Any hints how to go Autocad -> CNC -> flashlight?

I've got AutoCad Mechanical Desktop and even nicer I've got Autodesk's Inventor. Both acquired via educational use. I want to try designing a light body or reflector then getting it CNC'd for me. (I'll ask about anodizing at a later time. I think I recall seeing at least some postings on that topic.)

Does anybody know what file format I need to send to a CNC shop for their machine to use?

Does anybody have recommendations on selecting a machine shop to do that kind of thing? I know from some of my own very lightweight machining experience that 1-offs are very time consuming and would probably be kinda expensive, but I'd really get a thrill out of seeing such a result.

My Autodesk Inventor indicates that it will save a file to the following formats: IGES, SAT, STEP, "Streamline Assembly Packages", XGL, ZGL.

The Mechanical Desktop says it'll save to ".dwg", "dws", ".dwt", and ".dxf".

Please pardon my ignorance on this, but I'm just a newbie to the CNC thing.

ANY help would be greatly appreciated!!!

You will need a convertor, each type of machine uses a different code

The convertor program will usually take the DXF file since it is the most portable and generate the control codes for the CNC machine

So I need to find & phone a particular shop and ask them about their machine as they're not standardized. I hope the shop would have the converter.

Thanks Mike!

Its not really the machine, its the controller

You can purchase a CNC MILL or CNC LATHE and then put one of several different controllers on it; each controller uses a different command language

There are several different software packages that convert DXF to CNC command language, sometimes - if the product being machined is simple enough, its just easy enough to write the code yourself

A .dxf file is standard. The programmer will use this to generate tool paths, etc., then use a "post processor" to output code for the machine they intend to use.

JackBlades has it right.

The DXF (Drawing eXchange Format) is a well known standard. The newer standard for more complex parts (like molds) is IGES. The best thing you can do is to give the machine shop a 'print'. For "round" work like a flashlight body, you only need the profile. For square woulk you will need several views.

If the shop can work from your cad files they may not want all the fancy rendering and 3D stuff. Ask them and they will tell you what they prefer to work with.

And your right, a one off is going to cost a lot.

One piece might be $100 and two might be $101 .

The cost of programing and setting up a job is going to be the bigest part of a small run, not the time and metal to make it.

Just for fun here is a sample program:

:0712(EATON #ESK-10238)
(OP#-01)
(1/4-6061 ROD *7.00 LONG)

N10(FACE CNMG-430.5)
T0101M8
G99G97M3S2000
G0X.265Z.5
Z-.015
G1X.25F.003
U-.03Z.0F.001
X-.03F.002
G0X7.0Z7.0
M00
(FLIP PART)

N20(FACE+TURN)
T0121M8
G99G97M3S2000
G0X.265Z.5
Z.2
G72W.03R.01
G72P201Q204U0W0F.008
N201G0Z.005
N202G1X-.03
N203G0Z.2
N204X.265
G0X.175Z.025
G1Z-.248F.005
G0U.02Z.025
X.14
G1Z-.248
G0U.02Z.0
G1X-.03F.002
X.1F.004
X.135C-.017F.001
Z-.248F.0015
X.26F.002
G0X5.0Z7.0
M1

N30(THRD #6-32)
T0414M8
G99G97M3S1000
G0X.15Z.5
Z.125
G76P011030Q25R.0005
G76X.099Z-.205Q35P192F.03125
G0X5.0Z7.0
M1

N40(U/CUT .031)
T0616M8
G99G97M3S2000
G0X.265Z.5
Z-.255
G1X.25F.003
U-.01Z-.25F.001
X.099F.002
G0X.145
Z-.227
G1X.099Z-.25
X.135W.01F.02
Z-.02F.003
U-.04Z.0F.001
U-.05W.0015F.002
G0X5.0Z5.0
M1

N50(DEBURR THRD)
T0414M8
G99G97M3S1000
G0X.15Z.5
Z.125
G76P011030Q50R.0005
G76X.099Z-.205Q192P192F.03125
G0X10.Z10.
M30

I'm a programmer for the precision sheet metal industry. We usually convert Autocad files to a dxf format and that format get inputted to the program that creates the G-codes for the cnc presses (output is the same as shown in CNC Dan's sample code). Seeing how I work with sheet metal, all my files are in a 2D format (dxf format is best for 2D stuff). I use to help out a machine shop with their 5-axis mills, and they usually prefer files in a 3D format (igs or sat format). Just locate a machine shop and ask them what type of files they can accept. As CNC Dan says, most of the money in manufacturing stuff in small quantity is the programming & machine setup cost (when you order a large quantity, this cost gets amortized over the entire run, only adding penny to the unit cost). The cad software that I use all the time is autocad's Mechanical Destop (I also use Inventor, Solidworks and Pro-E).

Ed

Peter,

I have been reading your post along with the other posts. Correct me if I'm wrong, but all you need to know is how to get a file to someone to cut vs. the machining aspect. Right? JackBlades and CNC Dan are correct about file types. You should be fine exporting a dxf file. I have been doing prototyping(cnc work) for the last 12 years. We don't do lathe cnc work, but I can check with a vendor I know if you would like me to. Do you have the part(s) you want designed already? If you do, email them to me(dxf format) at [email protected] if you would like me to get parts quoted for you. The main cost will come down to how long it takes to program. Run time probably won't be bad. One thing to make sure is that whatever you design needs to be totally thought out down to the last detail. Tolerances, etc. The parts will be cut to your file unless noted otherwise. The last thing you want is for parts to be cut and something to not fit properly. You will then be charged for any extra time spent making corrections. Your project probably won't be cheap. Good luck.