[artdutra04]

I use SolidWorks, but here is the general process on how parts go from a CAD model to a finished part via CNC. (It's good to keep the entire process in mind, even if you are just designing the parts).

1. The first thing I do is make sure the part is actually manufacturable on the machines that I will be running it on. On milling machines, there cannot be any square inside corners (though you can use a small drill at the corner to achieve a square), and make sure any part radiuses are as large as they can. There's no sense in using a 1/8" end mill to make all those 0.0625" radius' corners if you can use a 1/2" end mill and functionally the part will be the same.
   
   Also as a subset of this, if the part is "deep", make sure you only use large radaii down there. They don't make things like a 1/4" end mill that has three inches of vertical cuttable edge. Also, if you want to do engraving on the surface, I've found that a number four center drill at a depth of five thousandths work well.
   
   Another thing to think about is how the part you are making can be held down while it is being milled. Rectangular parts are usually easy (they can just be clamped in a vise), though if you want holes or pockets near the edge (which might hit the parallels), you will need to figure about another way to fixture the part. Soft jaws (custom aluminum jaws made to hold that specific part) are one option, using bolts and mounting the part on a fixturing plate is another.
   
   Another critical thing to keep in mind is which dimensions are critical, and their expected tolerances. You should mark all part dimensions on a separate file from the main part, and show all part tolerances as well. Make sure all tolerances are set as low as possible; if certain dimensions or features are not critical, don't specify that they need to be within a tolerance of 0.0001" if a tolerance of 0.01" is just fine. Leaving the dimensions lower can make the part easier to be machined, as well as result in faster production time.
   
   Before the part can be made, the above points are crucial. Just because the part looks good in Inventor or SolidWorks does not mean that it can be manufactured.
   
   .
2. The next thing to do depends on what CAM program that use. For my parts, I always export a DXF of the part from SolidWorks and import that into the CAM program (FeatureCAM) that I use. There are a lot of different CAM programs, such as MasterCAM, GibbsCAM, Espirt, etc.) so the process may be different in each.
   
   But once I have the DXF (make sure it is exported at 1:1 (full-size) ratio), I import it into FeatureCAM. From here, I have to set the material size and composition, where the part origin is, how the X/Y/Z axis' are orientated, and where the part is in relation to the material. Then from here, I have to make each machine operation, such as pockets, grooves, holes, etc. I also select the tool, the feeds and speeds, the operation (climb or conventional), if I want a rough pass with a second finishing pass, how much material I want to take off in each pass, etc.
   
   Granted, FeatureCAM does help along the way and has a lot of preset options, but it is impossible just to import a .sldpart or .ipt file and expect it to do everything to make a .nc file for me.
   
   .
3. The next step is I simulate the CNC operation in FeatureCAM. This usually tells me if something wrong happens, like if I set a feature offset wrong and the cutter rapids into the part.
   
   .
4. Once this looks good, then I can generate the .nc file. The .nc file is what actually runs on the CNC machine. When you generate the .nc file, you also need to make sure you select the right post-processor for the machine you are using. I had a friend give me his customized post-processor for working with Haas CNC machines, as most CAM software only comes with generic post-processors.

Originally Posted by Generalx5

How do I get an ipt file to work with a CNC machine? I have a few aluminum parts that I've designed for use on the chassy, how do I export the ipt file so that the CNC mechanic or computer can read its dimensions?

I have more than a dozen parts, so dimensioning them would take a while, the CNC mechanic person would also have to design it back so he can run it on the CNC. Is there a way to convert the ipt file to a standardized format so that I dont have to dimension them, whoever opens the file, all dimensions will be available to them Via computer.

Is there even such a thing?

If the CNC work is being down by an outside person/company, consult with them, and ask what software and file formats they use. Generally, I've found STEP (.stp) files to be pretty universal for 3D models, and DXF files to be pretty universal for 2D models.

Also, in addition to the part models, it is always useful to submit a dimensioned drawing of the part, showing all the critical dimensions and their tolerances, as well as the number of parts needed, the material required, and any other part features which are important to keep in mind while manufacturing the part.

I'd suggest that if you don't have any experience in this field, ask for a tour of a CNC machine shop, and ask lots of questions along the way about the process. You'll learn a lot, and it'll most likely make your part designs even better.