[Gui Cavalcanti]

Hey, I'm exactly in your boat!

A company in Richmond, Jewett Machine, hired me to learn how to get their CAM software to work with their CNC lathes in the shop that are still running pure G-code. I'm working with a program called ESPRIT (not aspree, which was referred to earlier) 2003, which is kind of nice for lathe work. I haven't tried the milling functions, but I hear they're extremely easy to work with once you get the hang of them.

ESPRIT 2003 can import solid models and 2D drawings, all that good stuff. The basic distinction between ESPRIT and a true solid modeler is that ESPRIT goes a step further and defines "chains", or lines across your existing model. These chains indicate where a tool needs to move across a part. You then define your tools and everything associated with them (for lathes, things such as nose radius, relief angles; for mills it's more like 4 flute, 1/2" high-speed steel roughing end mill, and both need feeds and speeds), and then create tool paths based on the chains you defined earlier. Once you've defined all of your chains and tool paths, you can simulate the cut and watch the machine run across your part. You can also go through the trouble of defining your clamps, spindle maximums, and tailstocks in the case of lathes.

Anyway, you'll find that you'll have a great little computer-generated movie of your part being made, but now you need to get it to a CNC. I don't know if MasterCAM does this, but ESPRIT requires you to edit what's called a post-processor in order to translate your model's instructions into G-code. As someone said earlier, all CNC controllers (and even down to machine models, if you'd believe it) have different sets of machine codes. For instance, M03 on the Ecoca lathe I'm working on (with a Fanuc O-TC controller) means main spindle on, clockwise. However, on the OMega vertical lathe I'm also working on (again, with a Fanuc O-TC controller), M03 means main spindle on, counterclockwise. You can see how that might mess things up a little bit...

You'll find that you can learn whatever CAM software you have pretty quickly (assuming you have a working knowledge of a machine shop, another really good suggestion), but the post-processor will give you the most headaches. It's easy to tweak variables like switching the M03 definition on the OMega and Ecoca lathes, but it gets really hard when you start getting into canned cycles. For instance, to switch tools, the Ecoca simply has to move to a position that doesn't touch the part and turn it's tool turret (G00 rapid movement, M63 toolchange). The OMega, however, has to retract to it's home position, open the machine guard doors, move the turret to tool-change position, release, change the magazine, acquire the next tool, return to the home position, and close the machine doors (G28 U0 W0 home, M66 doors open, G30 U0 W0 change position, T# tool call, G28 U0 W0 home, M67 doors close). When you say "switch tools" in your CAM software for the first time, you may have no idea as to what your machine might do.

The good news is, once you get the post-processor right and tweaked to your machine, you'll probably never have to mess with it again. Do it right, though; don't translate code through it and then find one little nagging detail that you change at the machine just because you don't want to find it in the post (This should really be a G72 instead of G71, I'll just remember to change it). This will lead to extreme confusion if you ever have to switch CNC machinists.

If you were given the machine, the CAM program, and the appropriate starting post-processor on the same day, with all of their documentation, I'd say you could tweak it to near perfection and be turning out within-tolerance parts within 2 or 3 weeks. If you have a machinist who knows the codes, canned cycles, and trivia like machine home positions and codes that may not "work" (G28 can't be used on the Ecoca, for instance; usually it means machine home, but if you are already home it will move to a random location. This would happen if you paused the machining cycle at G28, and then resumed.), I'd say you could really get going in 1 to 2 weeks solid. Whatever you do, though, don't expect to hook up your computer to the CNC, make a nice little square on the screen and expect it to be waiting for you by the time you walk over to the CNC. It takes time, energy, and a lot of patience.

In case you're curious, I spent my first week at my job training on the manual lathes, then moving up and watching some manual/CNC hybrids work, then finally spending two days solid watching/learning how to use the Ecoca. Working with a very well-trained machinist who was responsible for the Ecoca, I got a part program exported and working without "at-machine tweaks" in one and a half weeks. I started working on the OMega last Friday and have yet to make real progress on it because the canned cycles are giving me lots and lots of grief (stuff like refusing to acknowledge rapid moves before a canned facing cycle, etc).

Any questions, don't be afraid to ask!