[idtat]

I feel this is a stupid question and have looked around a bit for an answer and maybe I cant see the forest from the trees

Do I build my tool table in Fusion or Path Pilot, or both.

Will PP reference 360 for offsets, lengths, rpm etc......

Should have the PCNC440 here next week and am trying to get ahead of the curve

Thanks
AW

[SCzEngrgGroup]

Both, as they are completely different, in terms of what information they contain. The tool table for the CNC controller only cares about tool length, and sometimes diameter. It neither knows nor cares the type of tool, and all the other things that are typically included in the CAM software tool table. BUT, both should either use the same tool numbers, or your POST should re-number the tools.

When it comes to tool tables, there are a million different ways to do it, and you need to figure out what works for you. Some people will try to convince you there is one, and only one, "right" way to do it. That is BS.

Personally, I have an extensive tool library for my CAM programs (>500 tools). However, many CNC controllers do not allow that many tools. Mach3, for example, only allows 255 tools. So, my Fusion360 CAM POST always re-numbers the tools in the g-code, so they are sequential. That means the CAM tool numbers are not the same as the physical tool numbers. But a typical job only uses perhaps a dozen tools, so it's easy to do the "mapping" when I load the tools into my ATC.

Regards,
Ray L.

[Warren_3Deee]

Set up PP with correct, measured tool lengths - it needs this to function correctly (F360 CAM is just going to say "use tool T3"... and your mill needs to know how long T3 is - this doesn't come from F360) - mandatory.
OPTIONAL - also set up tool diameters in PP if you are going to use conversational with PP (which is handy sometimes).

In F360, you really only need to create tools with same numbers as PP, and the correct diameters (or type, flat, ball, drill, etc.); this is really only required in F360 so it can create the correct CAM. You can also set the tool lengths in F360, flute lengths, etc. so you can get warnings about tool crashes, etc... but don't confuse the tool lengths set-up in F360 as anything to be used by your 440..... the 440 only cares about the lengths set-up in PP.

Personally, I have PP set up with correct tool lengths, cutter diameters, and descriptions, and then I went over to F360 and set-up the same info there, plus added the correct flute lengths, etc. because as my tool library grew, it was easy to forget the flute length of some specialty tools and try to take a depth-of-cut that was deeper than my flute length. Not necessary, but nice to have as a reference. The other thing I found is when I buy a new tool, all the specs are handy and easy to enter.. vs. trying to dig up the specifics of various tools later on.

[Warren_3Deee]

Just a couple other things.. F360 CAM will create gcode that gives feed rates, spindle rpm, and axis movement. All those things are determined when doing the CAM design in F360.. it is all written in gcode and that is what your 440 (via PP) will read. However, when you take that gcode (in the .nc file) and load it into PP, you have some overrides there to slow down (or speed up) the feedrate, the RPM, and the max velocity.... so you have some control over your machine at "runtime". Very handy when you are just getting started - rather than having to go back and forth between CAM and 440 to make small changes.

[Steve Seebold]

I am still using Mach III and I have "NEVER" used the tool library. I do all my tool offsets in the same page I use for work shift offsets.

If anyone would like to talk to me about how I do it, I'm near the end of a road trip and should be home in front of the machine by Friday. After that, you can call me at 714-420-2453 and I'll be happy to help.

[joshetect]

I have my tool library setup in fusion. I generally try to put a tool in a holder and keep it there, so far that has worked (other than drills)

I really like the setup sheet that fusion outputs. It gives you all the tools, with little pictures, #'s, ZMIN and a bunch of other info. I'll take that and double check that all my tools / tool heights are correct in PP and make sure everything is tightened down. I use a silver sharpie and write the tool #'s on the holder then go to town

I'll also make any notes I have and improvements in each op on the setup sheet.

[sharmstr]

Everything said here about Fusion and PP tool tables is great advice. But I suggest that you watch a few videos on the Fusion tool libaries. What you might get hung up on is the difference between your master libraries and your part libraries. I wont go into detail here since the Autodesk and NYC CNC videos explain it.

One thing I find really helpful is setting up master tool libraries for the different materials I run. They are cloud libraries so I have access to them regardless of the computer I'm on. I have one set up for aluminum and one for steel. As other have said, fusion doesnt care about your tool lengths, but it will tell PP the speeds and feeds to run so having the different material libraries is a huge time saver. Having your tool length and stick out is nice but it doesnt have to be accurate in fusion. As others have said, it will give you an collision indication. In those cases, I always double check the tool length in PP.

[idtat]

Thank you everyone, now makes more sense. My PCNC440 should be here Thursday and I took Friday and Monday off work to make chips.

AW