Changing tool diameter in library doesn't change the Gcode until...

[ovisopa]

I milled again a part I did in the past, 4 more times, but this time I need to make 2 and as I have a stock piece that perfectly fits 2 parts I copied my model and add the contours to existing operations.

 

What I noticed now, and didn't in the past models I milled, is that one internal contour is larger than it should be, I noticed first time when milling the interior chamfer, I didn't heard the tool touching the material, when it was finished I noticed there was no chamfer.

I flipped the part to Side B and milled the same contour and another larger one. when I removed the part from vise I noticed the contour on the bottom was smaller than the one I made from Side A. I measured the one on Side A and indeed it was larger than it should be, than I tried to find the issue, when I edited the operation I noticed  the Tool #6 is 1mm diameter - I know for sure it was defined as 1.58mm.

I think Fusion is caching the tool diameter for each milling operation, instead of using the diameter set in TOOL LIBRARY, and if any change is made in the tool library, the settings are NOT applied until I select again the same tool, in my case it was tool #6, so until I click SELECT and chose again the same tool #6, I could still see the tool defined as 1mm when editing that specific operation.

Is this behavior normal ? Shouldn't Fusion fetch the diameter from the tool library when generating a new GCODE file?

I know it's not a good habit to use the same tool number for a different tool, but I only did it once, when I broke the 1mm endmill, I placed this 1/16" endmill in the same collet and set the new dimensions both in Fusion and in PathPilot, usually I define as a new tool .. but when I broke the 1mm tool, now a few weeks ago I didn't do that 😞

With the new models I made those weeks I didn't had this issue as I started with a new file every time, but in this case, I opened the model I created about a month ago and modified it to mill 2 parts in the same time.

 PS. in the file attached, the operation named "2D interior Contour MUCH FASTER from 14min to 4min" in the first setup (the only operation not suppressed) is one that I did not modified yet, I will chose again the tool now to generate the correct toolpath this time, I will make the parts again now.

[Stuart-H · Accepted solution]

I think that f360 gets its tool info from the document section of the tool library when that tool is used in the cam for that design not from the actual libray

if you edit a tool in the document section it will not update the main library 

so in short you use a tool in your design and that info is in that designs document section

thats where subsequent info for that tool is gathered 

BTW it's caught me in the past ☹️

[ovisopa]

I just tried to look for the "Document library", I never select the tools from that tab as I don't like how "confusing" / annoying tools look in the document library, I'm always selecting the tools from my Cloud library, maybe this is why I get so many duplicates in the document library ?

In the document library you can see the first tool #6 is a 1mm endmill, all the others #6 are 1.58mm, to me the document library looks like a mess - I don;t understand why it duplicates the tool so many times .. anyway, probably this is the case with my issue. 

Is there a way to deactivate the document library and always use the tools from my main / default library ? (if there is a way to make a library, the default one)

[Stuart-H]

I think what's happening in your case but I may be wrong

is that the document lists all the tools that you have used in that design ( which is correct ) but you may have tried a number of different tools to try your tool paths but they are retained in that library 

as to tool 6 have you edited that tool in the doc lib. If so that's the reason for the difference between them and the main library 

that my take on it as as I said it's bit me in the past 

what gets my goat is that you cannot export the lib. To a excel/numbers file to keep the mill library in step but the only way I have is to print screen it 

as I use the gauge length of machine measurement it would help no end

hope someone else may pop in with further information 

[mill-art]

Fusion is working the way it is supposed to.  If you modify a tool from within the op then it modifies it for THAT op only.  If you use the manage tools outside of an op and modify the tool in your file (not saved library.) it see's that you have multiple ops in the setup running that tool and it will ask you if you want to change it for all ops.  That is how you modify it for all ops.    This is designed this way as you may run an adaptive clear for instance with roughing speeds and feeds leaving .02 on the floor.  Next you want to run a finishing op using adaptive clear again only this time you want to reduce your feed while leaving the RPM's high for a better finish.  Rather than modifying all the ops with these feed and speed settings it only modifies it for the op.  If you want to modify a tool.  If you want to permanently modify a tool you should only modify the tool outside of the OP in the manage tools and make sure to duplicate those modification in both your saved tool library and your open drawing file list.

[ovisopa]

@mill-art I had issues only regarding the diameter of the tool, and you can't change the diameter within the op, as I know, you only can change the feed and speed, which is ok and I understand the use of those settings.

It most probably was the document library that still had tool #6 defined as 1mm, as you can see in the screenshot above the first #6 tool is 1mm diameter, this was weeks ago when I was just starting up to mill my first steel parts, than changed the tool with a 1.58mm but keep the same number, this was my mistake - I think because Fusion has this dual-library (document vs main tool library) it's better to always give new tools, new numbers, and not modify tool #6 with another diameter tool, because it will happen the same thing, when generating the gcode from a previous made program, it will generate it using the diameter I had set before, it will not fetch the diameter from the main library, also there is not even a warning letting you know that tool #6 has different diameters in the same program, In my case I had on two operations the tool #6 selected from main library and one operation had the tool #6 selected from the document library (I haven't edited this op)

[Stuart-H]

Thanks for your reply your explanation fits with my findings

and a big round of applause for your admission it takes a big man to do that ,most do not even post back with that info.

with the tool library I think it's "caveat emptor "

i am a a bit OCD with my tool lib and maintain one for aluminium and one for steel ( they are different cutter anyway)

so its steel numbers start at 1 aluminium starts at 30. Drills at 60 and so on, keeps it in order and my brain cell 😀

Glad you have it under control

[ovisopa]

I will definitely create a different cloud libraries for aluminum vs steel , so far I only milled steel on the new mill.

And about numbering on the mill I haven't used any order, yet, just for the drills I copied the method I used to number my endmills and drills on the router, tool #133 is a 3.3mm drill, #145 is 4.5mm drill, I ll see maybe I will change this to have the drills starting at 1 or #10 for 1mm drill, and use the higher numbers for endmills, as anyway I won't have every drill bit mounted in a different holder, I have 3 holders for drill bits, I will buy more, but I'm sure I can work quite good with about 6 - 8 drill holders, so far I used 4 drills, and have the most used 3 drills, measured and saved in the tool library. For endmills is a different story, so far I have ~21 tool holders but I definitely want more .. like double 😄 Now all the tool holders are occupied by a tool, in the next months I will purchase more holders but for now I try to make some money first as the investment was quite high.

[mill-art]

@ovisopa- You actually can change it in the op.  If you edit the op and then click the select tool it opens the library where you can edit your tool's diameter and other measurements which is what I was referring too.   Otherwise from just within the op you can only modify the feed/speed for both cutting and non cutting tool paths.  Anyway glad you figured it out.