sinds i am familiar with fusion360 I want to make one .NC file to load in the OneFinity.
i do not want to use multiple files for different tool paths.
In this video Dustin Patton explains it perfectly but he is using V-Carve Pro to set it up.
When milling the machine stops at a certain point and comes up with some of the following messages:
“Change tool and attach probe”
“remove probe, start spindle”
“Click continue when spindle is up to speed”
My question is:
Given that i am using the OneFinity Post processor I was wondering if that functionality was in there.
If not how can I accomplish that exact same workflow as in the video?
Greetings from the Netherlands
try this. select all your tool paths that you want in the file. do post process. Make sure your using onefinity/onefinity post configuration processor in the selection. then in the window on the right hand lower corner turn optional stop and preload tool to Yes. Make sure the Circular interpolation is set to yes as well. I did this and when I looked at the code it shows boths bits on top of the code file and where the seperation is for the two codes it has a Tool number value that is different ex. T20 for my 1/8" tool and T21 for my 1/4" tool. Check that out and do a floating test without cutting anything and see if it asks you to change the tool bit. also make sure any and all tools you have in your library are set up to manual change as well since you will still have to manually change then unless you have a spindle that uses multiple bit changes. Hope this helps.
that is very detailled, thank you for that.
So, when I use multiple tools I should be getting multiple “T” codes?
and the machine comes up with the messages like “change tool” ?
Yes you should get this or the router will pause so you can turn the router off. change bits. reset your z height. and then hit Play. Check out my youtube page FL DESIGNSLLC. I will be posting a video showing these settings.
Watch this video to see how to do multiple post processing files into one g-code with the Onefinity CNC with multiple bits and be able to change your bits and continue cutting with out having to load multiple g-code files. Hope you enjoy.
How are you probing while the program is paused?
Oke, i made a small file in Fusion360 with multiple tools. I did everything in the video above but I only get one T-number
can someone look at my file and tell me what I am doing wrong
test.nc (150.8 KB)
The T# designation comes from the tool setup in fusion - in the tool itself you can designate the number. If you’ve copied or duplicated the same tool multiple times they will have the same number, you can change them if you like, This is mostly important when using a automatic tool changer, for the Onefinity with manual tool changes you’re the one in charge of what tool gets loaded.
Good but not good enough, I did what Derek told me and ran everything again but still no multiple T codes.
Does your 2d contour toolpath use the same tool?
One other thing to look at - when you select the tools from your library Fusion will create copies or references to them in the specific “document” folder - are the tool numbers unique there as well?
With the settings you have there you will have different T# in the output file, I think your question is something different - are you looking for it to probe when you change the tool?
if you right click on your “Setup1” and select “Create NC Program” Make sure “Output M6” is checked
And then on the “Operations” tab make sure all 4 toolpaths are checked
That should create one file with multiple tools in it
problem solved I now have 3 Toolpaths in my .nc file
thanks a lot
greetings from The Netherlands
It is my belief that a limitation of Fusion 360 (free) personal use copy is that it only allows one tool path per post processing file. A tool change is allowed but not continuing on from a 2D adaptive path and a Contour tool path in the same file. For that I believe we have to pay the big money version. But I’m not certain that there aren’t any work arounds. Like combining two files with an editor like Visual studio and some knowledge of NC code.
You can have as many toolpaths in one post file as you want, as long as they use the same tool. I just finished one of my Z assembly plates that has 2D adaptive, 2D contour, and boring all with a 3 mm O flute. The chamfer operation with a 90 degree endmill required a second post file, because you can’t have a tool change in one post. They removed that from the free version quite a while ago unfortunately.
AH! So right you are, I guess if I would read the Error MSG more carefully ,