balsaman

I did. I love it. Here is a pic.

Eric

balsaman

Here is some stuff I have cut. Fuse sides? Try that with a razor blade.

balsaman

Wing ribs.

BMatthews

Very nice.......

Is this all from scratch or one of the commercially available kits?

balsaman

Mine was from scratch. I designed and built it. It's made from MDF, some plastic and recycled linear rails and linear bearings. I had lots of help from info on the web.

Drive board and stepper motors were from www.stepperworld.com

There is a fellow on the web who sells plans for home made cnc machines made from hardware store parts and hand tools. I didn't buy his plans but he had lots of good advice for me anyways. Very knowledgable on home made cnc.

www.crankorgan.com


Mine is 12" x 24" cutting area. Cost me about $300 USD not including the router, which was another $60.00 USD. Slides and bearings were free.

Eric

chrisbarker

Eric,

In the picture your table has a bunch of holes in it. Is that your hold down system? What are you using for pins?
Do you have any problem when you get down to the last sliver holding your part in place. Does it do a little dance?
The last place I worked at had a large CNC that had a vacuum table. It had a 1 1/2" LDF sheet on the table and would suck down 3 sheets of 3/4" MDF on top of that.
Any way I was just wondering if there was any need for a vacuum hold down?
Nice looking machine.

Chris

AV8TOR

My Feedback: (2)

I don’t know what balsaman is using to hold down his parts but I built a vacuum box to hold down balsa sheet stock. These are wing ribs for my 27% Ultimate Bipe that I just started. It works fantastic.

AV8TOR

My Feedback: (2)

For 1/8” larger sheets I simply use double-sided tape to hold down my parts. These are also for my Ultimate.

catspaw

I bought the Hobby CNC package, and after putting the control electronics together, I decided I wanted a table capable of cutting a 12"x48" sheet. Has anyone considered this? I've looked at McMaster Carr catalog, and know that to get the rigidity over the 48" length, its gonna cost some money.
John

soarer

My Feedback: (1)

What type of software are you using for the layout of the ribs?

balsaman

The holes in the table were drilled by the cnc itself! I installed 325 10-24 blindnuts in the holes. They are drilled every inch square. I use them to clamp the parts with nylon bolts. I plan on also adding a vacuum attachment so I can use vacuum hold down as well. Same holes!

Yes, the parts flop around once they are cut out. I could leave little tabs but I have not found that they are needed. I set it up so it cuts all the inside holes first, then the outsides. Cutting the outside first makes the inside holes interesting!

I use Autocad to draw the parts, then convert the parts to Gcode with AceConverter, then use TurboCNC to run the machine.

AceConverter is freeware at www.yeagerautomation.com
TurboCNC is free download at www.dakeng.com. It's shareware and costs $20.00 to register. I registered it.

There is also more cnc software: Kcam from www.kellyware.com, CNCPro from www.yeagerautomation.com. Both these are more $$$. Kcam runs in Windows. Generally stepper motors/drivers don't like Windows. Turbocnc and CNCPro work in DOS mode.

AV8tor, thats a big table you have there! Did you build your cnc?

catspaw,

I know they don't recommend enlarging thier machine. I would start smaller for the first machine.

Eric

AV8TOR

My Feedback: (2)

No it is not a home built. It is a 5-axis Thermwood router w/ tool changer. The table is 60” x 60” x 24” in Z. 8 HP at 18,000 rpms see http://www.thermwood.com/Thermwood_R...res/M67_01.htm

It’s nice to have toys at work.

AV8TOR

My Feedback: (2)

Balsaman I should have added that it looks like you did a great job with what you built. It is really fun and rewarding drawing up the CAD file then CNC machining your parts Huh? You can do so things that you can’t do with a laser. Today I cut some ply parts for my Ultimate. The firewall was cut from Ό” lite ply. On the fuse top I am using some stringers but I did not want the stringers to go through all the way to the firewall so I did a pocket toolpath and stopped it from going al the way through. Now the stringer lay flat in the pocket.

balsaman

av8tor,

Those fuse sides look great! What kind of bit do you use? Looks like a clean cut! I use 1/8" and 1/16" two and three flute carbide endmills. Cut around 15 inches a minute (I can go up to 35 or so). My router is variable from 8,000 to 30,000 rpm. I need to sand the parts after cutting. Your parts look to be cut nice and clean. I have thought about using a burr instead of an endmill. What works for you? Feedrate and spindle speed too if you don't mind.

Eric

AV8TOR

My Feedback: (2)

On all the parts I have been cutting for the Ultimate I have been using 1/32” and 1/16” diameter End-Mills. I use the 1/32” for parts that need tight corner radius and the 1/16 for the others and sometimes a combination of the two. The feed rate was run at 30 IPM at 15,000 rpm. I don’t know if you can do this with your code program but I am using MasterCam, which will allows me to peck in the Z-depths. I also can take a rough then a finish pass. These parts were just with a finish pass. This will give you the better finish without the load. On the Balsa with the 1/32” end-mill I use 0.030” pecks and on Lite-Ply 0.020”. The 1/16” end-mill I use 0.060” pecks on Balsa and 0.030” on the ply. The finish is very nice only needing to sand some edge fuzz. Keep in mind this machine is designed to cut up to 400 IPM. The rapid traverse rate is 900 IPM.

a088008

Those are fantastic machines!

I'm considering making one for myself (maybe a little simpler and smaller for a beginner).

Would you recommend making one, instead of sending my designs for laser cutting?

-Q.

AV8TOR

My Feedback: (2)

Balsaman how much did you end up spending for that set up if you don’t mind me asking? Here is a site with some small machines in the 2-4K range for information purposes. Maybe Ebay might have some used.
http://www.maxnc.com/

balsaman

My machine cost me about $300 USD.

A088088,

Have a look at www.crankorgan.com for plans for cheap cnc machines.

A homemeade cnc is great for projects and one-offs, I would, and still do, have a laser guy do my cutting for production runs. The cnc is too slow. Also, laser cut parts do not require sanding etc.

Eric

balsaman

AV8TOR,

When you say pecks you mean plunge, stop, plunge, stop with the z into the wood?

I have mastercam but don't have the patience to learn it. I know Autocad quite well so I use it and convert with AceConverter to Gcode.

I imported a dxf into mastercam and used it to make the toolpath once. Worked good but I had to have the manual beside me to do it. I do think its a better way to go so I should try harder. I should install it at work when I have more time to play with it.

Eric

AV8TOR

My Feedback: (2)

Let’s say the wood is 1/16” thick or 0.060” If you wanted to take 0.020” pecks the first pass would start at 0.040” and complete the entire contour, then move down 0.020” taking another complete cut until it reaches the bottom.

I think once you start using MasterCam you will find it is not that hard to use, especially if you know AutoCad. What version do you have?

balsaman

Oh, ok. Multiple passes. yes, I can do that with aceconverter. I haven't tho, I just cut in one pass full depth. You find it does a better job that way?

I have version 8.1. Do you use wire or mill? I have a tutorial but it's version 7 so it's confusing ansd slightly different. If I sat down and worked on it I would probably be fine.

Eric

AV8TOR

My Feedback: (2)

Much better. If you can turn up to 30K in rpm's cut in pecks and you can increase the feedrate some.

There was a difference between version 7 and 8 and I know what you mean about tutorials. Feel free to email me direct if you have any specific questions. If you like send me a part file and I will email you a step by step quide. Once you see it you will be able to use that checklist on any contoured part. I am using version 9 but I still have 8 loaded.
[email protected]

catspaw

Yes, Mastercam is a terrific program. It's what I judge other CAD/CAM programs (turbocad, modelcad) by.
I have cut some parts on the Fadal machines at work, but thats on a avaibility basis, so I'd like to have my own CNC router.

I will probably the hobby CNC router with a 12" Y (instead of 9") just to get the feel of things.

But if I go with a 12"x48", I'll definitely make is sturdy, and probably use a laminate trim router.

Incidently, I use a 1/8" left hand spiral mill for those times I cut at work. This is to keep the part from pulling up on the bit. I dont have a vacuum table, just clamp along the edges.

I need to find one of those valves that allows you to use air pressure to make vacuum.

John

AV8TOR

My Feedback: (2)

I am just using a Shop Vac for my use, and the box was made from scrap MDF stock.

balsaman

Yeah I know what you mean about the part lifting due to the spiral flutes on the bit. I need to get the vacuum table done. I am always in there with my hands holding the wood down.

Where do you get your left hand bits? Has anyone tried anything other than an endmill?

Thanks for the offer to help AV8TOR, next time I look at Mastercam I will make a list.

Eric