More efficient way to update my tool info after replacing a tool

I am looking for a way to more efficiently update my tools in Fusion 360.

Whenever I need to replace a tool on my CNC I update the new info in Fusion 360 for that tool ( for example if I had a 1/4 inch end mill that breaks I find that in my list of tools in Fusion and update the new tool length & tool diameter since the diameter is always slightly different depending on the brand of end mill )

But then I have to go through each one of my drawings that use that tool and manually select the tool from my library and select that updated tool so that it updates all of my tool paths.

This is extremely time consuming.

Is there a quicker way to update my tool paths with this new tool info whenever I need to replace a tool if it breaks or is worn?

What would be really nice is if there would be an option to force it to go out and get all of the current tool data from the library. ( In other words a one click option, verses having to go through each one of the tool paths that use that particular tool so that it gets updated with current tool info )

Just to confirm, I have my tool library on the cloud

Thank You...

Kent

Hi Kent. Mate how much difference do you find between tool diameters? I've never measured mine and they range from $60 to $2

I always thought there was a "tool wear" setting in the CAM for that but don't think that will fix your problem.

Sent from my SM-N970F using Tapatalk

I have seen the common carbide 1/4 x 1'', 2 flute cutters run from 0.239'' to 0.2495'', so yes, this is pretty common.

Most CNC programs have tool offset tables that are job specific or at least are global to be able to set diameter and length of a given tool. This is something that would normally be done when setting up the job at the machine. Having said that, I have Fusion 360 on or at all of my machines and find it easier to post a new G-code file when setting up the job for diameter compensation, height comp is always set in the machine tool table when setting up the job. Under no condition would I go through all of my job files that use a particular cutter and make changes on a tool replacement.

Wow that's over 10thou. That's huge.

Sent from my SM-N970F using Tapatalk

When I get a new replacement bit and find the diameter to be different than the one it's replacing I copy the previous and give the new one a different number. I use 1/4" compression bits for a lot of my work and have found them to be 0.245" but one was 0.247" so they have different numbers in the tool library. That way if I buy a new bit and it measures 0.247" then it gets one number but if it measures 0.245" then it gets another number (most have been 0.245").

If I need to use a file for which I already have G-code but the new bit is a different size then I edit the toolpath to include the new bit and generate new G-code. My naming convention includes the bit diameter so it's easy to see which bit this file is designed to use.

Naming convention - File number is always 00x in order of use - Name of project - zt is zero off the top, zs is zero off spoilboard - toolpath function - tooling (90 bit is a 90° V-bit, 0.123 is a 1/8" downcut bit, 0.25 down bit is a downcut 1/4" bit, 0.245 bit is the 1/4" compression bit, etc.)
Attachment 460494
Attachment 460496

David

Use G41/G42, and you don't have to worry about it. Just update the size in the control.