remember correctly it was around 18ipm (don't rember the rpm off hand) that was full depth. I could have went to a 1/4 endmill and upped the feed rate a bunch but IMO it wasn't worth wasting that much material + I find my cuts to be much better and less material shifting going slow. The Key IMO for cutting 2024 is keeping the material cool while you cut. The .125 spar plates were a real learning curve. I ended up having to rig up an air blast as well as using WD for cutting fluid. I think my DOC was around .035 per pass. + always ramp in with your cutter, if you don't you can end up with a little disc riding under the cutter on a single O-flute. While its no machining center finish it looks pretty good for a home built router. On your forms Use a dove tail bit to do your outside profile cuts on the bending form. Once you bend your parts over on them they are almost 90* after spring back.

[Jflyer]

Hi Dan, Thanks for the info and I will definitely ask for help when getting CNC things setup. Vacuum table is in my plans as well. I figured it would be the best way to hold down sheets of aluminum. Is your setup a derivative of the Joe's CNC Hybrid, or something else?

I have a Techno Tabletop CNC Router I bought from a friend with the PC and all software. I used that to cut out the parts for Joe's 2006 version. I have rails and some additional items to build a version Joe's CNC Hybrid that will have a cutting area of 5+ feet by 10 feet. I want to be able to layout full sheets of aluminum for cutting parts including wing skins. Once the big boy is built, I plan to install a water cooled spindle on the Tencho in order to slow the rpms down to milling speeds to cut the heavier gauge aluminum as well as some metal parts with coolant added on.

I do have the DXF file from the Yahoo group. With the Techno Tabletop I cut out a nose rib out of thin ply and a center rib out of some aluminum flashing. All just for testing. It worked great.

Techno.jpg

[X'N]

Nice. I'd love a bigger router but I don't have room for it in my current garage. My router is basically a CNC Router Parts machine. Some day I hope to upgrade to a steel framed ATC spindle and ball screw machine, but as u know it takes a bunch of $ for quality components. What controller and cam software do u use? Dan scratch build patrol #243

[Jflyer]

The Techno machine came with a custom built controller the previous owner had built for this machine. I have no idea if even has a make. For software, I have AutoCAD, MasterCAM and Mach3 Loader. The little machine is lead screw, as is the Joe's 2006 CNC (24" X 48"), But the large machine will be rack and pinion. The Techno has only a 19" X 28" cutting area, but I made a fixture out of MDF that can be relocated along the X-Axis with pins and bushings. This allows me to cut pieces that are 48" long. Clamp the work material to the fixture, cut the first halve of the piece, then move the fixture 12" or 24" down and cut the second half. It works great. I'm still on the learning curve with CNC, but so far, so good.

[JohnF]

Any chance you could upload the files here? I just went to the yahoo group files directory and the dfx files I found give me "document not found" errors. Right now I'm interested in cutting a master form and checking to see if it matches the mylar.

I don't think I would trust the yahoo group as an information archive anyway.

[EDIT]

Wait, this thread is about CNC machines. I'll post a thread asking for the files in the forum for the specific model I care about.

[X'N]

Huh they open fine for me. http://groups.yahoo.com/neo/groups/Bearhawk/files

[Jflyer]

Unable to upload the DXF or the DWG files. Stating "Invalid File". I-M me your email and I'll send it to you.

[Jflyer]

http://groups.yahoo.com/neo/groups/Bearhawk/files

I've opened these DXF and DWG files in AutoCAD and DraftSight (free CAD software) and the flanges are on the drawings. I've also cut out some test pieces in thin ply and aluminum flashing. All looks good. I'll test some more and size up to the drawings once mine arrive from "The Bob"

Also. for a great free 2-D CAD software, take a look at DraftSight by Dassault Systems. The free version is a fully functional 2-D CAD that is incredibly similar to AutoCAD. Many of the same functions, clicks, key-strokes, and symbols are identical to those found in AutoCAD. I actually use the Draftsight more than AutoCAD mainly because it opens faster and in many ways, is easier to navigate.

Link to the DraftSight free download:
http://www.3ds.com/products-services...ight/overview/

[Jflyer]

Dan, Can you provide the specs and explanation of how your vacuum table works?

The vacuum tables I've researched have PVC pipes going to each quadrant and a glued on spoil board. Your vacuum table appears to just create vacuum inside the box and I see you don't use a spoil board.

[X'N]

Dan, Can you provide the specs and explanation of how your vacuum table works?

The vacuum tables I've researched have PVC pipes going to each quadrant and a glued on spoil board. Your vacuum table appears to just create vacuum inside the box and I see you don't use a spoil board.

I didn't feel like cutting holes in my top to add PVC and such (Also wasn't sure if the shop vacs I had would provide enough vacuum) thus I made the box that I can throw up on my table when needed.The top of the vac box is also my spoil board, I just surface it as needed. Once it gets too thin I can just plain it off and glue on a new top.

I may some day end up plumbing the table if I get a nice Vac source but for now all I use the vac table for is cutting my aluminum patrol parts. My spoil board under the vac table has T-nuts in the table every 8 inches so I usually just use clamps for most of my wood working or double stick tape if need be.

[X'N]

Just for reference for others here is the feeds and speeds I've had good results with for .020 & .025 2024 sheet: Single spiral O-flute 1/8 up-cut endmill, full depth 18,300 rpm and 18.4 ipm.
I tried cutting some .032 sheet today and it was gumming up really bad. I'm not sure I'll be able to take a full depth cut. I tried some other feeds and speeds but not near the results I got with .025 sheets. I'll update when I get some better results. On the bright side I found I'm able to nest all the aileron and flap spar attach angles in the .032 center rib lightning holes & I also drilled all the pilot holes for them too, it worked great! No way I could accurately drill 120+ holes in 5 minutes by hand

[Jflyer]

Dan, Great info. Thank you.
Please let us know the results of testing the feeds and speeds for the .032 and thicker materials. I'll be heading in the direction soon. (3 to 4 months).
Question: Were you trying to cut the .032 full depth in one pass?

[X'N]

Yes I was trying to cut at full depth in a single pass.

One good thing is someone posted this feeds and speeds link for me. I already had a feeds and speeds calculator but mine didnt have the material selection this one does. http://zero-divide.net/index.php?page=fswizard

[X'N]

I ended up ordering a couple new bits from Amana and was able to cut a sheet this weekend. The cut was nice until the very tip of the end mill broke. Not sure why it broke because I ramp in on my cuts (it only snapped off say .005 of the tip and I didn't realize it did until the job was finished. None the less the cut was much better with only air blast with the following: Cutter: Amana 1/8 spiral O-flute up-cut (aluminum bit) DOC .032 Spindle speed 24000, 48 ipm. I'm also begining to think that some of the 2024 you get depending on who you get your materail from or the MFG of the mateial was makes a difference on how gummy it is. (black ink lettered materail seems to be gummier than the red letterered suff)