PCNC Vertical Lathe and Acetal

[BlueFin]

Spent the last two days designing a part and hand G coding the tool path, I built a block that holds the tools I need in the vise. This starts with a tube of .520" OD .200" ID Delrin Acetal, the tip has an angle on the OD for about .250" and a step, while the ID is bored to .240" with a re-ground endmil, then the table shifts so the endmill will single point cut the bore cleanly to a .250" then again for a .190" deep counterbore. The part comes out very clean with a very nice surface finish.

YouTube - Tormach vertical lathe turning Acetal.

YouTube - Tormach vertical lathe turning Acetal.

[justgary]

Bluefin -

Thanks for posting this. I had wondered how I would cut a particular tool that I want to make, and you may have provided the answer! I'll post my results whenever I finish making a tool holder and get around to trying this method.

- Just Gary

[BlueFin]

Originally Posted by justgary Bluefin - Thanks for posting this. I had wondered how I would cut a particular tool that I want to make, and you may have provided the answer! I'll post my results whenever I finish making a tool holder and get around to trying this method. - Just Gary

Sure, just keep in mind that when writing the code for your moves you will realize that you end up with about 10 times as many lines as what you thought it would take and that translates into about 10 times the time too! All the moves are written bass akwards from what makes sense when you use the mill as a mill, and the results are never what they seem. But after two full days of screwing around you will be able to make a .29 cent part

[justgary]

Bluefin -

Here's my plan (I'm using SprutCAM, but this will work on any CAM system):

1. I draw the desired part profile in my CAD program, but instead of making it round, just leave it flat. Also, define the part so that the future rotational axis is along X (with what will be the spindle on the left side), and the side to be cut is up (positive Z). Use the very tip (center of the furthest end) of the part as (0, 0, 0).

2. Import the model into SprutCAM and define a cutting tool that looks like my lathe tool (since I use triangular TNMG inserts, it's a cone with a small radius at the tip).

3. Do the SprutCAM toolpath magic and post the G-Code.

4. Edit the G-Code and replace all occurrences of X and Z in the following order:
a. Replace all "X" with "A" (a placeholder character).
b. Replace all "-Z" with "X"
c. Replace all "Z" with "-X"
d. Replace all "-A" with "Z"
e. Replace all "A" with "-Z"

5. Save the file and run it. Note that this order of replacement is important, and assumes that your lathe bit is to the right of the spindle. Also, you may need to edit the spindle direction if your cutter faces you instead of away from you.

I did a test (without the part or the cutting tool), and it looked like the machine did what I expected. You would still have to program your center drilling cycle, but that one is the same as a real drilling cycle.

Give it a try the next time you need to do the "vertical lathe" trick. Programming the toolpath should get a lot easier, so you can do very complicated cuts without pulling your hair out. I'm lazy, and I want to keep all the hair I can.

Regards,

- Just Gary

P.S. It just occurred to me that you could reverse the X axis in the CAD program (put the spindle on the right) and not have to flip the sign of Z in the steps above. I'll probably do it the way I stated above, because I don't like thinking about the spindle on the right side.

You have to keep the Z axis up so the program will generate the toolpath correctly, then flip the sign as you swap the axes. If you put the lathe tool on the left of the spindle (and facing you), you would not have to flip the sign on X, or reverse the spindle direction.

Just a thought.

[justgary]

Ok, I finally got around to making a tool holder and tried it out. I had stated before what axis exchanges to make, but I found out that Z was upside down when I tested it (my part was nearly symmetric, so I couldn't tell at first). If you try the axis exchange method like I previously described, just replace "A" with "Z" and leave the minus signs alone.

Not satisfied, I went back to SprutCAM and fiddled with the lathe options. I discovered the X-Z lathe machine choice, which produces the proper G-code without modification provided that you put the tool holder to the left of the spindle with the top of the tool facing you. It is also waaaay easier to define a lathe tool instead of trying to fake it with a milling cutter.

You'll still have to touch off (for X, at least) each tool you use, but you'd have to do that if you hand-coded the part. You could try setting a local coordinate system for each tool and changing that when you change the tool.

As for me, touching off each tool is a small price to pay, and it keeps me conscious of what's actually happening.

Enjoy!

- Just Gary

P.S. Bluefin, I agree with you on the two days of screwing around for the 29 cent part, but I made a threadmill (I still need to heat treat it) which would have cost me around $50 to buy. If I charged myself by the hour to make it, it would only have cost about $800, so I figure I came out even... Plus, the next one will be much cheaper to make. Since I'm a tool wrecker, I know this won't be the only one I ever own.

On the other hand, I made a six flute taper reamer a few weeks ago that I couldn't buy because it has a non-standard taper. It warped a little when I treated it, but it works just fine for what I need.

I just lump all of the time into the experience basket and enjoy it.